Lathe Manual

Lathe Module GibbsCAM 2009, v9.0 version 1.1, February 2009

Proprietary Notice This document contains propriety information of Gibbs and Associates and is to be used only pursuant to and in conjunction with the license granted to the licensee with respect to the accompanying Gibbs and Associates licensed software. Except as expressly permitted in the license, no part of this document may be reproduced, transmitted, transcribed, stored in a retrieval system, or translated into any language or computer language, in any form or by any means, electronic, magnetic, optical, chemical, manual or otherwise, without the prior expressed written permission from Gibbs and Associates or a duly authorized representative thereof.

It is strongly advised that users carefully review the license in order to understand the rights and obligations related to this licensed software and the accompanying documentation.

Use of the computer software and the user documentation has been provided pursuant to a Gibbs and Associates licensing agreement. © 1996-2009 Gibbs and Associates, a Cimatron® Company. All rights reserved. The Gibbs logo, GibbsCAM, GibbsCAM logo, Virtual Gibbs, Gibbs SFP, MTM, SolidSurfacer, and “Powerfully Simple.

Simply Powerful.” are either trademark(s) or registered trademark(s) of Gibbs and Associates in the United States and/or other countries. Windows Vista and the Windows logo are trademarks or registered trademarks of Microsoft Corporation in the United States and/or other countries. All other brand or product names are trademarks or registered trademarks of their respective owners.

Contains Autodesk® RealDWG by Autodesk, Inc., Copyright © 1998-2008 Autodesk, Inc. All rights reserved.

Gibbs and Associates 323 Science Drive Moorpark, CA 93021

Modif ied: February 10, 2009 10:37 pm

Table of Contents

Table of Contents INTRODUCTION TO LATHE

1

How to Learn the System . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .3 Help Systems . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .3 Text Conventions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .3

PART SET-UP

5

Document Dialog. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7 Part Details. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8 Machine and Stock Details . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8

TOOL CREATION

11

Tool Creation Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13 Lathe Tool dialog . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14 Tool Type . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14 Insert Types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14 Insert Specifications . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15 Insert Orientation Diagram . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18 Tool Holder Definition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18 Tool Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18 Turret Shift. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19 Tool Offset . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20 Cutter Radius Compensation (CRC) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20 Tool List Summary. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21

MACHINING

23

Machining Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .25 Creating an Operation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .25 Multiple Tool Dragging . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26 What is a Cut Shape?. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26 Multiple Process Programming . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26 Modifying an Operation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26 Machining Palette . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27

PROCESSES

29

Process Dialogs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31 Contour Process. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31 Contour Cut Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31 Contour Entry and Exit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .32 Contour Style. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 34 Rough Process . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36 Roughing Cut Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36 Rough Type . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .37 Clearance Diagram . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 38 Rough Style . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39 Stock Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40 i

Table of Contents

Roughing Feeds and Speeds . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40 Coolant . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40 Cut Direction Axes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .41 Thread Process . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42 Thread Cut Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42 Thread Definition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42 Thread Depth of Cut . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 43 Thread Clearance Diagram. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44 Thread Machining Parameters. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44 Holes Process . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44 Holes Entry/Exit Cycle . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44 Holes Drilling Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 45 Holes Clearance/Drill Diagram . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 45 Holes Machining Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 46 Threading . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47 Thread Dimensions - Defining the kind of thread to cut . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47 Cut Information - Defining how to cut the thread. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47 Depth Of Cut . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 48 Thread Location - Defining where to cut the thread . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 48 Cutting standard NPT Pipe Threads . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 49 2.5" - 8 NPT External Pipe Thread . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 49 2.5" - 8 NPT Internal Pipe Thread . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50 American National Standard Taper Pipe Thread (NPT) Chart . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50 Pre-Defined Process Groups . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 52

OPERATIONS

53

Clearance Moves. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 Auto Clearance. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 Fixed Clearance . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 Clearance Diagrams. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 56 Approaches from Tool Change Position . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 57 Exits To Tool Change Position . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 58 Same Tool Positions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59 Canned Cycles. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 61 Machining Markers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 62 How Machining Markers Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 62 Start and End Points . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 62 Selected Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 63 Using The Profiler . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 63 Material Database . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64 Operation Tiles. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 65 Touch-Off Point Information . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69

CUT PART RENDERING

71

Cut Part Rendering Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 73 Comparing Standard and Flash CPR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 73 Rendering Palette . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 74 Cut Part Rendering context menu . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75 Optional Stop control . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75 Current Display Options. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75 Fast Update. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75 ii

Table of Contents

Flash Cut Part Rendering . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Flash CPR Context Menu . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Flash CPR/Simulation Settings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Printing the Cut Part Rendered Image . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

POST PROCESSING

81

Post Processing Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Post Processor Dialog . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Posted Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Post Output Preferences. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Lathe Post Label Definitions and Code Issues . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2-Axis Lathe . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Label Definitions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Code Issues: . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3 & 4-Axis Mill/Turn . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Label Definitions: . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Code Issues: . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

COMMUNICATIONS

77 77 79 80

83 83 84 85 85 85 85 86 86 86 87

89

About Communications . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 91 Protocols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 91 Adding a Protocol . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 91 Changing a Protocol . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 92 Removing a Protocol . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 92 Communicating with a CNC Machine. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 92 Communications Dialog . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 92 Sending a File to the Control . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 92 Sending Other .NCF Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 93 Receiving a File from the Control . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 93

LATHE TUTORIAL

95

Exercise #1: Lathe Tutorial . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97 This tutorial explains how to:. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97 Part Setup. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97 Custom Stock. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 99 Tool List . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 101 Creating the Operations - OD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .106 Creating Operations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .109 Multiple Process Group Op 2-4 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 110 Multiple Process Group Op 5-8 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 116 Creating the Operations - ID . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 120 Multiple Process Group Op 9-11 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 120 Threading . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 123 Op 12. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 123 Cut Off . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 124 Op 13. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 124 Post Processing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 126 Exercise #2: Form Tools . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 128 Form Tool Contour . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 129 iii

Table of Contents

PART PRINTS

133

INDEX

137

iv

INTRODUCTION TO LATHE

Introduction to Lathe

CHAPTER 1 : Introduction to Lathe HOW TO LEARN THE SYSTEM Congratulations on your purchase of the most productive programming system available! The most effective way to learn the system is to look through the Getting Started Guide to become familiar with the system and how it works. After going through Getting Started you should complete the exercises in the Geometry Creation manual followed by the tutorials contained in this manual. For simple explanations of on-screen items and their purpose, use Balloons and Prompting provided in the Help menu. The Common Reference Guide will help you with items contained in the menu bar.

This manual is intended for users of a basic 2-Axis Lathe; however, the lessons learned are applied across more advanced C-Axis and Multi-Task Machines. This manual covers information specif ic to Lathe machines; however, most of the interface concepts are similar to other types of machining. After elaborating the concepts of creating geometry, this manual proceeds with information on part set-up, tools, toolpath generation, Posting and communications with a CNC.

HELP SYSTEMS Online Help, Balloons and Prompting are built-in documentation and training information, also known as C.A.T. (Computer Aided Training). They are accessed from the Help menu or with a shortcut key (Ctrl+B).

They provide reference information, rules, and assistance in using the system. For more detailed information on Balloons and Prompting, see the Common Reference guide.

TEXT CONVENTIONS In this and all other GibbsCAM manuals you will f ind a number of standards used in the text, known as conventions.

Screen text: Any text you see like this is referring to text you will see in GibbsCAM or on your monitor.

Typically this is a button or text for a dialog.

Keystrokes: Words that appear like this refer to a keystroke or mouse action, such as right-click or Ctrl+C. Term: Words that appear like this followed by a colon refer to a word or phrase used in GibbsCAM.

3

Introduction to Lathe

4

PART SET-UP

Part Set-Up

CHAPTER 2 : Part Set-Up DOCUMENT DIALOG Clicking on the Document button will bring up the Document dialog. This dialog is actually a combination of two linked dialogs. The top dialog contains general information about the part such as the Machine and Material information. In addition, the top dialog provides f ile management options which give the user control over where the f ile is stored on the computer. The bottom dialog provides specif ic information about the part such as stock size, clearance moves and Tool Change positioning.

1.

2.

3.

4.

Machine list Part Material File Control Measurement Units

Top section of the Document Control dialog, the Part Details.

5.

6.

7.

8.

Stock Size diagram X Dimension Style Auto Clearance Option Fixed Clearance Positions 9. Tool Change Position 10. Lathe Shank Size 11. Mill Tool Holder Class 12. Part Comment

Bottom section of the Document Control dialog, the Machine and Stock Details.

7

Part Set-Up

PART DETAILS This part of the dialog contains a part’s basic parameters including the type of machine to be used, the material the part is made of, whether the part is metric or imperial. This section of the dialog also contains commands for opening, closing and saving part f iles.

File Control: The buttons used for f ile management described below are also available under the File menu.

Open (Ctrl-O) : Clicking on the Open button will bring up the Open dialog which allows the user to select which f ile to open. If a f ile is currently open, it will be closed and the selected f ile will be opened.

New (Ctrl-N) : This button will create a new f ile by opening a dialog and asking for a f ile name and a location to save the new f ile. If there is a f ile open, it will be closed.

Save (Ctrl-S) : If there have been any changes made while the f ile was open, this button will save the changes.

Save As : This button will open a dialog asking for a f ile name and a location to save the current f ile. The changes made since the last Save command will be written into the new f ile. The original f ile will not be affected. The new f ile will become the current, open f ile.

Save Copy : This button is very similar to the Save As button. The system will create a duplicate copy of the open f ile. The original f ile remains the current, open f ile. The name of the duplicate f ile can be changed.

Close : This button closes the current f ile. If the f ile has not been saved before clicking on the Close button, a dialog will come up asking if the f ile should be saved.

Machine list: Clicking on the Machine pop-up menu will produce a list of all machines the software is set up to handle. A copy of the Machine Type selection is stored with the part f ile. Thus, if you have a custom MDD (machine type f ile) you may easily transfer the part f ile to another system. If the Mill, Advanced CS or MultiTask Machining modules have been installed, there will be additional choices.

Part Material: The information in this box is used to specify the material of the part. This will help in the calculation of feeds and speeds for the machining processes. The calculations will come from either the CutDATA Material Database (which is an option that can be purchased with the system) or from the default material database. A custom material database can also be created. Refer to the “Material Database” section in the Common Reference Guide for more information.

Measurement Units: These two radio buttons determine whether values input will be based on an English or metric standard and entered in inches or millimeters. The measurement type used to generate the posted output is determined by the post processor itself. There are English and metric post processors. If an English post is used on a metric part, the posted numbers will be converted from millimeters to inches. Likewise, metric posts will convert values from inches to millimeters.

MACHINE AND STOCK DETAILS The bottom section of the Document dialog is specif ic to the type of part being made. This section of the dialog will change to reflect the part def inition requirements as different machine types are selected. Thus, a horizontal or vertical turning part’s setup is different from a 3-axis mill part which is different from a 4-axis mill part which is different from a Multi-Task Machining part. In this manual we will strictly concern ourselves with the turning settings.

8

Part Set-Up

Stock Size diagram: This section of the dialog is used to specify the starting size of the part stock. The stock size entered here will be used by the system to determine positioning moves when using the Auto Clearance function. The stock dimensions will also be taken into account when generating toolpaths with the Material Only option selected in the Process dialog. If custom stock has been created, the system will use the custom stock size for toolpath and positioning moves. In that case, the values entered here will only be used to draw the stock outline and origin marker correctly. The text box for the X dimension will be a radius or diameter value depending on which option is selected for the X Dimension Style.

1. Part Diameter 2. Stock +Z dimension (past origin) 3. Stock –Z dimension (behind origin)

X Dimension Style: These two radio buttons determine whether the X values for the part are input as radii or diameters. Some text boxes in particular dialogs specify that the value entered is either a radius or a diameter value, regardless of the selection made here.

Tool Change Position: If the Tool Change option is turned “on” the turret will be sent to the X and Z dimensions specif ied when a tool change occurs. If Tool Change is not on, it is assumed that either f ixture offsets are being used or the operator will hand input the tool change moves.

Recommendations: Having Tool Change enabled is best for newer machines which use generic offsets or Work Fixture Offsets. Having Tool Change off is best used with older machines which use G50 offsets.

Auto Clearance Option: When the Auto Clearance option is turned on, the system will calculate positioning moves between operations. These positions will be dynamically calculated, meaning that they will change as the material conditions of the part change. The value entered is an offset amount from the current part stock that the system will use to maintain adequate clearance from the material. Refer to “Clearance Moves” on page 55 for more information.

Fixed Clearance Positions: Fixed Clearance positions must be entered when the Auto Clearance option is turned off. When the Auto Clearance option is on, the f ixed clearance position text boxes will be grayed out. The X and Z values entered specify the location the tool will rapid to and from during a tool change. This position will also be used when moving from one approach type to another. Refer to “Clearance Moves” on page 55 for more information.

Holders: The items here describe the size or class of the tool holders found on the current machine.

Lathe Shank Size: This is the shank size of lathe tool holders for the current machine. This setting controls what tool holders are actually available when def ining tools.

Mill Tool Holder Class: This is the class or standard size of the mill tool holder on the current machine.

Part Comment: Any text entered as a part comment will be shown in the part preview section of the Open dialog and in the posted output.

9

Part Set-Up

10

TOOL CREATION

Tool Creation

CHAPTER 3 : Tool Creation TOOL CREATION OVERVIEW The tools button in the main palette will open the Tool List. The Tool List can hold up to 999 tools in a part f ile. To create a tool double-click on an empty tile location to open a Tool Creation dialog. This dialog is used to create and modify tools. Once the tool information has been entered and the dialog closed, a Tool Tile will be created in the Tool List which displays the tool type and insert width. To index through the various tools that have been created, click on the scroll arrows located at the top and bottom of the Tool List.

Tools can be reorganized in the list at any time, even after operations have been created, without reprocessing the operations. To reorganize the order of tools, click once on the Tool Tile to be moved and drag it to an insertion point. The system will automatically adjust the operations to reflect the change in tool order and number. For more information on Tile Lists, refer to the Getting Started Guide.

Tool specif ications can be modif ied at any point during part creation. However, if operations have been created using the tool, those operations must be reprocessed. To reprocess an operation, double-click on the Operation Tile in the Operation List and click on the Redo button. The new tool specif ications will be incorporated into the operation toolpath.

13

Tool Creation

LATHE TOOL DIALOG In order to def ine lathe tools a Lathe machine type must be selected in the Document dialog. The basic turning tools are created using the Tool Creation dialog shown below. Each of the items contained in the dialog is described in the following section.

1.

2.

3.

4.

5.

6.

7.

Tool Type Insert Types Insert Specifications Insert Orientation Diagram Tool Holder Definition Tool Options Turret Shift

TOOL TYPE This button is used to toggle between mill tools and lathe inserts. Mill tools should only be used with the face drilling function unless you have the Mill/Turn or Multi-Task Machining module(s) installed.

INSERT TYPES This area is used to select the type of insert used with the tool holder. The Insert Specs will change depending on the selected insert. Below is a list of Insert Types with each type’s available specif ications. In many cases, checking Other brings up different options. The alternate options are listed after Other and any additional modif ications are noted. See the Insert Specif ications section for a detailed description of each option.

80° Diamond Insert (80° C): Tip Radius, Inscribed Diameter, Thickness, Other 55° Diamond Insert (55° D): Tip Radius, Inscribed Diameter, Thickness, Other 14

Tool Creation

35° Diamond Insert (35° V): Tip Radius, Inscribed Diameter, Thickness, Other Round Insert (rnd. R): Tip Radius, Thickness, Included Angle, Other Square Insert (sqr. S): Tip Radius, Inscribed Diameter, Thickness, Other Triangle Insert (tri. T): Tip Radius, Inscribed Diameter, Thickness, Other Trigon Insert (tgn. W): Tip Radius, Inscribed Diameter, Thickness, Other Pentagon Insert (pent. P): Tip Radius, Inscribed Diameter, Thickness, Other 55° Parallelogram (55° K): Tip Radius, Width, Thickness, Other, Length Rectangle (rect. L): Tip Radius, Size, Thickness, Other, checking Other replaces Size with insert Length(L) and Width(W) Grooving Insert (groove): Tip Width, Tip Radius, Insert Width, Full Radius, Deflection Compensation, Other, checking Other replaces Full Radius with Length Cut Off Insert (cut off): Tip Width, Tip Radius, Face Angle, Other, Length Groove Style Threading Insert (thd. N): Style, TPI, Insert Width, Insert Type, Other, checking Other removes the TPI option and replaces Insert Type with Length Lay Down Style Threading Insert (thd. LT): Style, TPI, IC 35° Profiling Groove Style Insert (35° VN): Tip Radius, Width, Thickness, Other, Length Form: Thickness, Entry/Exit Angle (Please see the FormTool section for additional data)

INSERT SPECIFICATIONS This information will change depending on the currently selected insert type. Each of the pop-up menus will limit the selections available in the pop-up menus that follow it. For example, selecting a Tip Radius will limit the number of available Inscribed Circles and Thicknesses. Selecting an IC will further limit the number of Thicknesses available. These settings will limit the number of available tool holders and boring bars in the holder diagram. If no tool holders or boring bars are available, the None choice will be automatically selected.

15

Tool Creation

When the Other checkbox is checked, the user can enter any tool specif ications they wish. When Other is selected, the holder diagram is automatically set to None.

1.

2.

3.

4.

5.

6.

Tip Length Tip Width Tip Radius Insert Width Face Angle Inscribed Diameter

Diameter Relief: The angle the tip is approaching, changing affects the Face Relief.

Entry/Exit Angle: The angle used for plunging into and retracting out of material before and after cutting.

Face Angle: The angle of the insert’s cutting face.

Face Relief: The angle of the insert’s approach, changing affects the Diameter Relief.

Full Radius: When enabled, this option will limit the grooving inserts available to only those with a full radius tip.

IC: The inscribed circumference of the insert, effectively the size of the insert.

Included Angle: Used to def ine the touch off point and automatically calculate the Face Relief and Diameter Relief settings for Round inserts.

Inscribed Diameter: The inscribed circle of the insert.

Insert Type: The type of insert.

Insert Width: The width of the insert.

Length: The length of the insert.

Other: If this item is on, the insert specs will switch from pop-up menus to text boxes. Any value can be entered in the text boxes. The type of tool holder will automatically be set to None (although there might be tool holder or boring bar selections available).

Size: The IC size of the rectangle. If the Other button is turned on with this type of insert, the length and width of the insert need to be entered instead of the size.

Thickness: The thickness of the insert.

16

Tool Creation

Tip Radius: The tip radius of the insert.

Tip Width: The width of the tip of the insert.

TPI: The threads per inch that the blueprint calls for.

Style: The thread style of the insert.

Width: The width of the insert. This is utilized when the tip width and the insert width would be the same measurement.

FormTool: The system supports custom form tools for Lathe parts. Unlike Mill parts, Lathe form tools must be a closed shape. Be sure to create the shape with the part origin in mind. The origin is used as the touch-off point for the tool. All posted output with this tool is relative to this point. The Touch-off point is shown as a red cross in the tool diagram.

The Steps To Make a Form Tool: 1.

Create the prof ile geometry, taking into account the touch-off point.

2. Select the geometry (double click it).

3. Create a new tool, designate it as a Form Tool.

4. Click on the Apply button.

17

Tool Creation

INSERT ORIENTATION DIAGRAM This diagram is used to specify the orientation of the insert in the tool holder or boring bar.

Changing the information will not affect the availability of other items in the dialog, but it will change the orientation of the drawing in the Holder diagram.

TOOL HOLDER DEFINITION Tool Holder: This option will display the tool holders available for the specif ied insert type and size, as well as for the machine’s shank size.

Boring Bar: This option will display the Boring Bars available for the specif ied insert type and size. All shank sizes will be displayed.

Custom Holder Definition: This option is only recommended if you need to create a custom holder shape. Holders can be def ined by a geometry prof ile (similar to creating a custom tool shape), by a solid model of the holder or by numeric values (Custom). By default the holder is set to None, meaning a holder will not be used. To use a geometry shape, select the geometry, select Profile and click OK. To use a solid model, select the solid, select the Solid option and click OK. The Apply To All Selected Tools option will apply the current tool holder def inition to all the tool tiles currently selected. The Show Solid option will show the solid model that is currently set to be the holder. Clicking the Make Profile button will create a geometry prof ile from the Custom tool holder def inition.

None: If None is selected, the insert will be drawn without a holder. This is automatically selected if there are no tool holders or boring bars available in the database for the selected insert. The face and diameter relief angles must be entered. The cross hair marker indicates the Touch-off point of the insert. The radio buttons below the holder diagram designate whether the holder will be shown at its actual size, or at a calculated size that is scaled to f it in the diagram.

Tool Diagram: The tool diagram provides information about the touch off and type of holder or boring bar that will be used for the insert. The None choice is used for holders not in the software’s database. Use the scroll bar to scroll through the list of available holders. The holder selection is used to determine the diameter relief and face relief angles. The red circle on the insert shows the location of the Touch-off point. The radio buttons below the holder diagram designate whether the holder will be shown at its actual size, or at a calculated size that is scaled to f it in the box.

Holder Specs: Detailed information appears to the right of the diagram displaying the holder data.

TOOL OPTIONS

Forward/Reverse : Forward will turn the spindle in the forward or normal direction. Selecting Reverse will reverse the spindle.

Offset #: Normally, the offset number of the tool is determined by its location in the Tool List. This box allows the user to override that default with a different number.

18

Tool Creation

Deflection Compensation: If this option is turned on, all contour and rough toolpaths generated with this tool will contain deflection tool offset utility markers at every location in the toolpath where deflection occurs.

This will allow the user to f ine tune the deflection compensation that occurs while using this particular groove tool.

Offset #: When Deflection Compensation is used, this is the offset that we will switch to at the end of the stroke.

Tool ID #: Enter the tool ID you wish to use instead of the tool list position.

Insert Material : This is a pop-up menu used to specify the material of the tool. The information given here is used by the Material Database as another factor in determining speeds and feeds. The default setting for Lathe parts is Carbide Insert, Coated.

Notch Ramp: By selecting a notch ramp amount in a Tool Dialog, the toolpath will be created by adding the ramp value to alternating strokes: one with, one without. In Roughing Operations, this will reduce the depth of cut on one stroke and increase it on the next. Please ensure that the ramp value is smaller than the depth of cut. (Notch Ramp is not available for Groove, Cut Off or Thread tools.)

Comment : This is a comment associated with the tool. It will be output in the f inished code at the beginning of every operation that uses this tool.

TURRET SHIFT This enables a Turret Shift (see below). It is used to specify the preset point for the tool. It can also be used to set up different tool change positions for each tool.

1. Default Tool Change 2. Preset Point 3. Turret Shift

Default Tool Change: This is a reference to the setting in the Document Control Dialog.

Preset Point: This information is only required on some older machines. The two boxes are for entering the Xr and Z distances from the preset point to the default tool change position. They are absolute values. These vales are unique to each tool This function is useful for pre-programming G50 offsets in the off ice using GibbsCAM rather than on the floor.

Turret Shift Dialog: This dialog is used to specify the distance from the preset point (also known as the Touchoff point or the theoretical tip of the tool) of the tool to the center of the turret. It can also be used to specify a different tool change position for the tool.

19

Tool Creation

TOOL OFFSET When roughing or contouring, the system calculates a tool offset amount based on the tip radius of the insert.

This is the amount the f inishing pass of the toolpath (the only pass if contouring) will be offset from the selected part geometry. If a stock amount is entered for the process, that stock amount will be added to the tool radius offset.

CUTTER RADIUS COMPENSATION (CRC)

In the File > Preferences > Machining Prefs dialog there are options to control the CRC types for Milling and Turning ops. Tool Center is the recommended option because that is the method used by the system to display the toolpaths and cut part rendered images regardless of the setting of the Contour Cutter Comp, which only affects the posted output.

When the Tool Center item is selected, the numbers generated in the posted code will be the geometry offset by a tip radius (providing the Stock amount is 0). Tool Center is the recommended selection for this preference. When the Tool Edge item is selected, the numbers generated in the posted code will be the same as the blueprint numbers.

Roughing operations will always be calculated from the tool center. If the Tool Edge item is selected for this preference, CRC should be turned off in all roughing operations.

When using Tool Center, the offset in the CRC register at the control should be the difference between the tip radius of the actual insert used and the tip radius of the insert programmed in the system. If the inserts are identical, the CRC offset number should be zero. If the actual insert is smaller, a negative value can be used.

When using Tool Edge, the offset in the CRC register must be the full tool radius. Toolpath is to the tool edge, including tool geometry. You also need a post processor that supports Tool Edge output. If your post processor is incompatible, the system will warn you if this incompatibility.

When using Finish Profile, the output path is the prof ile that follows the selected geometry. The CRC register must contain the full tool radius and any desired stock amount.

!

20

WARNING: The system does a much better job offsetting the tool than the majority of controls currently available. Regardless of the setting made in this preference, all toolpath drawing and cut part rendering will be calculated and displayed using the system’s offsetting mechanism. Therefore, it is possible for the cut part rendered image produced by the system to look good while the tool, cutting according to the posted code, will not cut well. If the control’s offsetting mechanism is less advanced than the system’s, it is possible that when the control produces the offset values, errors and interference will result.

Tool Creation

TOOL LIST SUMMARY Selecting Tool List Summary from the Window menu displays the Tool List Summary dialog which provides information in spreadsheet form about each tool contained in the Tool List. The information in the dialog can either be saved as a text f ile or printed out. To save the summary as a text f ile, select the Tool List Summary item from the Save Special submenu in the File menu. To print the summary, select the Tool List Summary item from the Print submenu in the File menu.

21

Tool Creation

22

MACHINING

Machining

CHAPTER 4 : Machining MACHINING OVERVIEW Clicking the Machining button will bring up the Process List, the Machining palette, and the Operation List. The Process List is used to create sets of operations to be performed on cut shapes. The Machining palette contains Function Tiles that when used in conjunction with Tool Tiles create Process Tiles.

The Process List is a “staging area” that is used to generate f inished operations which contain the toolpaths for cutting the part. When an operation is f inished and placed in the Operation List, the items in the Process List can be thrown away or reused with a different cut shape. The Operation List contains the completed operations that will be output during post processing.

CREATING AN OPERATION Each tile in the Process List will be applied to the selected geometry. A Process Tile is created by dragging a Function Tile from the Machining palette and a Tool Tile from the Tool List to the same location in the Process List. They can be dragged in any order. When a Process Tile is complete, a Process dialog specif ic to the chosen machining function will appear. This dialog contains detailed information about the way the operation’s toolpath will be created.

1. Tool List 2. Process List 3. CAM palette

To def ine multiple processes with the same machining type, hold down the ALT key and drag a machining tile over any selected process tile. This will apply the machining process to all selected tiles.

Contouring and roughing functions require that geometry be selected to act as the cut shape for the operation.

Machining Markers are used to select the portions of the geometry to be used as the cut shape when creating a toolpath. The markers will appear on the geometry when it is selected. If a drilling or threading function is being used, no geometry is required to create an operation.

25

Machining

After the information in the Process dialog has been entered, place the machining markers in the correct locations on the geometry. Machining Markers are not used for drilling and threading functions. Clicking on the Do It button will create an operation(s). The operation(s) will be placed in the Operation List. If any completed operations are selected (in yellow), the Redo button is available. If the Redo button is depressed, the selected operations will be replaced by the new operations. Clicking on an empty operation location or an insertion point between operation locations will deselect all the operations.

Operations contain the f inished toolpaths. A toolpath consists of the actual moves the tool will make. The toolpath is based on the cut shape. The data contained in the operation is what the post processor will use to make G-code.

MULTIPLE TOOL DRAGGING There are two behaviors to consider when dragging multiple tools. First, by selecting multiple tools (shift-click or CTRL-click) and dragging the group to the machining palette, the tools will f ill in wherever they are dropped. If there are machining tiles present, they will be populated. If the machining tiles are blank, the tools will populate wherever they are dropped (including between tiles if placed on an insert point.) If you hold down the ALT key when dropping tools on top of machining tiles, the tool (or tools) will populate all selected tiles.Holding down ALT and dragging also works to populate multiple tools with process tiles at once.

WHAT IS A CUT SHAPE? A cut shape is used to generate a toolpath. It is not drawn on the screen, but can be visualized as the f inished shape left after the removal of material by the toolpath. A cut shape (not the original geometry) is used to create a toolpath because programming the toolpath to the geometry as it is def ined on the blueprint will usually gouge the part. The software automatically generates the cut shape. Various specif ications and limitations are taken into consideration in the creation of the cut shape.

The machining markers (the start and end point and start and end feature markers) allow the user to specify the portion of geometry (or the entire shape) that will act as the initial outline of the cut shape. The system then takes into account the physical attributes of the tool being used in the process, such as insert type, tool holder, relief specs, etc. in order to prevent possible tool interference when applying the tool to the cut shape being machined. The cut shape is further governed by information entered in the Process dialog, such as Entry/Exit Radius, Stock Shape, Axes, etc. The system employs the concept of a cut shape so that it is not necessary to create different geometry for different operations in order to avoid gouging the part.

MULTIPLE PROCESS PROGRAMMING The Material Only option available in the Contouring and Roughing Process dialogs is particularly useful when doing multiple process programming. Material Only provides for “no air cutting.� When selected, the system optimizes the toolpaths created by only making feed moves where there is material that needs to be removed.

The system takes into account the material conditions in terms of what has already been cut in previous operations, including those contained in the same Process List.

MODIFYING AN OPERATION Double-clicking on an item in the Operation List will recreate all of the information in the Process List. It will also select the geometry and place the markers exactly as they were when the Do It button was pressed. Any operations that were created at the same time as the selected operation will become selected and their information will also be placed in the Process List. Click on the Redo button after the changes have been made.

This will replace all selected operations in the Operation List with the newly created operations.

26

Machining

MACHINING PALETTE Each tile in the Machining palette has a different function. The Contouring function is used for taking a single f inish pass. The Roughing function is used for taking multiple passes. The Threading function is used for making different types of threads. The Drilling function is used for drilling a hole at X = 0.

The order of machining in the f inished NC program is the same as in the Operation List. This means that the order of Operation Tiles in the Operation List is very important. Eff icient use of multiple process programming may produce operations in a less-than-optimal machining order. The Operation List can be organized as the part is being created or when all operations to cut the part have been completed. Clicking on the Sort Operations menu item from the op tile right mouse menu reorganizes the operations by tool number and creation order. Operations created in the same Process List will maintain their order to ensure that f inishing passes cannot be moved in front of roughing passes, etc. The Operation List can also be manually rearranged by moving tiles to different locations in the list.

While the Operation List can be reorganized to create a more optimal machining order, there are some other considerations. When using the Auto Clearance option and/or the Material Only option, the system takes into account the material conditions when it creates the positioning moves and toolpath for each operation.

Changing the order of operations has the potential to change the initial material conditions for existing operations. If the order of operations is changed or operations are added or removed from the list, the toolpaths and positioning moves should be checked. Rendering the part is a good way to check if changes need to be made to the tool moves due to tool interference or unnecessary incorrect positioning moves. If adjustments need to be made, the operations must be reprocessed. Reprocessing all operations in a part f ile is very easy using the Redo All Ops item under the Edit menu. When the operations are reprocessed, the system will recalculate all of the toolpaths and positioning moves based on the new order of operations.

27

Machining

28

PROCESSES

Processes

CHAPTER 5 : Processes PROCESS DIALOGS Process dialogs appear on the screen when a Function Tile from the Machining palette and a Tool Tile from the Tool List are placed in a Process List location. There are four types of Process dialogs that correspond with the four types of functions available in the Machining palette. The options available with each of these processes are described in this section.

CONTOUR PROCESS The Contour process is used to take a single pass along a shape. When a Contouring Function Tile is combined with a tile from the Tool List, the following Process dialog will appear.

1. Contour Cut Options 2. Contour Entry and Exit 3. Contour Style

Contour Cut Options Approach Type: This should be the f irst selection made in any Process dialog. The Approach Type selection designates the axis (Z or X) along which the tool will approach the part. The OD and Front ID options specify that the tool approach and retract along the X axis, while the Front Face option requires that the tool approach and retract along the Z axis. Also, selecting one of these radio buttons will change the Clearance Diagram that appears in the middle of the Process dialog.

Clearance Diagram: This picture will change depending on the Approach Type selection and on the Clearance selection made in the Document dialog. The Approach Type selection will change the axis of approach.

If Auto Clearance is selected in the Document dialog, the diagram will disable the clearance position values because they are calculated based on the Auto Clearance value.

31

Processes

Entry Clearance specif ies the diameter or radius location the tool will make a rapid move to before feeding to the operation start point. The Exit Clearance position specif ies the location the tool may rapid to after completing its toolpath for that operation. Both boxes are labeled with arrows going towards and away from the part, respectively.

Forward: This indicates the direction the tool will move along the designated cut shape. If the Forward option is selected, the tool will move from the start point to the end point of the selected cut shape as designated by the machining markers. Left unchecked, the tool will move from the end point to the start point of the selected cut shape.

Square Corners: This checkbox determines the external corner moves for a cut shape. When this option is turned on, the system does not add a radius move at the corners of the cut shape. Instead, the tool only makes sharp moves when going around a corner and will leave contact with the f inished shape, possibly creating a burr at the corner. If this option is not selected, the system automatically makes a radius move when rounding a corner so that the tool always stays in contact with the part.

No Drag: A checkbox that indicates how the contour will be cut. When this option is selected, the chosen cut shape is automatically broken up into segments that will be cut along the positive insert angle direction. All cutting will be “pushing” the insert, not “pulling” it.

Deflection Compensation (Groove Tool): By choosing a “No Drag” style toolpath you have the option to specify a deflection compensation amount.

The tool motion is modif ied whenever the deflection compensation is in effect. This will break a contour into (possibly) several toolpaths so that the insert is always cutting in a “forward” direction. This eliminates drag or cutting with the back side of the insert.

Cut Off: A checkbox for use with cut off tools. If the post processor has been appropriately customized, turning this option on will trigger the post processor to output any special codes necessary for removing a part from bar stock.

Contour Entry and Exit

The Entry and Exit options can create additional movements that will be added to the tool path. When the f irst option is selected, a 90° arc of the specif ied radius value will be added to the toolpath. This arc will be tangent to the start feature at the start point. If a value is entered in the Line text box, a line of the specif ied length will be created tangent to the arc. Also, if this is selected and the radius value is zero, the line will not be

32

Processes

perpendicular but instead will be parallel. When the second option is selected, a line of the specif ied length will be added to the cut shape. This line will be perpendicular to the start feature at the start point.

Selecting the Advanced option allows you to def ine custom Entry and Exit Moves using the Entry/Exit Tab. The options and behavior of these moves are similar to Mill entry/exit except that there are no Z Ramp moves for Lathe. You may def ine moves for Entry and Exit independently. Checking the Exit option enables the Exit moves, which can be set to the defaults or to advanced options.

Radius Entry/Exit: Select this option to base your entry/exit move on a radius.

CRC Line: This generates a line that allows Cutter Radius Compensation to activate. The CRC line can be tangent or perpendicular to the Off Part Line depending on your machining preferences.

Off Part Line: This is generated after the CRC line, and generates a line that feeds into (or off for exit) the part.

Entry/Exit Radius: This determines the radius of the entry/exit curve.

Off Part Dist: This determines how far the system should follow the radius of the entry/exit curve. If this value is equal to the entry/exit radius, a 90-degree curve will result.

Line Entry/Line Exit: Line entry or exit will be based on a custom angle. The entry/exit axis will be perpendicular to the feature.

33

Processes

Contour Style

The Contour Style selection affects the toolpaths created for the current operation. If the Material Only option is selected, the system takes into account the current stock conditions, including custom stock specif ications, when creating the toolpaths for an operation. When Material Only is on, the toolpath will only feed over areas that have not yet been machined in previous operations. The system keeps track of material removed in previous operations and generates the current toolpath based on that information, providing for “no air cutting.”

Because of this, the order of operations directly affects how the part will be cut. If the order of operations is changed or operations are added or removed, all operations should be reprocessed in order to account for the change. The Redo All Ops item in the Edit menu makes reprocessing all operations of a part very easy.

The Clearance value specif ies an offset amount from the material that the system uses to calculate where the tool can safely rapid during an operation. If the tool is within the clearance amount, only feed moves will be allowed.

The Full option gives the user more control over toolpath creation. When the Full option is selected, the toolpath generated will feed over the selected cut shape from the start point to the end point as designated by the machining markers.

Corner Break: The value entered in this text box specif ies a radius that will be put on every outside sharp corner of the selected cut shape. A value of zero will not break the corner, but will keep the tool in contact with the part as it moves to the next feature. Note that Corner Break is only available when Square Corners is not selected.

Fin. Stock ±: The Fin. Stock value specif ies the minimum amount of material that will be left on the cut shape (equally on all faces) after a toolpath is completed.

Xr Stock: The Xr Stock value allows the user to specify any additional stock amount for the X axis. The value entered here specif ies the amount of material that will be left on the cut shape along the X axis only.

Z Stock: The Z Stock value allows the user to specify a stock amount for the Z axis. The Z Stock value specif ies the amount of material that will be left on the cut shape along the Z axis only.

Cutter Radius Compensation On: A checkbox that indicates whether Cutter Radius Compensation is turned on or off. GibbsCAM has a number of rules for when and where it will generate CRC markers. These rules have been chosen so as to be as safe as possible for the widest range of machines. This means that while a specif ic machine may be able to handle different CRC rules, we will not generate markers for all cases by default. CRC rules on arcs are the primary example of this.

For new toolpaths, GibbsCAM will do the following: 1.

CRC will be activated on entry moves, before the entry arc. If there is no move before the entry arc, CRC will be activated on the arc. GibbsCAM has a warning that will tell the end user when they are using CRC without a line move. In general we consider CRC activation on an arc to be an invalid case, because it does not accurately cut the arc.

2. CRC will be activated on exit moves, after the exit arc. If there is no move after the exit arc, the CRC deactivation will be made on the Depth move. Again, GibbsCAM will warn when a user does not have a line move. In general we consider CRC deactivation on an arc to be an invalid case, because it does not accurately cut the arc.

34

Processes

3. Some Operations have the option of deferring CRC activation until later in the toolpath (roughing with a f inish pass.) Rules 1 and 2 will be applied to the f inish pass only.

For old Toolpaths, GibbsCAM will only follow rules 1 and 2. No markers will be added for rapids imbedded in the toolpath.

Coolant: A checkbox which indicates whether coolant is turned on in a process. Flood is the standard coolant option. Additional coolant options are available with custom post processors.

CSS (Constant Surface Speed): Selecting the CSS item will activate Constant Surface Speed (CSS). CSS will cause the spindle RPM to constantly change based on the diameter the tool is at and the SFPM used.

Max RPM: The Max RPM setting is used to set an upper safe limit on the spindle RPM. If CSS is off, the specif ied RPM value will be used for the spindle speed.

The SFPM and Feed values can be automatically calculated based on the material selected if the CutDATA Material database is installed. In order for these values to be calculated and entered in the appropriate boxes, the SFPM and Feed buttons must be clicked. If no material is selected or the CutDATA Material database is not installed, the user will need to manually enter values for the feed and speed.

Entry Feed: By clicking on the Entry Feed button, the software will calculate the value based on our materials database. Alternatively, you may manually override the calculated value by inputting your own value. The entry feedrate is written to the toolpath for output in G code.

Contour Feed: This will calculate the best feedrate based on the material type selected using CutDATA. Cut Direction Axes: The Cut Direction Axes checkboxes allow the user to regulate the axes and directions of the cut shape. Deselecting an axis will prevent cut shape moves in that axis direction. The default settings should have all axes selected.

35

Processes

ROUGH PROCESS Rough processes are used to take multiple passes on a shape. When the Rough function tile is combined with a Tool tile, the following Process dialog will appear.

1.

2.

3.

4.

5.

6.

7.

8.

Roughing Cut Options Rough Type Stock Options Roughing Feeds and Speeds Clearance Diagram Rough Style Coolant Cut Direction Axes

Roughing Cut Options Approach Type: The Approach Type selection designates the axis (Z or X) along which the tool will approach the part. The OD and Front ID options specify that the tool approach and retract along the X axis, while the Front Face option requires that the tool approach and retract along the Z axis. Also, selecting one of these radio buttons changes the Clearance Diagram that appears in the right-hand corner of the Process dialog.

Cut Direction: These checkboxes indicate the direction the tool will move along the designated cut shape. If the Forward option is checked, the tool will move from the start point to the end point of the selected cut shape as designated by the machining markers. Otherwise the tool will move from the end point to the start point of the selected cut shape. When the Back & Forth option is turned on, the tool will cut in both directions without rapiding to the beginning of the toolpath after each pass.

Start Side Extension: This option allows you to set an extra start distance for each roughing pass. This helps to ensure the tool will have a feed move starting off of the material.

36

Processes

Rough Type

The Rough Type radio buttons indicate what type of roughing cycle will be used for the current process. The three available rough types are Turn, Plunge, and Pattern Shift. Each rough type has a corresponding Clearance Diagram. The Plunge and Pattern Shift options will bring up dialogs asking for additional information specif ic to the selected rough cycle. The information required for each rough type is detailed below.

Turn: When the Turn option is selected, a Cut Depth amount must be entered that specif ies the depth of cut the tool will make on each roughing pass. Depending on the Approach Type selected, the cut depth will either be an Xr or Z value. Please note that Notch Ramp (set in the tool dialog) will reduce the depth of cut on one stroke and increase it on the next. Please ensure that the ramp value is smaller than the depth of cut.

Pull Off Wall: Checking this box will cause the tool to pull off the wall instead of machining the wall. This will result in a “stair-step” toolpath as the tool pulls up and retracts.

Cleanup Pass: A cleanup pass will go back and remove any material left by Pull Off Wall.

Figure 1: Toolpath generated with Pull Off Wall and a Cleanup Pass.

Plunge: When a Plunge Rough Type is selected, the following changes are made to the standard Rough dialog.

Plunge dialog: This dialog allows the user to input specif ications for Plunge roughing cycles. The Plunge Angle specif ies the angle at which the groove tool will plunge into the part. The default value for the Plunge Angle is 270°, which causes the tool to plunge straight down.

There are two options available for the Cut Width. When the Exact option is selected, the user enters a distance in Z that the tool will step over on each plunge. The Calculate option will vary the cut width as necessary so that the toolpath hits the endpoints of every feature in the selected cut shape. When the Center Out Cuts option is selected, the tool will make its f irst plunge in the center of the groove, and then proceed to rough out each side. The Multi-Pass option performs “breadth f irst style plunging.” This will take cuts across at the same level X and then drop down by the step amount. The Plunge Type options allow the user to select the type of move the tool will make when it f irst enters the part in a plunge roughing operation. The Plunge Type options include Feed, Peck Full Out and Peck Retract and are described in detail below.

Plunge: This option designates that the f irst plunge will be a continuous feed move from the clearance position to the bottom of the groove. The First Feed percent value specif ies the percentage of the feed rate setting for the Process.

37

Processes

On First Plunge Only: For Peck Full Out and Peck Retract, you may designate these options for the f irst plunge only.

Peck Full Out: This option designates that the f irst plunge be a peck. The user specif ies a Peck Amt and a Clearance amount. Because it is a Peck Full Out, after each peck the tool will retract all the way out of the groove to the clearance position. The tool will then reenter the part and begin its peck move a clearance distance away from the remaining material.

Peck Retract: This option also designates that the f irst plunge be a peck. A Peck Amt is again specif ied. In addition, the user specif ies a Retract amount which specif ies how far the tool will come out of the actual cut instead of coming all the way out of the part.

Pattern Shift: This dialog allows the user to input specif ications for Pattern Shift roughing cycles. The Xr Cut and Z Cut values specify the amount of material to be removed on each roughing pass. The cut amount in each axis does not need to be the same.

If the Full option is selected for the Rough Style, the user must enter a Cycle Start Point and designate the number of passes to be made. The Cycle Start Point specif ies the coordinate the tool uses as the beginning point for the Pattern Shift roughing cycle. This point should be clear of the part. The Fixed option, when turned on, designates that the tool will return to the Cycle Start Point after each pass. When this option is not on, the tool will return to the Cycle Start Point minus the Xr Cut and Z Cut after each pass. The Passes value specif ies the number of cuts necessary to remove the desired amount of material in this process.

If the Square Corners option is selected, the system will not add a radius move at the corners of the cut shape.

Instead, the tool will only make sharp moves when going around a corner and will leave contact with the f inished shape, possibly creating a burr at the corner. If this option is not selected, the system will always stay in contact with the part when moving around corners.

Offset Contour: This type of roughing produces passes that follow the shape of the part prof ile on every pass, using a decreasing offset for each pass. This should be used when it is desirable to follow the shape of the f inal contour with all roughing passes. This is advantageous in that each pass removes a consistent amount of material for the entire pass, unlike other roughing types which can intersect the part prof ile at different positions along the pass. This is particularly important for materials that work-harden due to the fact that these materials can cause too wear or breakage if any of the cutting is performed with a thin amount of material being removed.

Clearance Diagram

The picture will change depending on various options such as the Approach Type selected and the Clearance option selected in the Document dialog. Auto Clearance will calculate the clearance positions automatically if it is the selected option. If not, the user must enter Entry and Exit Clearance Positions which are used differently depending on the Approach Type selected.

38

Processes

An Auto Clearance value in the Document dialog will disable the Entry and Exit Clearance positions because they are handled universally.

If Material Only is selected as the Rough Style, the diagram will have options for Entry and Exit Clearance Positions as shown in the picture.

The Entry Clearance Position specif ies the location the tool will make a rapid move to before feeding to the operation start point. The Exit Clearance Position specif ies the location the tool may rapid to after completing its toolpath for that operation. Both boxes are labeled with arrows going towards and away from the part, respectively. The use of the values entered for the Entry Clearance Position and Exit Clearance Position changes depending on the Approach Type selected. Refer to the Clearance Moves section in this chapter for more details.

The X Stock Start Position designates the position the f irst cut will be calculated from. This position will only need to be specif ied if the Full option is selected for the Rough Style (instead of Material Only). The move from this position to the f irst cut will be the amount of the cut depth. It will be a rapid move if the Rapid Step option is turned on under the Full option. Otherwise, it will be a feed move.

The Entry Clearance Position specif ies the position the tool will retract to between each pass. The use of this value changes depending on the Approach Type selected. The use of the value entered for the Exit Clearance Position changes depending on the Approach Type selected. Refer to the Clearance Moves section in this chapter for more information.

The X Stock Start Position only needs to be specif ied when the Full option is selected for the Rough Style. This position will only be used when either Peck Full Out or Peck Retract is chosen for the First Plunge option.

When that is the case, the value entered will be used as the point the f irst peck will be calculated from. The axis will change depending on the Approach Type selected.

Rough Style

The Rough Style selection affects the toolpaths created for the current operation. If the Material Only option is selected, the system takes into account the current stock conditions, including custom stock specif ications, when creating the toolpaths for an operation. When Material Only is on, the toolpath will only feed over areas that have not yet been machined in a previous operations. The system keeps track of material removed in previous operations and generates the current toolpath based on that information, providing for “no air cutting.�

Because of this, the order of operations directly affects how the part will be cut. If the order of operations is changed or operations are added or removed, all operations should be reprocessed in order to calculate for the change. The Redo All Ops item in the Edit menu makes reprocessing all operations of a part a very easy process.

The Clearance value specif ies an offset amount from the part geometry that the system uses to calculate where the tool can safely rapid during an operation. If the tool is within the clearance amount, only feed moves will 39

Processes

be allowed. This Clearance amount will be looked at along with the Auto Clearance amount when creating any necessary entry and exit moves.

The Full option gives the user more control over toolpath creation. When the Full option is selected, the toolpath generated will simply feed over the selected cut shape from the start point to the end point as designated by the machining markers. If the Rapid Step option is turned on, the tool will make rapid moves between each pass, otherwise all moves in the toolpath itself will be feed moves.

Stock Options Corner Break: The value entered in this text box specif ies a radius that will be put on every outside sharp corner of the selected cut shape. A value of zero will not break the corner, but will keep the tool in contact with the part as it moves to the next feature. Corner breaks are only calculated with turn and pattern shift roughing cycles.

Fin. Stock ±: The Fin. Stock value specif ies the minimum amount of material that will be left on the cut shape after a toolpath is completed. The Fin. Stock amount affects the cut shape which in turn affects the toolpath created in a canned cycle.

Xr Stock ±: The Xr Stock value allows the user to specify an additional stock amount for the X axis. The value entered here specif ies the amount of material that will be left on the cut shape along the X axis only. This stock amount is used as a parameter in canned cycles.

Z Stock ±: The Z Stock value allows the user to specify a separate stock amount for the Z axis. The Z Stock value specif ies the amount of material that will be left on the cut shape along the Z axis only. This stock amount is used as a parameter in canned cycles.

Roughing Feeds and Speeds

CSS (Constant Surface Speed): Selecting the CSS item will activate Constant Surface Speed (CSS). CSS will cause the spindle RPM to constantly change based on the diameter the tool is at and the SFPM used. The Max RPM setting is used to set an upper safe limit on the spindle RPM. If CSS is off, the specif ied RPM value will be used for the spindle speed.

The SFPM and Feed values can be automatically calculated based on the material selected if the CutDATA Material database is installed. In order for these values to be calculated and entered in the appropriate boxes, the SFPM and Feed buttons must be clicked. If no material is selected or the CutDATA Material database is not installed, the user will need to manually enter values for the feed and speed.

Entry Feed: By clicking on the Entry Feed button, the software will calculate the value based on our materials database. Alternatively, you may manually override the calculated value by inputting your own value. The entry feedrate is written to the toolpath for output in G code. This value affects every potential entry move of a toolpath.

Coolant Flood: This is the standard coolant option. Additional coolant options are available with custom post processors.

Prefer Canned: A checkbox that will output roughing cycles as canned cycles if the lathe being programmed is capable of handling canned cycles. If the Auto Finish option is turned on, a canned f inishing pass will automatically be added to the post processed code after the roughing canned cycle. The Prefer Canned option is only available when using Fixed Clearance positions (NOT Auto Clearance) and the Full Rough Style (NOT Material Only).

40

Processes

Cut Direction Axes

The Cut Direction Axes checkboxes allow the user to regulate the axes and directions of the cut shape.

Deselecting an axis will prevent cut shape moves in that axis direction. The default settings should have all axes selected.

41

Processes

THREAD PROCESS Thread processes are used to create ID and OD threads. When the Threading Function tile is combined with a Tool tile, the Process dialog shown below will appear. For more information on thread creation, see “Threading” on page 47 1.

2.

3.

4.

Thread Cut Options Thread Definition Thread Depth of Cut Thread Clearance Diagram 5. Thread Machining Parameters

Thread Cut Options Cut Direction: The selection made for this option determines the direction the tool will move when creating the thread. If the Z- option is selected, the tool will move towards the spindle. If the Z+ option is selected the tool will move away from the spindle. The Run In and Run Out distances and the actual thread start and end will change positions in the Clearance/Thread Diagram depending on the cut selection.

Approach Type: With both selections in the threading process, the approach is along the X axis. These selections allow the user to determine whether the thread will be located on the OD or the Front ID of the part.

The Clearance/Thread Diagram will change according to the choice made here.

Thread Definition

Style: The choices for Style are contained in a pop-up menu and allow the user to specify what type of thread will be cut. The selection made here designates the appropriate thread form for control of calculations.

Nominal Xd: The value entered in this text box is the diameter location of the thread as specif ied on the part blueprint.

TPI: The value entered in this text box specif ies the number of threads per inch.

Pitch: TPI and Pitch are interactive inputs. Entering either the TPI or Pitch calculates the value for the other input. For example, entering a TPI value of 1.0 will calculate a Pitch value of 25.4 (and vice versa.)

Taper: Taper is a “slope” value, not an angle. A slope is a ratio of vertical/horizontal distances. The equivalent angle is: 42

Processes

angle = tan (vertical/horizontal) or tan (slope) The NPT specif ication def ines the taper as 1/16, or 1” vertical for 16” horizontal, with the horizontal measured on the diameter. This entry requires a radial slope, or 1/32. You may type in 1/32 or you may type in .03125, the decimal equivalent. If your taper is def ined as a radial angle, the slope = arctan (angle). # of Starts: The value entered here is the number of starts for the thread. Most standard threads have one start.

If a value greater than one is entered here, the process will create a multiple thread start.

Major Xd: The value in this text box automatically defaults to the value entered for the Nominal Xd; however, it can be changed. Cutting begins at this diameter on an OD thread.

Minor Xd: The value in this text box defaults to a calculated value based on the Nominal Xd and the desired pitch. Cutting begins at this diameter on an ID thread.

Thrd Ht Xr: This value is calculated by taking the difference between the Major and Minor diameters and dividing it by two. It represents the Thread Height given as a radius value.

In Feed: This section allows the user to control how a threading insert will cut. The Balanced option will cut with both sides of the insert equally. For UN thread forms, a Balanced or 0° In Feed takes all cuts at the same Z position. The Thrd Angle selection allows the user to specify the In Feed angle. The value entered is measured in degrees and specif ies the single edge In Feed angle for the thread form. The value 29.5° is the default Thrd Angle for all thread types. Each cut starts at a different Z position, always cutting with one edge. The Alternate option is available when Thrd Angle is the In Feed selection. When turned “on,” each cut taken at the specif ied angle will alternate (e.g. 29.5°, -29.5°, 29.5°) Only one edge is used at a time to cut, but it alternates to provide for maximum insert life. This is also known as “using the leading edge & trailing edge alternately”.

Thread Depth of Cut The selections made in this box allow the user to designate the cut depth for each pass of the threading operation. The One Finish Pass option specif ies that the tool will make a single pass over the thread. Its primary use is to remove burrs or small excesses of material on an existing thread. Selecting One Finish Pass will grey out the Last Cut dialog, as there is only one pass. The Const Cut selection allows the user to designate the Depth Of Cut that the threading tool will make on each pass. The value is measured as a radius and is entered in the text box labeled 1st. The Const Load selection allows the user to specify the depth of the cut made on the f irst pass. This value is also measured as a radius and entered in the text box labeled 1st. The amount of material (the load) removed for that depth of cut will be calculated, and on each successive pass the depth of cut will decrease while the tool pressure remains constant.

The Last Cut option is selected to prevent any cut from removing less than a given amount of material on the last pass. The value entered is measured as a radius value and specif ies the minimum cut for the constant load to diminish to. The Spring Pass option can be used in conjunction with any of the depth of cut selections. It will create additional passes equal to the number entered after the thread has been cut.

43

Processes

Thread Clearance Diagram 1.

2.

3.

4.

5.

6.

7.

Auto Clearance Thread End Thread Start Z Run Out Z Run In Entry Clearance Exit Clearance

If the Auto Clearance option is on, no Entry and Exit Clearance Positions need to be entered. If Auto Clearance is off, the Entry and Exit Clearance Positions must be entered to specify where the tool will move to when approaching and retracting from the part.

Run In values are used if the threading tool needs to begin a certain distance away from the actual thread start in order to accelerate to the proper feed rate. The Z Run In distance allows the user to designate a distance along the Z axis to begin the threading pass. The X Run In distance can be used in conjunction with the Z Run In distance to start the thread at an angle. The Run Out values allow the user to designate a distance and angle for the threading tool to come off the thread and function the same as the Run In values.

The Run In and Run Out labels and values will change positions in the diagram depending on whether the tool is cutting towards the spindle or away from the spindles which is determined by the selection made for cut direction (Z+ or Z-).

The Actual Thread Start and Actual Thread End values specify where along the Z axis the thread will begin and end. Any Run In or Run Out values will be added on the actual length of the thread.

Thread Machining Parameters

Coolant: This checkbox indicates whether coolant is on. Flood is the standard coolant option. Additional coolant options are available with custom post processors.

Prefer Canned: A checkbox that will output threading passes as canned cycles if the lathe being programmed is capable of handling canned cycles.

Material button: Clicking on this button will open the Materials dialog which will enable the system to calculate the recommended speed for the material selected. Refer to the Material Database section in this chapter for details.

Speed: RPM: The value entered here is the rate of the spindle measured in revolutions per minute. You may manually enter the RPM or click the button to auto-calculate the RPM based on the Material database.

HOLES PROCESS Holes Processes are used to make holes on center (X0). When the Drilling Function tile is combined with a Tool tile, the following Process dialog will appear.

Holes Entry/Exit Cycle The selections made here determine the cycle the tool will use to make its hole features. The choices include: Feed In-Rapid Out, Feed In-Feed Out, Tap, Rigid Tap, Peck Full Out, and Peck Chip Breaker. Additional Entry and Exit Cycles are available with custom post processors.

44

Processes

1.

2.

3.

4.

Holes Entry/Exit Cycle Holes Drilling Options Holes Clearance/Drill Diagram Holes Machining Parameters

Holes Drilling Options

Clearance: This text box is only active if Peck Full Out is the selected Entry/Exit Cycle. The value entered specif ies the incremental distance away from the material that the tool will start its next peck from.

Peck: This text box is only active when either Peck Full Out or Peck Chip Breaker is the selected Entry/Exit Cycle. The value entered here specif ies the depth increment the tool will drill on each peck.

Retract: This text box is only active if Peck Chip Breaker is the selected Entry/Exit Cycle. The value entered here specif ies the amount the tool will retract after each peck.

Holes Clearance/Drill Diagram 1.

2.

3.

4.

5.

6.

7.

Auto Clearance Drill Surface Z Spot Diameter Entry Clearance Plane Exit Clearance Plane Sharp Tip Z Full Diameter Z

Entry and Exit Clearance Positions will need to be entered only if the Auto Clearance option is turned off, in which case these values specify the positions the tool may use when approaching and retracting from the part.

The other four values described below are all interactive, automatically calculating the unknown values.

Sharp Tip Z: Specif ies the absolute Z depth of the tool tip, and is the number that will be used in the posted output of the f inished code.

Drill Surface Z: Specif ies the absolute Z value of the surface of the part.

Spot Diameter: Specif ies the diameter of the hole at the Surface Z. This is useful when counter-sinking, for instance.

Full Diameter Z: Specif ies the absolute Z depth of the full diameter of the drill.

45

Processes

Holes Machining Parameters Dwell: The value entered in this text box allows the user to specify the length of time the drill will pause at the hole bottom with the spindle on. The value can either be measured in seconds (entered in the text box labeled sec) or in revolutions per second (entered in the text box labeled revs). Because the two boxes are interactive, a value only needs to be entered in one and the system will calculate the other.

Material button: Clicking on this button will open the Materials dialog which will enable the system to calculate the recommended speed for the material selected. Refer to the Material Database section in this chapter for more information.

Speed: RPM: The value entered here is the rate of the spindle measured in revolutions per minute. You may manually enter the RPM or click the button to auto-calculate the value from the Material Database. For information see the Material Database section in this chapter for details.

Feed: Plunge: The value entered here is the inches per revolution. You may manually enter the feed rate or click the button to auto-calculate the value from the Material Database. For information see the Material Database section in this chapter for details.

Coolant: A checkbox which indicates whether coolant is turned on in the process. Flood is the standard coolant option. Additional coolant selections are available with custom post processors.

Prefer Canned: A checkbox that will output the drilling moves as canned cycles if the lathe being programmed is capable of handling canned cycles.

46

Processes

THREADING This section is intended to assist in calculating the correct parameters for cutting both straight threads and standard NPT pipe threads using the system. First, an overview of general thread cutting using the system will be outlined. There are three things the user must def ine in order to properly cut a thread using the system: what kind of thread to cut, how to cut the thread, and where to cut the thread.

THREAD DIMENSIONS - DEFINING THE KIND OF THREAD TO CUT Style: This pop-up menu is used to select the thread style, such as UNF, NPT, etc.

Nominal Xd: This is the nominal thread diameter.

TPI: This is the number of threads per inch, (per millimeter for metric parts).

Taper (Slope): This is the decimal slope of the thread taper, measured radially. For straight threads, this value should be zero. For standard NPT pipe threads, this value should be 1/32 or 0.03125 (the slope of NPT threads is 1/16 of an inch per inch on diameter, which is 1/32 of an inch per inch radially). If you are creating a tapered thread with Run In, Canned Cycles should not be used. This is because most machines cannot handle this situation. # of starts: This is the number of thread starts. For multiple start threads, enter the number of starts here.

Otherwise, this value should be one.

Major Xd & Minor Xd: These values will default to the theoretical major and minor diameters based on a perfect sharp thread. The value as calculated is primarily for reference; this value can be changed as required for the particular thread class and f it desired. For OD threads, the minor diameter is critical as this will be the diameter that the tool will cut on the f inish pass. On ID threads, the opposite is true. The major diameter is critical as this will be the diameter that the tool will cut on the f inish pass of an ID thread.

Thrd Ht Xr (Thread Height Xr): This value is the actual thread height as a radius dimension. This value is calculated as the radial difference between the Major Xd and the Minor Xd and can be changed as required.

CUT INFORMATION - DEFINING HOW TO CUT THE THREAD Cuts (Z-, Z+): This is used to specify the direction of the thread cut; Z- will cut toward the spindle and Z+ will cut away from the spindle. The Z- choice is the default as most threads will be cut toward the spindle; only in rare cases is the Z+ option used.

OD, Front ID (Approach Type): This is used to specify whether the user is cutting an external or internal thread; the type of thread will affect the approach moves to the thread cutting cycle. It is also correct to think of this as the Thread Type.

In Feed - Balanced: This choice will feed the thread tool straight in for each pass resulting in both edges of the thread tool cutting equally.

The Balanced In feed is often used when cutting tough stainless steels that are easily work hardened, as the equal metal removal method helps prevent work hardening during the cutting cycle. This method usually does not work well on softer materials that tend to load up on the insert; for these materials it is usually best to use the Thread Angle In feed.

47

Processes

In Feed - Thrd Angle (Thread Angle): This choice will cause the positioning move at the start of each pass to feed the thread tool in at the angle specif ied, resulting in the leading edge of the tool doing most or all of the cutting. It is common to set the in feed angle slightly steeper than the thread angle so that the trailing edge of the tool takes a ‘light’ cut to ensure that the back side of the thread cleans up.

This option is often used to improve the chip flow on soft or gummy materials that tend to tear during the cutting cycle because of material load up on the tool Alternate: This option is only available when the Thrd Angle is selected for the In feed. It will alternate the in feed, resulting in the tool f irst cutting with the leading edge, then alternating to the trailing edge, and then back to the leading edge, etc. This provides even tool wear, in turn providing maximum tool life.

Depth Of Cut The values and options in this section of the Thread dialog are used to control the number of cuts as well as depths of cuts, minimum cut depth, and spring passes.

1st Xr: This value is the stock amount to remove on the f irst rough pass. This value also controls the entire roughing cycle as described below for Constant Cut and Constant Load.

One Finish Pass: This option specif ies that the tool only take one cut at the f inish thread depth. This would normally be used to re-cut a thread as part of a de-burring process.

Const Cut (Constant Cut): The Const Cut option will cause the roughing cycle to step in the amount specif ied in 1st Xr on each subsequent pass until the tool reaches the Last Cut amount. A larger 1st Xr will result in fewer passes, while a smaller 1st Xr will result in more passes.

Const Load (Constant Load): The Const Load option is the most commonly used type of thread roughing cycle.

This cycle will take a constant volume of material on each pass, resulting in a smaller depth of cut on each subsequent pass until the tool reaches the Last Cut amount. The volume removed on each pass is calculated based on the depth of cut specif ied in the 1st Xr f ield. This can also be considered a constant amount of tool pressure.

Last Cut: When selected, this option will prevent the roughing cycle from taking any rough passes at less than the value specif ied. In addition, the rough cycle will always leave exactly this amount for the last pass.

Spring Pass: This value is used to specify whether to take one or more spring passes at the f inish depth.

THREAD LOCATION - DEFINING WHERE TO CUT THE THREAD Thread Start Z: This value is used to specify where the actual thread begins in Z. If a thread begins at the face of the part, this value should be Z0; note that this is not the Z start of the thread cycle.

Thread End Z: This value is used to specify where the thread ends in Z. Z Run In: This is where the user specif ies the acceleration distance, incrementally. For example, if the thread cycle is to start 3/10” before the actual thread start, simply enter 0.300 for the Z Run In.

48

Processes

X Run In: This value would be used to specify an X acceleration value if necessary. Note that this value should normally be zero.

An example of where this is used would be to machine a cable groove in the drum of a cargo winch; in this case a round groove needs to be cut at a given pitch (similar to a thread) where the groove must start in, and be timed with, a hole drilled through the diameter of the part. Using both the X & Z Run In would allow the plunging of the tool into the hole after starting the thread cycle, thereby not cutting the area between the face of the part and the hole.

Z Run Ou: This value will extend the thread by the amount entered. If the threading tool needs to pull out from the thread on an angle, enter a value for the Z Run Out and the X Run Out. Typically, a zero would be entered.

X Run Out: When used with Z Run Out, will cause the tool to pull out of the thread on an angle. For example, to specify a thread pull out of 3/20� at 45 degrees enter 0.150 X Run Out and 0.150 Z Run Out. A pull out move at 45 degrees for a distance of 0.150 will be added to the thread cycle.

If the X Run Out value is less than the Z Run Out, a pull out move of less than 45 degrees will occur; and if the X Run Out is larger than the Z Run Out, a pull out move greater than 45 degrees will occur.

CUTTING STANDARD NPT PIPE THREADS The primary problem that most people encounter when trying to cut pipe threads is determining the correct Major or Minor diameter, which is necessary in order to program the tool path. Unfortunately, the Machinery’s Handbook does not supply these numbers. It provides the pitch diameter, and the major or minor diameters must be calculated accordingly. This becomes tricky due to the fact that all of these diameters are at an angle; therefore, these values will change depending upon the horizontal Z value.

Step by step instructions will be provided for programming both a 2.5"-8 NPT external and a 2.5"-8 NPT internal thread to show the actual process required to determine the minor and major diameters.

First, a given horizontal value must be established to act as a gauge point. Since the Machinery Handbook supplies the pitch diameter at the start of the thread, the horizontal value most commonly used is Z0 (the face of the part). The system also assumes this value for the major and minor diameters, and will calculate the major and minor diameters at the start and end of the toolpath based on this assumption. The advantage of this is that only one value needs to be calculated; in the case of external pipe threads, only the minor diameter at the face of the part is needed, and with internal pipe threads only the major diameter at the face of the part is needed.

2.5" - 8 NPT External Pipe Thread 1.

Find the Pitch Diameter at Beginning of External Thread (E0) from Machinery Handbook: American Pipe Threads: Table 3 (Basic Dimensions, American National Standard Taper Pipe Threads). For a 2.5" - 8 NPT external thread this value is 2.71953

2. Find the nominal truncated Height of Pipe Thread (h) from Machinery Handbook: American Pipe Threads: Table 1 (Limits on Crest and Root of American National Standard Taper Pipe Threads). This value is given as a max/min dimension; add the minimum and maximum height and divide by two to obtain the nominal thread height. For a 2.5" - 8 NPT external thread this would be (.1000+.09275)/2 or 0.096375 3. Find the Minor diameter at the start of the thread. To calculate this value, simply subtract the nominal thread height from the Pitch diameter (E0). For a 2.5" - 8 NPT external thread this would be 2.71953 0.096375 or 2.623155 49

Processes

2.5" - 8 NPT Internal Pipe Thread 1.

Find the Pitch Diameter at Beginning of External Thread (E1) from Machinery Handbook: American Pipe Threads: Table 3 (Basic Dimensions, American National Standard Taper Pipe Threads). For a 2.5" - 8 NPT internal thread this value is 2.76216

2. Find the nominal truncated Height of Pipe Thread. This value does not change for external and internal threads and is the same as the 2.5" - 8 NPT external thread above (0.096375) 3. Find the Major diameter at the start of the thread. To calculate this value, simply add the nominal thread height to the Pitch diameter (E1). For a 2.5" - 8 NPT internal thread this would be 2.76216 + 0.096375, or 2.858535

AMERICAN NATIONAL STANDARD TAPER PIPE THREAD (NPT) CHART This is a simple chart containing the values for the Standard NPT Pipe Thread sizes. For an external thread, enter the Minor diameter as given on the chart, and for an internal thread, enter the Major diameter as given on the chart.

PIPE SIZE

50

EXTERNAL THREADS

INTERNAL THREADS

Nominal Pipe Size

TPI

Minor

Major

Minor

Major

1/16”

27

0.2439

0.2985

0.2539

0.3085

1/8”

27

0.3362

0.3908

0.3463

0.4009

1/4”

18

0.4360

0.5188

0.4502

0.5330

3/8”

18

0.5706

0.6534

0.5856

0.6684

1/2”

14

0.7045

0.8124

0.7245

0.8324

3/4”

14

0.9138

1.0216

0.9349

1.0428

1"

11 1/2

1.1475

1.2797

1.1725

1.3047

1 1/4”

11 1/2

1.4910

1.6232

1.5173

1.6495

1 1/2”

11 1/2

1.7300

1.8622

1.7563

1.8884

2"

11 1/2

2.2029

2.3351

2.2302

2.3624

2 1/2”

8

2.6232

2.8159

2.6658

2.8585

3"

8

3.2442

3.4370

3.2921

3.4849

3 1/2”

8

3.7411

3.9339

3.7924

3.9852

4"

8

4.2380

4.4308

4.2908

4.4835

5"

8

5.2944

5.4871

5.3529

5.5457

6"

8

6.3497

6.5425

6.4096

6.6023

8"

8

8.3372

8.5300

8.4037

8.5964

10"

8

10.4489

10.6417

10.5246

10.7173

12"

8

12.4364

12.7286

12.6208

12.7142

Processes

14" OD

8

13.6786

13.8714

13.7763

13.9690

16" OD

8

15.6661

15.8589

15.7794

15.9721

18" OD

8

17.6536

17.8464

17.7786

17.9714

20" OD

8

19.6411

19.8339

19.7739

19.9667

24" OD

8

23.6161

23.8089

23.7646

23.9573

51

Processes

PRE-DEFINED PROCESS GROUPS All machining operations are created from the information contained in the Process List. Processes are created by combining a Function tile with a Tool tile and entering the necessary information in the Process dialog. A Process Group is the collection of Process tiles contained in the Process List at any one time. A Process Group contains all of the tooling and machining information needed to generate a specif ic set of operations.

A Process Group can be saved as an external f ile that can then be loaded into other part f iles. This capability allows user to access and reuse common machining and tool data for multiple part f iles quickly and easily without having to recreate tools and processes.

Process Groups can be saved by selecting Save from the Processes menu when the Process List contains the completed Process tiles that will compose the group. The system will ask for a f ile name and a location to save the f ile. Once a Process Group f ile is saved, it can be loaded into any part f ile by selecting the Load item from the Processes menu. Another way to quickly load Process Groups is by choosing a directory that contains Process Group f iles. The directory is chosen by selecting the Set Directory item from the Processes menu. When a directory is set, all the Process Group f iles contained in that directory will appear in the Processes menu. For a quick load, simply select the name of the Process Group f ile to be loaded from the list.

When a Process Group is loaded into a part f ile, any Process tiles currently highlighted in the Process List will be removed and replaced by the loaded Process Group (if this removes process tiles that were needed, simply select Undo from the Edit menu). If the Tool List contains Tool tiles, those tools will become deselected but not removed from the list. The system will search through the existing Tool List to f ind the necessary tools for the loaded Process Group. If the system f inds an exact tool match, that tool will be used. If an exact match is not found, the necessary tools for the loaded Process Group will be created and added to the Tool List in the f irst available positions. Added tools will be highlighted.

Once the Process Group is loaded into the Process List, select the appropriate geometry to act as the cut shape and click on the Do It button to create the operation and toolpath.

52

OPERATIONS

Operations

CHAPTER 6 : Operations CLEARANCE MOVES This section contains information and diagrams on rapiding and feeding around lathe parts. It is very important when working with lathes to avoid tool interference with the part, the spindle, etc., while at the same time quickly and eff iciently maneuvering around the part. Clearance positioning is the term used for various positions the tool will move to when not actually cutting the part.

The primary tool change position is specif ied in the Document dialog. This position can be overridden on a tool by tool basis using the Turret Shift function in the Tool Creation dialog. For more information on Turret Shift, refer to the Tool Creation chapter. If Tool Change is turned off, it is assumed that the f inished code will be manually edited to handle the tool change. Otherwise, the tool will start at the Tool Change position entered in this dialog.

In addition to specifying the position of the turret when tools are changed, the Document dialog provides the user with two options for handling part clearance, Auto Clearance or Fixed Clearance. The selection made will determine how the system will calculate positioning moves between operations.

AUTO CLEARANCE

The Auto Clearance option performs several functions when it is turned on. It will calculate the part clearances in both Z and X that are used to position the tool between each operation. These positioning moves will be dynamically calculated for each operation. This means that as the stock conditions of the part change as material is removed, the clearance positions will adjust accordingly. When Auto Clearance is on, the system will also take into account where the tool needs to be to begin the next operations’ toolpath when calculating the positioning moves. Additionally, the Auto Clearance function may add entry and/or exit moves to the toolpath in order to safely maneuver around the part. The Auto Clearance function generates the most eff icient positioning moves around a part. However, canned cycles cannot be used in conjunction with Auto Clearance. In order to use canned cycles, which are turned on in Process dialogs by selecting the Prefer Canned option, Fixed Clearance positions must be used.

The Auto Clearance option requires the user to enter an offset amount from the part stock that the system uses to calculate the clearance positioning moves between operations. Because the stock conditions are constantly changing as material is removed from the part, in order to optimize the toolpaths, an offset amount is used for positioning rather than absolute positions. Fixed clearance, which is used when Auto Clearance is turned off, uses absolute positions.

FIXED CLEARANCE

When the Auto Clearance option is turned off, f ixed clearance positions are used by the system to calculate clearance moves. The user must enter an overall part clearance in the Document dialog, as well as Entry and 55

Operations

Exit Clearance Positions in the Process dialogs for each operation. When using canned cycles, f ixed clearance positioning should be used.

The overall part clearance is entered in the Document dialog in the X and Z text boxes that become active when Auto Clearance is turned off. They designate the position the tool will rapid to and from during a tool change. This position will also be used when moving from one approach type to another between operations that use the same tool. The absolute positions specif ied in the X and Z text boxes are locations the tool can rapid to when moving around the part. One or both of these f ixed positions are used whenever a tool is moving to the start point of the toolpath or exiting from the toolpath. Where the tool moves when approaching and retracting from the part depends on the Approach Type selected and the positions specif ied in the Clearance Diagrams in the Process dialog.

The Approach Type selections are located in the upper left corner of the Process dialog. The tool can approach the part along two different axes—either X or Z. The tool will approach the part along the Z axis if Front Face is selected. The tool will approach the part in X if OD or Front ID is selected. When a Drilling Process is selected, the Approach Type is automatically set to Front Face. Only one selection can be made for each process.

Once the Approach Type is selected, the corresponding Clearance Diagram appears in the Process dialog. The boxes with the arrows next to them represent the Entry and Exit Clearance Positions that the tool may use when approaching and retracting from the part. The Entry and Exit Clearance Positions are only required when Auto Clearance is turned off.

When a Turn roughing cycle is selected, an additional move will be added between the Entry Clearance Position and the X Stock Start Position. When a Pattern Shift roughing cycle is selected, an additional move will be added between the Entry Clearance Position and the contour start point.

CLEARANCE DIAGRAMS The tool will use some or all of the clearance positions depending on which Approach Type is selected. When Auto Clearance is selected, the tool will still move to the positions indicated in the diagrams shown below.

However, the system will calculate these positions and they will change as the material conditions of the part change. Also, when Auto Clearance is on, the system may add additional entry and exit moves as necessary to prevent tool interference. The following conventions are used in the clearance diagrams.

Black Dot

Absolute coordinate the tool will move to; each Black Dot has an X and Z coordinate

Dashed Line

Rapid Move

Solid Line

Feed Move

SP - Start Point

The f irst move of the operation. Not necessarily the Start Point Machining Marker.

EP - End Point

The last move of the operation. Not necessarily the End Point Machining Marker.

OP1

Operation 1 (the f irst series of cuts made on the part)

OP2

Operation 2 (the second series of cuts made on the part)

56

Operations

APPROACHES FROM TOOL CHANGE POSITION The tool can approach the part in three different ways from the tool change position.

OD Approach From Tool Change 1.

2.

3.

4.

Tool Change SP Z, Part Clearance Xd SP Z, Entry Clearance Xd SP Xd

Face Approach From Tool Change 1.

2.

3.

4.

Tool Change SP Z, Part Clearance Xd Entry Clearance Z, SP Xd SP Z

ID Approach From Tool Change 1.

2.

3.

4.

5.

Tool Change Part Clearance Z, Part Clearance Xd Part Clearance Z, SP Xd SP Z, Entry Clearance Xd SP Xd

57

Operations

EXITS TO TOOL CHANGE POSITION The tool can exit from the cut shape to the tool position in three different ways.

OD Exit To Tool Change 1. EP Xd 2. EP Z, Part Clearance Xd 3. Tool Change

Face Exit To Tool Change 1.

2.

3.

4.

EP Z Part Clearance Z, EP Xd Part Clearance Z, Part Clearance Xd Tool Change

1.

2.

3.

4.

5.

EP Z EP Z, Part Clearance Xd Part Clearance Z, Exit Clearance Xd Part Clearance Z, Part Clearance Xd Tool Change

ID Exit To Tool Change

58

Operations

SAME TOOL POSITIONS If the next operation uses the same tool, there are seven different methods the tool could use to get to the next start point.

OD To Face

Op #1 Op #2

1.

2.

3.

4.

5.

6.

EP Z EP Z, Part Clearance Xd Part Clearance Z, Part Clearance Xd Part Clearance Z, SP Xd Entry Clearance Z, SP Xd SP Z

1.

2.

3.

4.

5.

EP Xd EP Z, Exit Clearance Xd SP Z, Exit Clearance Xd SP Z, Entry Clearance Xd SP Xd

OD To OD

Op #2

Op #1

Face To ID

Op #1

1.

2.

3.

4.

5.

EP Z Part Clearance Z, EP Xd Part Clearance Z, Entry Clearance Xd SP Z, Entry Clearance Xd SP Xd

Op #2

59

Operations

Face To OD

Op #2

1.

2.

3.

4.

5.

6.

EP Z EP Z, Part Clearance Xd Part Clearance Z, Part Clearance Xd SP Z, Part Clearance Xd SP Z, Entry Clearance Xd SP Xd

1.

2.

3.

4.

5.

EP Z EP Z, Part Clearance Xd Part Clearance Z, Part Clearance Xd Entry Clearance Z, SP Xd SP Z

1.

2.

3.

4.

5.

6.

EP Xd EP Z, Exit Clearance Xd Part Clearance Z, Exit Clearance Xd Part Clearance Z, SP Xd Entry Clearance Z, SP Xd SP Z

1.

2.

3.

4.

5.

EP Xd EP Z, Exit Clearance Xd SP Z, Exit Clearance Xd SP Z, Entry Clearance Xd SP Xd

Op #1

Face To Face

Op #2 Op #1

ID To Face

Op #2

Op #1

ID To ID

Op #2 Op #1

60

Operations

CANNED CYCLES The Auto Clearance and Material Only functions of the system calculate more eff icient toolpaths than canned cycles. Auto Clearance is activated in the Document dialog and designates that the system dynamically calculate clearance positioning moves for the part. The Material Only option is located in Process dialogs and designates that toolpath calculation for an individual process take into consideration the material conditions of the part to provide for no “air cutting.� If either of these options are being used, the Prefer Canned option found in the Process dialogs will not be available.

Using canned cycles will output shorter processed code however, the Auto Clearance and Material Only functions will produce more eff icient toolpaths in general. To generate canned cycles in the posted code, turn Auto Clearance off and enter f ixed X and Z clearance positions in the Document dialog, and select the Full Rough Style in the Rough Process dialog.

61

Operations

MACHINING MARKERS Machining Markers allow the user to specify the start and end feature and start and end point of the cut shape, the cut direction, and the offset position of the tool. These markers appear on the screen when geometry is selected as the cut shape for Contouring and Roughing Processes.

Start Feature: The geometry feature (line or circle) on which the tool will start cutting.

Start Point: The point on the start feature where the tool will start cutting.

End Feature: The geometry feature on which the tool will stop cutting.

End Point: The point on the end feature where the tool will stop cutting.

Move Start\End Point by . . .: The right-click context menu for a start or end point includes the Move Start\End Point by . . . option. By selecting this option, you will be prompted by a dialog to enter a new value (+ or -) by which to extend or trim the point from the beginning or end of the last feature. The options presented will depend on whether you select a Start Point or and End Point machining marker.

Cutter Side and Direction: The circles represent the offset position of the tool with regard to the cut shape. The three possible options are the inside, centerline or the outside of the cut shape.

The arrows indicate which direction the tool will travel. Simply click on the desired circle and direction arrow.

HOW MACHINING MARKERS WORK Machining Markers appear on selected geometry for contouring and roughing processes only. To move a marker, the cursor is placed over the marker, and when the mouse button is depressed, the cursor changes to the marker. This is called “picking up a marker.” The marker is then moved to the desired location and the mouse button released. Note: When positioning or placing a marker, place the “tip” of the “marker arrow head” onto the line, circle or point.

When the Start Feature marker is moved to a new feature on the geometry, the Start Point marker will “follow” it and snap to the same point as the Start Feature. This is also true for the End Feature marker. To make the Start Point and End Points the same: drag the Start Feature to the desired feature, and drag the Start Point to the desired location, drag the End Feature to the same feature- the End Point automatically snaps to the Start Point.

For precise control over the Start and End Point marker locations, create a geometry point at the desired location. Dragging a Start or End Point marker close to the point will cause the marker to “snap” to the point and use its exact XZ values.

START AND END POINTS The Start and End Points do not necessarily have to be on the part geometry. There may be times when it is desirable to have the tool start or end its toolpath off the part. This can be done by moving the markers. A geometry feature (e.g. line or circle) is trimmed between two connectors. When the Start Point marker is dragged off the part, it automatically snaps to the nearest extension of the Start Feature. The nearest section of the Start Feature may be a section that was trimmed away, so the Start Point will snap to an extension of the Start Feature. This is also true for the End Feature. The end feature markers may be quickly set using a

62

Operations

Ctrl+Shift click. When performing a Ctrl+Shift click the end point markers will snap to the location you clicked.

SELECTED GEOMETRY The machining markers allow the user to specify the portions of geometry to act as the outline for the cut shape. When markers are present on geometry, the cut shape is indicated by a dark blue color. When the cut shape is not the entire contour, the geometry not included as part of the cut shape is drawn in light blue.

The prof iler may also be used to create the geometry for lathe processes from a solid. For detailed information on this process please see the 2.5D solids manual or the Solid Surfacer manual.

USING THE PROFILER You can use the prof iler at Z0 to select a cut shape prof ile directly from a solid. The prof iler acts just like geometry except that it is volatile and will not be shown when prof iler is turned off. If you create an operation in the prof iler and subsequently turn it off, double clicking on the operation will turn the prof iler back on and display the machining markers.

63

Operations

MATERIAL DATABASE The Material Database is used for storing and quickly retrieving feeds and speeds for various types of materials.

The calculations will come from either the CutDATA Material Database (which is an option that can be purchased with the system) or from the default material database. A custom material database can also be created. The information in the database can be changed by selecting Materials from the File menu. To use the information, click on the Material button in any of the Process dialogs. Below is a picture of the Materials dialog. It is used for both creating and editing materials as well as placing feeds and speeds information into Process dialogs. These values can be directly overridden by typing in the speed or feed info in the Process dialog at any time. The Material database is fully detailed in the Common Reference guide.

64

Operations

OPERATION TILES The operation list context menu contains several useful functions as detailed in the following paragraphs.

Operation Data: It is possible to edit certain operation specif ications in the Operation Data dialog. Values are locked by clicking once on the lock next to the text box. Unlocked values will return to their original values if the operation is reprocessed. Locked items will retain the values entered in this dialog even if the operation is reprocessed. Changes that affect the toolpath can be seen in the toolpath drawing and the rendered image. The information in the Process Tile that created the operation will not be modif ied to reflect the changes made in the Operation Data dialog.

Information entered in the Op Comment text box will appear in the posted output before the selected operation it refers to. Utility data can also be entered in this dialog.

Custom posts allow the user to input custom commands in the At Op Start and At Op End text boxes that will trigger actions inside the post processor. In addition, any text that appears in quotations in the At Op Start and At Op End text boxes will appear in the posted output. Each set of quotes will be on a separate line in the posted output.

The Program Stop checkbox is only available in the Operation Data dialog. If it is turned on, a program stop command will be added at the end of the operation in the posted output. The default position is off.

If operations contain locked values, a small lock symbol will appear on the Operation Tile.

If utility data is

entered in the At Op Start text box, a small recessed square will appear on the Operation tile in the upper left hand corner. If utility data is entered in the At Op End text box, a small recessed square will appear in the lower left hand corner of the Operation Tile.

Utility Markers: The Utility Markers menu item allows editing of various position-dependent toolpath data. When chosen, the dialog shown will come up as well as the current operation’s toolpath.

For each operation, you may select a variety of utility marker types, many of which have additional sub-options. The primary options are Variable Feed Rate, Spindle Speed, Tool Offset #, Text, CRC, Dwell and Tool Sub Position.

To add markers of any type to a toolpath, drag and drop the marker of the desired type to a toolpath. The currently selected markers properties will be displayed in the dialog, and the currently selected marker will be displayed in red.

65

Operations

Additionally, you may select the checkbox to “Show All Markers.” When this checkbox is on, the icons for all utility marker types are displayed on the toolpath. When you step through the markers, the dialog performs context switching so you can see the details of each utility marker. Each marker now has a unique icon.

All of the new markers will require a post processor upgrade, except for Variable Feed Rate and CRC. Please contact the Tech Support Department for more information.

Variable Feed Rate: This marker allows you to set the feedrate for the elements of the toolpath following the marker. The f ive sub-options for this type of marker are User, Entry, Contour, Percent and Max. User allows you to explicitly set the feedrate to your desired value. Entry sets to feedrate to the operation’s def ined entry feedrate. Contour sets the feedrate to the operation’s def ined contour feed rate. Percent sets the feedrate to a user def ined percentage of the last f ixed feedrate marker. Max sets the feedrate to the maximum feedrate def ined by the post processor.

Spindle Speed: For turning ops, this marker sets the spindle speed to the value def ined in the SMPM or SFPM f ield.

Tool Offset #: This marker sets the tool offset. There are three options available here Tl Offset, Deflect Tl Offset and Explicit Offset. Tl Offset will set the offset to the Offset # def ined by the tool. Deflect Tl Offset will set the offset to the Deflection Compensation Offset # def ined by the tool. Explicit sets the offset to a user def ined value.

Text: This marker allows you to insert a comment into the posted output.

CRC: This marker is used to turn CRC on or off during an operation. There are three options available for this marker, On, Off and Reverse. Please see the section on CRC in the Process portion of the manual for further details.

Dwell: This marker causes the program to pause (dwell) for the specif ied time. This marker has two option, Seconds or Revolutions. The Revolutions option uses the current spindle speed to compute the time.

Program Stop: This marker causes the post to output a program stop (M0). If the Optional Program Stop box is checked the post will output an optional stop (M1).

Tool Sub Position: This option is only available for Lathe machines that allow tool sub positions. This marker allows you to set the tool sub position.

66

Operations

This image shows Utility Markers placed on toolpath. The markers are placed by an arc, modifying the speed going into and coming out of the arc.

Open Tool: This brings up the tool dialog associated with the operation.

Operation To Geometry: This option converts the selected operations to geometry. This geometry can be edited and used as a centerline contour op if necessary.

Redo Selected Ops: This will reprocess the toolpath for any selected operation(s).

Redo All Operations: This will reprocess the toolpath for all operations.

Move To: This selection allows the user to move one or several of the operation tiles to the end of the list or to another tile location by entering the tab number of the destination tile location and clicking Move To. It functions exactly the same as the Move To item on the Tool and Process tiles.

Find: The Find option allows a user to locate a specif ic tile By Tile #, Tool # or to f ind the last tile. It functions exactly the same as the Find item from the Tile List Scroll Arrows.

Sort Operations: This command will change the order of all operations. The operations will be sorted by tool number, from low to high. Operations created in the same Process List will maintain their order to ensure that f inishing passes cannot be moved in front of roughing passes, etc.

Operation Manager: The Operation Manager is an expanded view of the Operation list. The Operation Manager can show 31 different operation parameters, can sort operation data and can calculate accurate runtimes. Additionally the Operation Manager and the Operations list have synchronized selection meaning that as operations are selected or

67

Operations

deselected in one they are also selected or deselected in the other. Double clicking on an entry will load the operation’s process tiles

Right clicking on a column header: The items displayed in the Operation Manager can be customized. The Operation Manager supports 31 different parameters but it is impractical to try and view all at the same time. Right clicking on one of the parameter headers, such as the Depth parameter seen in the previous graphic, allows you to choose which parameters are displayed.

Right clicking on the title bar: The title bar offers access to several very useful commands including the sort command and runtimes. Additionally, the Operation Manager can be printed from here.

Sorting: Selecting the Multi-Level Sort‌ command opens a dialog where you can select how you wish to sort operations. Operations may be sorted by up to four parameters and each may be in an ascending or descending order. The sorts are based on the parameters shown in the Operations Manager.

It is important to realize that performing a sort will change the order of your operations. If you are not careful you could tell the system to do something you do not want, such as tapping a hole before the hole is drilled. The system does have a reminder to warn you that performing a sort can be harmful but you should still be aware of the potential consequences.

Right clicking on a cell entry: Right clicking on an entry brings up the same menu as right clicking a tile in the Operations list. From this menu you can access things like Operation Data, Utility Markers and Redo functions.

68

Operations

TOUCH-OFF POINT INFORMATION All post data is output to the theoretical tool tip. If the tool is machining parallel to the Z-axis, the X values are output to blueprint dimensions. If the tool is machining parallel to the X-axis, the Z values are output to blueprint dimensions. So, the theoretical tool tip only aligns with blueprint dimensions on faces and diameters.

When the tool is machining at an angle, the X and Z-axis values will not match the blueprint dimensions. This is because the theoretical tool tip is not always a blueprint dimension. So, in order for the system to get the surface of the tool in position to cut the part, the theoretical tool tip is calculated closer to the part, and in some cases inside the part.

69

Operations

70

CUT PART RENDERING

Cut Part Rendering

CHAPTER 7 : Cut Part Rendering CUT PART RENDERING OVERVIEW Modeling is the process of def ining a three dimensional object. Rendering is the process of displaying a picture of this model. A cut part model is def ined when the operations necessary to machine a part have been created.

The computer has 3D knowledge of the inside of the model, even of the areas that are not visible.

The cut part rendering capability in the system is called Three Dimensional Real Time Cut Part Rendering.

“Three Dimensional” refers to the fact that the model can be rotated around in space and viewed at any angle.

“Real Time” refers to the speed at which the part is rendered. The cutting action is rendered as it is calculated rather than calculating the rendered image and then playing back a “movie,” or just displaying a picture of the f inished model. Real Time does NOT mean actual feed rates are used. The tool can cut as fast as the computer can calculate the moves. “Cut Part” refers to watching the effect of the tools cutting, as opposed to seeing only the f inished picture. Seeing the cutting process is more valuable, in most cases, than the f inished picture.

Rendering refers to the process of displaying the graphic image of the cut part model def ined by the machining operations.

The system has two distinct Cut Part Rendering (CPR) methods. The f irst is Standard CPR. Standard CPR is the system’s legacy rendering mode. The second mode is Flash CPR. Flash CPR is an OpenGL-based system which is more powerful and flexible than Standard CPR. We have two modes for CPR because each has its own strength. You can use whichever suits your needs or use both modes. Additionally, if you have purchased the Machine Simulation option you can use that render mode.

All operations are rendered in their current order. Selected operations will render in shades of yellow, and all others will render in shades of grey. Shades of red will be drawn when non-cutting tool surfaces or rapid moves hit the material. Selected tools will be drawn in shades of yellow. Deselected tools will be drawn in shades of grey. Smaller pictures will render faster and use less computer memory.

COMPARING STANDARD AND FLASH CPR The two rendering modes are two completely different technologies. The primary difference between the two rendering modes is that Standard CPR is view dependent while Flash CPR is view independent. Basically, with Standard CPR the rendering process will start over whenever the view is changed or zoomed while Flash CPR is a “machined” solid model so it can be manipulated while being rendered.Flash CPR is far more useful for part analysis despite its slower speed.

Function

Standard CPR

Flash CPR

Speed

For any specif ic view Standard CPR is The speed of Flash CPR is dependent upon the usually faster. image quality and size of the rendered image.

Change of View

Restarts every time – it is best to select the view you want f irst.

Rendering is not interrupted by a change of view.

Quality

A f ixed image quality.

Image quality is user-controlled.

Transparency

Tools may be set to transparent.

Tools, f ixtures and stock can be transparent.

Collision Checking

None.

Yes.

Facet Bodies

None.

Create from rendered image and use as a stock condition.

73

Cut Part Rendering

RENDERING PALETTE When the Cut Part Rendering button is clicked, the Cut Part Rendering palette appears on the screen, and the stock shape will be displayed as a blue, solid image. The Cut Part Rendering palette controls the cut part rendering process. The functions of the items in the palette are described below.

Current Display: This box displays the number of the current operation being rendered or the current runtime.

Rewind: This button sets the current operation to the f irst operation. If the Play button is down when the Rewind button is depressed, the part will be redrawn.

Stop: This button stops any rendering in progress and raises the Play button.

Step Forward: This button renders the next feature of the current operation. If the Play button is depressed, it will be raised and rendering will be stopped at the end of the current feature.

Play: When the play button is depressed, the part will be rendered from the current feature of the current operation as listed in the Current Display box. Rendering will continue until one of the other buttons is depressed or the last feature of the last operation is rendered. The Stop and Step Forward buttons stop the rendering and raise the Play button. Pressing the Play button during rendering will also stop the rendering. The Next Operation and Rewind buttons will change the current operation being rendered, but will not stop the rendering process. When the last feature of the last operation is complete, rendering will stop, but the Play button will remain depressed. Anytime the rendering process stops, hitting the Play button again will resume rendering from the current location.

Next Feature: If the Play button is depressed, the current feature being rendered is f inished and the remaining features for that operation are skipped. The next feature to be rendered is the f irst feature of the next operation. If the Play button is not depressed, the current operation is set to the next operation. The Operation Box will be updated, but nothing will be rendered until the Play button is depressed again.

Throttle Control: Shows the current location of the Throttle slider. The plus side represents maximum rendering speed, and the minus side the minimum. The location of the slider can be changed by dragging it left or right. This can be done during the rendering process and the effects will be seen as the slider is moved.

Invisible Tool: If this button is selected, the tools will not be drawn during the rendering process, although the material as a result of the tools cutting is removed (see example below). Radii will render more smoothly, and the part will render faster with this choice selected.

Transparent Tool: If this button is selected, transparent tools will be drawn during the rendering process (see example below).

Visible Tool: If this button is selected, solid tools will be drawn during the rendering process (see example below).

During the cut part rendering process, if the screen is redrawn due to a view change or redraw, the rendering process will start over from the f irst operation. Therefore, it is good practice to set the desired view before rendering the part.

74

Cut Part Rendering

When the rendering process is stopped by pressing either the Stop or Step Forward button, the next time the part is rendered the system will automatically stop the rendering process at the same location. User set stops are maintained by the system. Anytime the rendering process is stopped, simply click on the Play button to continue.

If the Play button is depressed when the Cut Part Rendering button in the Top Level palette is raised, it will resume playing when the Cut Part Rendering button is selected once again. It is essentially the same as pausing the render. However, if the view was changed, it will restart as stated above.

CUT PART RENDERING CONTEXT MENU Right-clicking on the title bar of the Cut part Rendering palette will bring up optional controls for setting a stopping point during rendering and changing the status display.

Optional Stop control Set Op Start/Stop #s... This option opens a dialog to specify a start and stop point before a specif ic operation begins.

Use Op Start: Placing a check mark on this option activates the Set Op Start #... option. Removing the check mark will disable the stop point specif ied in the Set Op Start And Stop dialog.

Use Op Stop: Placing a check mark on this option activates the Set Op Start/Stop #... option. Removing the check mark will disable the stop point specif ied in the Set Op Start And Stop dialog.

Current Display Options Show Time: This will set the status to display the elapsed cut time.

Show Op: This will set the status to display the current operation number.

FAST UPDATE The Fast Update quickly gets you back to the last rendered state of your part after changing the view. If you have begun rendering your part, press Stop then zoom or change the screen position of the part and press Play, the system will regenerate the rendering in the new viewing position and orientation as quickly as possible. It does this by automatically setting the CPR speed to the fastest speed and hiding the tool when replaying the

75

Cut Part Rendering

rendering. Once the render reaches the place it was last stopped the controls will revert back to your previous setting.

76

Cut Part Rendering

FLASH CUT PART RENDERING Flash CPR is an OpenGL based rendering option that provides an alternative to the standard rendering mode. Flash CPR is a non-view dependant option meaning that the part can be rotated, zoomed and panned during the cut part rendering. There are several other capabilities that go along with Flash CPR including the Rapid Cut option that displays only the end condition of each operation, resulting in a much faster rendering, but at a lower display resolution. Flash CPR is activated and deactivated by right-clicking on the Render button in the Top Level palette and choosing the Flash CPR option. The Flash CPR option uses the same Render palette as the traditional rendering engine.

FLASH CPR CONTEXT MENU Right clicking on the Render palette title bar provides access to the Flash CPR options. Set Op Stop#, Use Op Stop, Show Time and Show Op# are the same functions as the standard rendering mode.

Analyze Cut Part: The Analyze Cut Part dialog provides several options to determine the results of the toolpath on a rendered part. This is an easy way to determine if there are areas on a body that are not being machined (Remaining Material) or if any cuts violate the part. A solid must be selected prior to starting Flash CPR to use the Analyze Cut Part option.

Transparent Stock: If Transparent Stock is selected, the stock will be transparent, showing both the part and the stock when rendering.

Transparent Fixture: If the Transparent Fixture item is selected any f ixtures in the part will be transparent, allowing you to more readily see the stock body when rendering.

Rapid Cut: When enabled this will generate the f inished part in the background. The f inished result will be slightly less smooth than a normally rendered part. This will be disabled on any part with a rotary move.

Acceleration & Checking: The next set of options provide methods for accelerating or conf ining the rendered part.

Skip Pecks: The Skip Pecks option will not render any pecking moves used in drilling operations.

Skip Unselected Ops: Skip Unselected Ops will only render the currently selected operations.

Op Color Mode... This option utilizes color to enhance the functionality of CPR and Simulation. The corresponding options sub-dialog has 3 color modes, cut color, tool number and op number. The color palette is generated automatically to create a set of colors that are readily distinguishable from one another. The color of the remaining material changes with each operation.

77

Cut Part Rendering

Set CPR Stock=Target: This option causes Flash CPR to ignore the stock def inition. Instead, the selected body is used as stock and rendering is run on this body. This is a quick and easy way to check for gouges.

Collision Checking: Selecting Collision Checking enables the collision checking based on the options set in the Preferences, See the section “Flash CPR/Simulation Settings” or the Common Reference Manual for more information.

Show Rapid Tool: When this mode is on (indicated by a check next to the menu item) the tool is rendered in a different color to show when it is moving in Rapid mode.

POV Lock: The choices here all control how the part (or part/ machine) move during the simulation sequence. This gives the user control over how the virtual camera moves around the scene, def ining the point of view during animation.

The choices available for Point of View Lock will be different depending on the rendering mode. For CPR, Part Sim and Tool Sim, the options are Fixed Part, Tool Rotary Axes, Tool Linear Axes and Too Rotary & Linear Axes. For Machine Sim, the choices are Operator, Part, Machine Component, Tool Rotary Axes, Tool Linear Axes and Tool Rotary and Linear Axes.

Save To STL: Save To STL will save the current stock results of the Flash CPR rendered image to disk in STL format.

Create Facet Body: The Create Facet Body function turns the current cut rendered condition into a facet body.

The facet body will appear in the workspace as a transparent body. One of the few uses of facet bodies is that they can be set as stock for “display only” purposes, i.e. they cannot be used as a stock condition for creating toolpath but they can be shown in rendering for Flash CPR sessions. Looking at the properties dialog you can see that essentially nothing can be done but setting the body as a part, f ixture or stock. Setting a facet body as stock can be quite useful for saving a rendered condition so you can instantly get to later operations.

Don’t Pre-Load Sub Spindles: Disables sub-spindle stock generation. This will improve performance at the cost of not having accurate stock on the sub-spindle during the f irst run.

Reload Simulation: This option will reload the Flash CPR simulation.

Overlay Geometry: This will display the workgroup geometry on top of Flash CPR continuously. To display the Geometry temporarily, use CTRL+], which continues to work as in prior releases.

78

Cut Part Rendering

Settings: Settings opens the Rendering Preferences dialog that allows you to control the speed, quality and color of the Flash CPR display. Alternatively, this dialog can be accessed by opening the Display preferences tab (File->Preferences-Display) and clicking the Edit Flash CPR Settings . . . button which opens the Flash CPR Settings dialog.

Flash CPR/Simulation Settings Cutting: The Cutting options section allow you to control the quality and responsiveness of Flash CPR. Steps Per Update: Specif ies the maximum number of CPR features to render before updating the display. Large numbers will increase the rendering speed but will result in a rougher rendering animation. With large numbers the tool may appear to jump ahead of rendering, which will suddenly snap to the tool. This may be jerky, but can be rather fast. A low number provides a smooth animation, but may be slow.

Cut Part Chord Height: This is the resolution for the part and tools displayed in Flash CPR. There are separate settings for inch and metric tools. The smaller the value, the higher quality of the display and the more resources needed by the system, resulting in a slower rendering.

Body Chord Height: This option determines the resolution of bodies (part, stock and f ixtures) in rendering. There are two ways this can be set, either by the Chord Height (which is setting a specif ic value), or by the % of Body’s Chord Height option. This second option uses the value set in the Properties dialog. A setting of 100% will use the body’s Chord Height while a setting of 10% will is 1/10th of the body’s Chord Height.

Any percentage between 1 and 100,000 is acceptable. As the percentage is set higher the body will appear rougher but the display will be faster.

Collisions/Limits: The items found in the Collisions/Limits section of the dialog provide control over how the system reports machining errors while rendering. A collision in Flash CPR occurs when the tool rapids into the stock or touches a f ixture or if a holder touches anything. Any combination of the three available alert methods may be used. Please note that the Collision Checking option (in the Render Control palette) must be activated for the system to check for collisions.

Alert Types: The Beep option provides an audible alert, Log To Display will output an error in a collision log window and Stock Flash provides a visual alert to the error by flashing the rendered stock. Stop Animation will cease the rendering at the point of a collision.

79

Cut Part Rendering

Tolerance: The Tolerance setting allows a different value for metric and inch parts. Any collision within the specif ied tolerance will generate a collision alert.

Slider: This item allows you to change the sensitivity of the render speed control. The render speed is based around the size of features being rendered.

Circular Threads: Activate this option to create fake, “circular” threads when using Flash CPR. The rendered thread will be a series of indented circles the size of the thread and will not be helical.

This option renders much faster then drawing proper, accurate threads. A comparison of normal and “circular” threads is seen to the right.

Statistics: Select this option to open a window that shows the Flash CPR frame rate (how often the image is updated while rendering) and any errors that get logged. To close the window you need to deselect this option

PRINTING THE CUT PART RENDERED IMAGE After the rendering is complete, the rendered image can be printed in either black and white or color. When the rendered image is on the screen, choose Drawing from the Print sub-menu in the File menu. To adjust the way the image will print, choose Printing from the Preferences sub-menu in the File menu. The Printing Preferences dialog, shown below, allows the user to specify how the software will handle the background color.

If the printer being used is a black and white printer, choose the Black on White option to ensure that all portions of the image, including those that are of a light color, can be seen in the print.

80

POST PROCESSING

Post Processing

CHAPTER 8 : Post Processing POST PROCESSING OVERVIEW Once the operations to machine the part have been created, the f ile needs to be post processed. Post processing generates a text f ile (NC Program) that contains the machining operations and toolpaths from the part f ile (VNC.) This NC program is created using Post Processor f iles (PST Files) specif ic to individual machine controls. Communicating the posted text f ile to the CNC machine is discussed in the Communications chapter which follows this one.

POST PROCESSOR DIALOG The Post Processor button in the Top Level palette becomes active once machining operations have been created in a f ile. Clicking on the Post Processor button will display the Post Processor dialog shown below.

This dialog allows the user to select a specif ic post processor f ile, specify a program name and currently open part.

1.

2.

3.

4.

Post Processor Selection Program Name Communications Text Window

The Process button will generate the NC program for the f ile currently open. The text f ile will be saved under the f ile name displayed to the right of the Program Name button. If a f ile with that name already exists, clicking the Process button will erase the old f ile and replace it with the new one. To view the text f ile as it processes, click on the Text Window button. When this button is depressed, a window will appear that displays the posted text f ile as it is created. The program will scroll by in the window as it is being generated. The Pause button allows the user to stop the scrolling of the output as it is being processed. The Print button will be available after the program f ile is f inished processing.

83

Post Processing

Before posted output can be generated, the post processor and program f ile name must be specif ied. When a f ile is post processed, a text f ile is created with the extension specif ied in the Post text box in the File Extension dialog. By default, this extension is set to .NCF. A f ile can be post processed multiple times and saved with different .NCF f ile names. If changes are made to the part f ile, it must be post processed again in order to incorporate the changes into the posted output. As a default, the text f ile uses the part f ile name with an .NCF extension (e.g. EXAMPLE1.NCF). This f ile name can be changed by clicking on the Program Name button and entering a new name.

To specify an output f ile name for the f inished program, click on the Program Name button. The system will automatically add the extension specif ied in the File Extension dialog. Selecting the File tab from the Preferences dialog will display the File Extension dialog shown above.

To select the post processor, click the Post Selection button. An Open dialog will appear that allows the user to access the directory or folder where the post processors are stored in the system.

The actual f ile names of the post processors are different depending on the operating system. However, when selecting a post processor, the full name (including the Control and Machine) will be displayed in the Open dialog.

POSTED OUTPUT FORMAT

The items in the top box of the Post Processor dialog change the format and contents of the f inished output.

Each item can react differently with different post processors. Below is a description of the effect they will have with most post processors.

Selected Ops: Checking this item will cause the output to only include operations that are currently selected in the Operations list. Items that are unselected will not be output.

Starting Program Number: This is the number of the program as it will appear in the control. It is also the starting number for all sub-programs. If the Starting Program Number is one, the f irst sub-program will be two, the second three, etc.

Sequence from: This is the starting number for the block numbers or “N� numbers. The by box determines the increment.

Minimize: If this option is turned on, the post processor will only output block numbers on tool change positions.

Insert Comments: This option will output information about each operation and tool used as well as f ile length.

If any additional comments have been entered by the user about tools or operations, they will be output as well.

Insert Optional Stops at Tool Change Positions: If this option is on, the software will output a machine operator selectable program stop at every tool change.

84

Post Processing

POST OUTPUT PREFERENCES The Post Processing preference allows the user to specify comment data that is output in the NCF f ile generated by the system. If an item is checked, that data will be output. This dialog can be found in the File menu under Preferences -> Post Processor Comments.

LATHE POST LABEL DEFINITIONS AND CODE ISSUES Lathe post names use letters to signify their capabilities. The designation may be a single letter or multiple letters to specify the post's capability. Following the letter designation is a unique number for this post.

The general format of a post can be described as: <control name><machine name>[client initials]<letter>###.## Note that a metric post will end with an â&#x20AC;&#x153;mâ&#x20AC;?.

Following is a description of how Lathe Posts are named and what they do. Also included are brief explanations of code issues that might be encountered in Lathe Posts.

2-AXIS LATHE Label Definitions L This designates a regular 2-axis turning post. A Lathe post has 2 linear axes (X and Z) that can position and cut simultaneously.

Example:

Fanuc 16T [VG] L800.18.pst

85

Post Processing

Code Issues: â&#x20AC;˘

Tool Tip 1.

The system draws the toolpath to the center of the tool tip radius. The X and Z-axis values are output to the theoretical tool tip if the system is able to calculate a touch-off point in both axes. X or Z-axis values are output to the center of the tool tip radius when the software is not able to calculate the touch-off point in that particular axis.

2. If the tool is machining parallel to the Z-axis, the X values are output to blueprint dimensions. If the tool is machining parallel to the X-axis, the Z values are output to blueprint dimensions. So, the theoretical tool tip only aligns with blueprint dimensions on faces and diameters.

3. When the tool is machining at an angle, the X and Z-axis values will not match the blueprint dimensions. This is because the theoretical tool tip is not always a blueprint dimension. So, in order for the system to get the surface of the tool in position to cut the part, the theoretical tool tip is calculated closer to the part, and in some cases inside the part.

4. Most Lathe Posts output X and Z values to the theoretical tool tip. Posts can be modif ied to output X and Z values to the center of the tool tip radius. â&#x20AC;˘

Canned Cycles 1.

Lathe canned cycles are output when the Prefer Canned checkbox is checked. This checkbox will only be available if Auto Clearance and Material only are not selected. If Auto Clearance and/or Material Only are selected, the system will not output Canned Cycles.

3 & 4-AXIS MILL/TURN A Mill/Turn post supports both milling and turning operations in the same part. A 2-axis lathe post is no longer needed if a Mill/Turn post is available.

Label Definitions: ML This designates a Mill/Turn post.

S

This designates a Mill/Turn post that segments rotary arcs into linear moves.

Example:

Fanuc 16T [VG] SML800.19.pst

I This designates a Mill/Turn post that supports Polar and Cylindrical Interpolation. A Polar and Cylindrical Interpolation Mill/Turn post will output a G2 or G3 with rotary moves.

Example: Y

Fanuc 16T [VG] IML800.19.pst

This designation is for a 4-axis Mill/Turn machine that has a linear Y-axis.

Example:

Fanuc 16T [VG] YIML800.19.pst Fanuc 16T [VG] YSML800.19.pst

P This designates a C-axis positioning post. A Mill/Turn positioning post will rotate the part and then move in X and Z. It will not rotate and cut simultaneously.

86

Post Processing

Example:

Fanuc 16T [VG] PML800.19.pst

N This designates a Mill/Turn post that does not use subprograms. This is known as a “Long Hand post”.

Subprograms are frequently used for multi-process drilling, C-repeat drilling, Z-repeat milling, C-repeat milling, Patterns (OD only), etcetera.

Example:

Fanuc 16T [VG] NSML800.19.pst Fanuc 16T [VG] NIML800.19.pst

B This designates a B-axis rotation post. This supports the creation of coordinate systems that has the tool rotate about the B-axis.

Example:

Super Hicell 250 HS [JMC] BSML1082.19.7.pst

Code Issues: •

Tool Orientation 1.

•

When using a mill tool on the Face or OD, it is important to def ine the orientation of that tool correctly. When Milling or Drilling on the face, make sure the orientation of the tool is perpendicular to the face. When Milling or Drilling on the OD, make sure the orientation of the tool is perpendicular the OD. If the tool is not oriented properly, the output will not be correct.

C-Axis And Y-Axis Output 1.

The radio buttons Position and Rotary Milling in the Rotate Tab determine whether C-axis moves or Yaxis moves are output during Rotary Mill operations. If the Position radio button is selected, the system calculates Y-axis moves. If the Rotary Milling radio button is selected, the system calculates C-axis moves.

2. If your machine does not have a Y-axis, then you need to select the Rotary Milling radio button.

3. If your machine has a Y-axis, this capability can be added to any Mill/Turn post.

•

Rotary Feedrates 1.

Most rotary feedrates are calculated in Degrees Per Minute per rotary segment based on its length.

Since the length of each segment is variable, the system outputs a different feedrate for each segment.

The resulting rotary feedrate can be a large value based on the Degrees Per Minute calculation.

2. Certain CNCs, such as Haas and Mazak, calculate rotary feedrates using Inverse Time. Any Mill/Turn post can be modif ied to use Inverse Time for feedrates.

3. Polar Interpolation posts use inches per minute for rotary feedrate calculations. Any Mill/Turn post can be modif ied to use Polar Interpolation with inches per minute feedrates.

87

Post Processing

88

COMMUNICATIONS

Communications

CHAPTER 9 : Communications ABOUT COMMUNICATIONS The system contains integrated communications. Third party communications packages can also be used to communicate with CNC machines.

Before a f ile can be sent to the CNC machine, the parameters for a f ile transfer need to be set-up. This is done in the Com Set-Up tab in the Preferences sub-menu of the File menu. This dialog is used to set up communication protocols needed for sending a program (text f ile) to a control or receiving a program from the control. Different controls have different protocols (parameters). Refer to the machine control manual for the necessary protocol specif ications.

PROTOCOLS ADDING A PROTOCOL A new protocol is added by typing in a new name and changing all of the settings to match those of the CNC machine. Clicking on the Add button will add the protocol to the current database of protocols.

91

Communications

After a protocol has been added, the name will appear in the upper left hand corner.

Additional protocols can be entered and saved in the same manner. Saved protocols can be accessed in the Protocol pop-up menu in the upper left-hand corner of the dialog.

CHANGING A PROTOCOL To change information about a protocol, select the protocol from the list and change the information. The changes are automatically saved when the dialog is closed or when a different protocol in the list is selected.

REMOVING A PROTOCOL

To remove a protocol, simply select the desired protocol from the list and click on the Remove button.

COMMUNICATING WITH A CNC MACHINE To send a f ile to or receive a f ile from a CNC machine, click on the Communications button in the Post Processor dialog.

COMMUNICATIONS DIALOG

The Communication dialog can also be accessed from the File menu. Files can either be sent to the machine control or received from the control. The File type radio buttons indicate what type of f ile will be sent. When a f ile is post processed, a text f ile (NCF f ile) is created. NCF (text) is the necessary selection when sending posted NCF f iles from the computer to the control or vice versa. The VNC (binary) selection allows users to send and receive VNC f iles, which are the actual part f iles that contain the geometry and toolpaths. VNC f iles can be communicated between computers that have the system installed. This is especially useful when the system is built into the control of a machine tool. Part f iles (VNC f iles) can be communicated in their entirety from a computer to the machineâ&#x20AC;&#x2122;s control, and from the control back to the computer.

SENDING A FILE TO THE CONTROL To send a f ile, the Send Mode button must be depressed. The protocol is chosen by using the Protocol pop-up menu. The program to be sent is specif ied by clicking on the Program Name button. When everything is set correctly, click on the Send button to send the f ile. While the program is being sent, the Send button becomes the Stop button. Click on the Stop button to stop the communication. The Progress Bar shows the status of the 92

Communications

1.

2.

3.

4.

5.

Send Mode Receive Mode Program Name Protocol Menu Progress Bar

f ile being sent. If the Text Window is opened from the Post Processor dialog, the program will scroll by as it is being sent to the control.

SENDING OTHER .NCF FILES

Any text f ile that matches the extension set in the Post text box in the File Extensions Preference can be sent to the control. Refer to the Post Processing chapter for more information on output f ile extensions.

RECEIVING A FILE FROM THE CONTROL

To receive a f ile from the control, open the Communication dialog from the Post Processor dialog or from the File menu. The Receive Mode button should be depressed. Choose the correct protocol from the Protocol popup menu. The name of the received program is specif ied by clicking on the Program Name button. When everything is set correctly, click on the Receive button, and then send the program from the control. If the Text Window is open from the Post Processor dialog, the program will scroll by as it is received.

It is recommended that edited NCF f iles received back from the machine control be saved under a different name than the original NCF f ile that was initially sent to the control. That way if the original VNC f ile is reprocessed, it won't affect the edited NCF f ile. For example, a part f ile named SAMPLE.VNC is post processed and a text f ile named SAMPLE.NCF is created. Changes are made to the program at the machine control and the new f ile containing those changes is sent back and received at the offline computer, but under the name SAMPLE1.NCF. If SAMPLE.VNC is reprocessed again at a later date, it won't destroy the SAMPLE1.NCF f ile that contains the changes that were made at the machine.

93

Communications

94

LATHE TUTORIAL

Lathe Tutorial

CHAPTER 10 : Lathe Tutorial The Lathe module is the most basic of the turning machines supported by the system. This chapter provides instruction on how to create turning operations. Covered in this chapter are tool setup, process def inition, operation creation, custom stock def inition, cut part rendering and form tool use.

Most of this information is covered in “Exercise #1: Lathe Tutorial” while “Exercise #2: Form Tools” primarily covers creating and using a form tool.

EXERCISE #1: LATHE TUTORIAL The following tutorial shows how a simple lathe part is set up, tooled and output. Each step is bulleted and additional information and tips are also provided. It is recommended that all the information contained in this tutorial is read to gain the most thorough understanding. This part was created in the Geometry Creation manual and the dimensions for this part are also on page 135. Refer to the Geometry Creation manual for details on constructing the Geometry for this part. You may convert the measurement units with the Modify > Scale command if necessary.

1.

Set up stock, clearance and tool change settings

2. Specify custom stock 3. Create a tool list with standard and custom tool settings 4. Generate different types of operations that rough, contour, drill and thread a part.

5. Render the machining operations.

6. Create posted code for the part.

PART SETUP •

Exercise #1: Lathe Tutorial

THIS TUTORIAL EXPLAINS HOW TO:

Open the Documents dialog.

The Document dialog contains information about the Machine Type, Material, measurement system, stock, Tool Change, clearance and a part Comment. It also has the f ile management tools to open, save, close, etc.

•

Select Open in the Documents dialog.

•

Locate the Lathe tutorial part that was created using the Geometry Creation manual.

This part was created in both the Geometry Expert and Free-Form CAD Exercises in the Geometry Creation manual. Either of the part f iles can be used. If the part was not created, go back to the Geometry Creation manual and do so or use the dimensions at the end of the book to create the geometry.

•

Click the file then click Open or double-click Lathe Tut.vnc in the list.

97

Lathe Tutorial

•

Select the Auto Clearance option.

Auto Clearance defaults the clearance values of each process unless overridden by unchecking Use Auto Clearance in the Process dialogs.

The Auto Clearance option will calculate part clearances (in both Z and Xd/Xr) that are used to position the tool between operations. These values are dynamically calculated as the stock condition changes as material is removed. The clearance positions calculated will also take into account where the tool needs to move to begin the next operation’s toolpath. Additionally, the Auto Clearance option may add entry and exit moves as needed to safely maneuver around the part and complete each toolpath.

Exercise #1: Lathe Tutorial - Part Setup

•

Enter the stock, Auto Clearance and Tool Change positions shown.

Tool Change will send the tool to the specif ied location for the tool change. If Tool Change is turned off, it is assumed that f ixture offsets are being used or the operator will manually input the tool change moves.

•

Close the Document dialog (Ctrl+1, F1, Ctrl+W).

•

Open the View palette (Ctrl+5, F5).

•

Choose Help > Balloons from the menu.

Balloons provide a reference to the interface. A check mark will appear next to the Balloons item, indicating that it is on. Move the cursor over the object to see the information.

•

Select Unzoom (Ctrl+U).

The part may already be unzoomed if the part was saved.

•

Select the Isometric view (Ctrl+I).

The Isometric view is a 45° perspective of the part. This view gives the best overall perspective of the current status of a part from the top, right and front view of the part.

The Top or Home view is recommended for creating geometry and toolpaths, while the Isometric view is an excellent choice for rendering and viewing the cut part.

•

Choose Help > Balloons to deactivate them.

Balloons are also activated by using the associated shortcut to the right of the menu command (Ctrl+B).

98

Lathe Tutorial

•

Switch back to the Top view.

•

Click the View button again to close the View palette.

CUSTOM STOCK The stock specif ications entered in the Document dialog simply creates a cylindrical stock shape using the X and Z coordinates entered. It is possible to def ine a custom stock shape by drawing the stock shape in a separate workgroup designated for part stock. This is very useful because the stock shape affects the machining of the part in that the stock conditions are used to calculate the clearance positioning moves when using Auto Clearance. The custom stock shape also appears when viewing the rendered image of the part.

Open the Geometry palette. (Ctrl+2, F2)

•

Click the Workgroup list button in the Geometry Creation palette.

In Level 2 this can be accessed from the main palette.

This button also accesses a workgroup selection menu if the mouse button is held down. The menu will be discussed later in this tutorial.

•

Click New WG and rename it “Stock”.

A second workgroup is created and is now the current workgroup, indicated by the open eye. Also, notice that the screen now displays an empty stock outline.

•

Right click the name of the workgroup, choose WG Info.

The Workgroup #2 dialog def ines whether the workgroup will contain part geometry or a stock outline.

•

Select the Part Stock Revolve option.

•

Close the Workgroup #2 Info dialog.

Exercise #1: Lathe Tutorial - Custom Stock

•

In order to create the geometry for the stock outline, it will be necessary to view the part geometry that we have already created as a machining workgroup. The entry highlighted in the Workgroup Selection dialog is the active workgroup.

Other workgroups can be viewed by opening the eye next to their name in the Workgroup Selection dialog. Geometry in inactive workgroups are gray and can not be edited while inactive.

99

Lathe Tutorial

•

Double-click the closed eye next to Workgroup #1.

Both eyes are now open. Workgroup 2: Stock is highlighted to indicate that it is the active workgroup. Workgroup #1 is visible but inactive.

•

Close the Workgroup list.

Exercise #1: Lathe Tutorial - Custom Stock

We will use the Mouse-line tool in the Geometry Creation palette to draw a rough outline of the stock. Any geometry creation method can be used to create a stock outline.

100

•

Click the Line button.

•

Click the Mouse-Line button.

The Mouse-Line dialog contains Z and Xd values determined by the location of the cursor. The Grid value specif ies constraint spacing the lines will snap to. For a review on using the Mouse-Line tool, refer to Exercise #5: Doodle in the Geometry Expert Section of the Geometry Creation manual.

The initial stock is a cylinder with two different diameters for our stock outline. The stock does not need to be perfect, but should not cross the f inish geometry def ined. The only condition is that the bottom line must be drawn at X0 to have a correctly revolved part.

•

Draw a stock shape around the part as shown.

This will be the stock condition before cutting is preformed.

•

Hold the Workgroup Selection button down until the selection menu appears.

•

Select Workgroup 1.

•

Close the Geometry Creation palette.

Lathe Tutorial

TOOL LIST •

Open the Tool list button in the Top Level palette.

•

Double-click tile position #1 in the empty tool list.

The Tool Creation dialog contains all tool specif ications necessary for the system to calculate accurate toolpath and rendering. Tool information can be edited at any time by clicking on tool tiles and editing the information contained in the Tool dialog. For more information, refer to “Tool Creation Overview” on page 13.

•

Select the 80° C insert with the following specifications.

Holders can be chosen by using the scroll bar next to the insert diagram. The text to the right of the scroll bar displays the holder specif ications which provide detailed information about the insert angle and holder type. For our part, the f irst position provides the desired selection. The red circle at the end of the insert indicates the touchoff point of the tool.

The selection of insert and tool holder also affects the toolpaths created using this tool.

The system uses the selections made here when constructing a toolpath to prevent tool interference. Therefore, selections made here directly affect the machining of the part.

•

Exercise #1: Lathe Tutorial - Tool List

Values for insert specif ications, such as Tip Radius, IC (Inscribed Circle), Thickness, etc. can either be selected from the list of standard inserts in the menus or manually entered by selecting Other.

Double-click the empty tool tile at position #2.

This closes the Turning Tool #1 dialog and brings up the Turning Tool #2 dialog. A tool tile displaying the insert type and tip radius appears in position #1 of the tool list.

This next tool is a drill, so it must be def ined in a Milling Tool dialog.

•

Click the Milling Tool button.

101

Exercise #1: Lathe Tutorial - Tool List

Lathe Tutorial

102

•

Select the Drill specifications.

•

Double-click tile position #3 in the Tool List.

•

Click the Turning Tool type button.

•

Select the 35° V diamond insert.

•

Enter the tool information shown.

tool

with

the

following

The position on the insert orientation diagram remains the same as the previous insert selection, so no adjustment is necessary.

The insert angle and holder type selection is the last one in the group.

Lathe Tutorial

â&#x20AC;˘

Create this insert as tool #4.

Double-click the tool tile to open the new tool dialog. We will skip this step from here on.

Create this custom insert as tool #5.

The tool holder diagram is set to Custom.

Only the insert is drawn in the diagram according to the values entered.

Exercise #1: Lathe Tutorial - Tool List

â&#x20AC;˘

103

Lathe Tutorial

•

Create this insert as tool #6.

The Insert Orientation Diagram changes in appearance when the Boring Bar option is selected.

Exercise #1: Lathe Tutorial - Tool List

•

104

Scroll down to reveal two empty tiles (if necessary).

The scroll arrows at the top and bottom of tile lists allow you to easily move through the tiles in the list. To scroll quickly through the list, hold down the button and drag the mouse downward. This will change the arrow to red and scroll a “page” at a time. Refer to the the Getting Started guide for more information on tile lists.

•

Create this insert as tool #7.

Once the Style and TPI (threads per inch) values are selected, the Insert Width and Insert Type will default to the desired values.

Lathe Tutorial

•

Create this custom insert as tool #8.

•

Close the Turning Tool #8 dialog.

The tools necessary to machine this part have now been created. A good way to review the tools contained in the list is by using the Window > Tool List Summary.

Choose Window > Tool List Summary.

The Tool List Summary contains all of the current tool information.

The information may be printed by choosing File > Print > Tool List Summary. While the Tool List Summary is the active window the print shortcut Ctrl+P will work. The list is set up to print in landscape mode ONLY. When any of the summaries are displayed on the screen, they can be printed or saved as a text f ile with the Save Special command.

•

Close the Tool List Summary.

Exercise #1: Lathe Tutorial - Tool List

•

105

Lathe Tutorial

CREATING THE OPERATIONS - OD â&#x20AC;˘

Click the CAM button in the Main palette.

Exercise #1: Lathe Tutorial - Creating the Operations - OD

The Machining palette, Process List and the Operation List appear.

106

The Machining palette contains Function tiles. The functions available for use with lathe are contouring, roughing, threading, and drilling.

Process tiles are created by dragging a Tool Tile and a Function Tile to a Process List location. Operation tiles are created from Process tiles when the Do It or Redo button is depressed.

In order to machine this part, operations must be created. Operations are created from completed processes. To create a process, one tool and one process (roughing, contouring, drilling, threading) is needed. In this tutorial, we will f irst describe the necessary machining operation, then we will detail the steps necessary to create that operation.

First, we will create an operation that will face the front of the part. â&#x20AC;˘

Select the Contouring Function Tile

and drag it to position #1 in the Process list.

Lathe Tutorial

•

Drag tool #1 (80° C) and drag it to position #1 in the Process List. Place it on top of the Contouring tile in position #1.

When you place the Tool Tile in position #1, the tool number is displayed in the small box on the Contouring Process Tile. The Contour Process dialog appears after the Tool tile is added.

Enter the information shown in the Contour dialog.

To position the tool to cut the face of this part, we need the tool to approach and retract along the Z axis. Therefore, the Front Face option is selected.

For this process, the Material Only option is selected so no toolpath will be generated unnecessarily to cut the face.

•

Close the Contour Process dialog.

When the Process dialog is complete, the cut shape must be def ined. Machining Markers (shown below) are used to designate a cut shape for contouring processes.

•

1.

2.

3.

4.

5.

6.

7.

Start point Offset cut Start feature End Point End Feature Centerline cut Direction

Exercise #1: Lathe Tutorial - Creating the Operations - OD

•

Select the vertical line at Z=0.

The Machining Markers will appear on the selected feature. The markers allow you specify the start and end feature and the start and end point of the cut shape. They can be “picked up” by clicking on them and dragging them to any location on the part geometry. The arrows allow you to choose the cut direction. The two circles allow you to choose the side from which the tool will be offset.

107

Lathe Tutorial

In this case, the start feature and end feature markers will stay in their initial positions because only one feature, the face, will be cut. The start point and end point markers will be moved to cut the entire length of the face. The start and end point markers can rest anywhere on the selected line, even on the trimmed sections. Refer to the Machining Markers section in the Machining chapter for more information.

•

Select the outside circle.

Exercise #1: Lathe Tutorial - Creating the Operations - OD

This is the OD side of the geometry.

108

•

Click the arrow pointing down.

We will approach the line from the OD and bring the tool just past the center to ensure a complete facing is done.

•

Drag the start point marker above the workspace as shown.

Because Material Only is used in this process, the start and end point markers do not need to be placed in exact positions as long as they clear the stock outline we def ined.

•

Drag the end point marker down to the location shown.

If markers are not properly placed a process may not generate the desired toolpath.

The common mistake is to chose the wrong cut side.

•

Click the Do It button in the Machining palette.

An Operation tile will be created and added to the Operation list and the approach and retract moves and the toolpath drawn. The orange lines represent the toolpath, while the

Lathe Tutorial

dashed gray lines represent positioning moves. The solid lines for both the toolpath and positioning indicate feed moves. And the dashed lines of both colors indicate rapid moves.

The angled lines at the beginning and end of the toolpath are entry and exit positioning moves that have been added because Auto Clearance is turned on. They are angled along the centerline of the insert angle. The position the tool can safely rapid to before beginning the toolpath is determined by the Auto Clearance value entered in the Document dialog. â&#x20AC;˘

Deselect the operation created by clicking on an empty Operation location, or by clicking an insertion point between Operation locations.

Tiles are considered selected when they are highlighted in yellow. Deselected tiles are the standard gray color.

CREATING OPERATIONS

Exercise #1: Lathe Tutorial - Creating Operations

The picture above on the right shows the toolpath without the Machining Markers so you can get a better picture. To view the toolpath without the Machining Markers, simply click anywhere off the part. The dashed gray line shows the tool rapiding from the tool change position (entered in the Document dialog, to the start point of the toolpath).

When operations have been satisfactorily completed, it is VERY IMPORTANT before proceeding that all operations are deselected. By deselecting the completed operations, they become f ixed in the Operations List and will not be affected by changes made to the Process List. Operations can be edited, but to do so they must be reloaded into the Process List by double-clicking on them. â&#x20AC;˘

Drag the Process in position #1 to the Trashcan.

When creating a new Process, you can either throw away the old tiles in the list or modify them in order to create the new operations. In this case we will throw away the old tile and start from scratch.

Every tile in the Process list will be used to create operations.

109

Lathe Tutorial

The next group of operations will rough and f inish the outside contour of the part. This will be accomplished using multiple process programming which allows multiple process tiles to be applied to one cut shape.

Multiple Process Group Op 2-4

Exercise #1: Lathe Tutorial - Creating Operations

â&#x20AC;˘

Create this Rough process with tool #1.

To properly position the tool to rough the OD of this part, we need the tool to approach and retract along the X axis.

Therefore, the OD option is selected for the approach type.

Lathes use different roughing (multiple cut) cycles. There are three general types: Turn, Plunge, and Pattern Shift. These three types of cycles will allow us to output the different canned cycles def ined in programming manuals for lathes. The software will output these roughing cycles as canned cycles if the Prefer Canned option is selected and the lathe is capable of using canned cycles. If not, the post processor will output every move necessary to rough the part.

Turn roughing cycles are the standard contour rough cycle. For turning cycles, the selection made for the approach type (OD, ID, Front Face) determines what type of contour rough style will be generated by the system.

Plunge roughing cycles are used to generate grooving operations. These cycles are used when it is desirable to rough the part with a groove tool. Pattern Shift roughing cycles are commonly used when roughing a cast part. This type of cycle generates the part contour and shifts the toolpath on each successive cut until the specif ied area is roughed.

In this process, we will use a turn roughing cycle. When a turning cycle is selected, a Cut Depth value is entered which designates how much material will be removed on each pass.

For this process, the Cut Depth value entered is 0.1. The Xr label indicates that it is a radius value. This means that 0.1" of material will be removed from each side on each pass.

The Shape Axes check boxes allow the user to regulate the axes and directions of the cut shape.

Omitting an axis (such as X-) will prevent cut shape moves in the disallowed direction. Refer to the Machining chapter for more information on cut shapes and the Shape Axes buttons.

For this process, the X axis in the negative direction is turned off. This will prevent the toolpath from making any moves in the X- direction so it doesnâ&#x20AC;&#x2122;t go into the grooves.

110

Lathe Tutorial

The value entered in the Fin. Stock ± text box designates the minimum amount of material that will be left outside of the part geometry after the roughing cycle is completed. The toolpath created by the system will be offset from the part geometry in Z and in Xd. We will remove this excess with the f inish pass.

•

Close the Rough Process dialog.

•

Create another Roughing Process with tool #3 in position #2.

Material Only is again selected for the Rough Style so that the toolpath generated for this operation will only cut the remaining material left on the part after the previous operations have been completed. The Material Only selection is particularly useful when utilizing the multiple process programming capabilities of the system. Feed moves will only be made where it is necessary to remove material. The tool will make rapid moves whenever possible while maintaining the clearance offset.

In addition to entering a f inished stock amount which will leave the designated amount of material around the entire cut shape.

•

Exercise #1: Lathe Tutorial - Creating Operations

This process is included in this group to rough the neck groove on the part. Again, an OD approach type is selected so the tool will approach and retract along the X axis. And a Turn rough cycle is selected using a Cut Depth.

Close the Rough Process dialog.

111

Exercise #1: Lathe Tutorial - Creating Operations

Lathe Tutorial

•

In position #3 create this Contour process with tool #3.

•

Close the Contour Process dialog.

Now that the Process List is complete, we will def ine the cut shape.

•

Click the chamfer as shown.

The Machining Markers will appear on the selected feature.

•

Click the outside circle.

•

Click the arrow pointing up.

•

Drag the Start Point Marker to the position shown.

The Start and End Point Markers do not need to be placed in exact locations as long as they clear the material.

•

Drag the End Feature Marker (black square) and drop it on the part geometry as shown.

The End Point marker will automatically move with the End Feature marker.

Alternately the End Feature Marker can be placed by pressing Ctrl+Shift and clicking on the end feature geometry.

When positioning any one of the four machining markers on a geometry feature, place the tip of it’s arrowhead on the geometry feature.

112

Lathe Tutorial

•

Drag the end point marker to the position shown.

The Dark blue line represents the cutting path. Notice that the middle V groove and the O-ring groove are not included in this cut shape.

•

Click the Do It button.

Three operations are created.

The Operation list should have four operations now.

The positioning moves and toolpaths for each of the operations are also drawn on the screen. In order to get a better picture of the toolpaths generated by the system, we will view the tool moves for the f irst roughing operation separately.

•

Select Operation #2.

Clicking once on a tile will select and highlight the tile without opening any dialogs or selecting other tiles that were created with it.

•

Exercise #1: Lathe Tutorial - Creating Operations

This will create the toolpath. If any mistakes were made, edit the process and use the Redo button to make changes to a selected operation.

Open the View Control palette.

113

Lathe Tutorial

•

Click the Redraw button (Ctrl+R).

Exercise #1: Lathe Tutorial - Creating Operations

Only the toolpath and positioning moves for the selected operation are drawn. This is helpful if you use multiple process programming and wish to view individual toolpaths.

Notice that the custom stock outline was taken into account because Auto Clearance is on and the Material Only option was selected. Also, the toolpath created does not slope at all into the neck groove because the X- Shape Axis was deselected in the Rough Process dialog that created this operation.

The dashed gray lines show the tool rapiding from the end point of the previous operation to the start point of this operation, and to the tool change position at the end of the operation.

Now that operations have been created, we will render the part. There are several ways to verify that the toolpaths generated by the system will safely and correctly cut the part. Looking at the toolpaths, as we have done thus far, is one way. Another way is to render the part which allows you to actually view the tool removing material and cutting the part.

•

Choose View > Isometric.

•

Open the Rendering palette.

This changes the working mode to Cut Part Rendering. The initial stock we def ined at the beginning will display as a solid object. The Geometry is hidden but can be viewed by using View > Show Geometry ( Ctrl+[ ).

•

Click the Play button.

The Cut Part Rendering palette shown below also appears on the screen.

•

114

Click the Show Solid Tool button.

Lathe Tutorial

•

Click the Play button.

A part can be rendered at any time once operations have been created. The stock will always be shown in shades of blue. Selected operations will render in shades of yellow, while all other operations will render in shades of gray. Red will be displayed when noncutting tool surfaces or rapid moves hit the material.

Refer to the Cut Part Rendering chapter for more information.

Close the Rendering palette.

•

Choose View Top from the menu or Ctrl+E. This is also the same as the Home view in CS1.

•

Deselect the operations by clicking on an empty operation location or by clicking on an insertion point between operation locations.

•

Shift select the three tiles in the Process List and drag them to the trash.

You may also use the Delete key.

Exercise #1: Lathe Tutorial - Creating Operations

•

115

Lathe Tutorial

Multiple Process Group Op 5-8 •

For Process 1 create this Rough process with tool #4.

Exercise #1: Lathe Tutorial - Creating Operations

An OD approach type is selected so the tool will approach and retract along the X axis. Material Only is again selected for the Rough Style. Also, a Finished Stock amount is left on this groove that will be removed in the following f inish pass.

In this process, we will use a Plunge roughing cycle.

When the Plunge option is selected for the Rough Type, the Plunge dialog will come up on the screen. To make the Plunge dialog come up, click the Plunge option in the Rough Type selections.

•

Enter the information shown below in the Plunge dialog.

The Plunge Angle specif ies the angle at which the groove tool will make its plunging moves. The default is 270° which has the tool plunging straight down.

For this process, we have selected the Details option for the Cut Width.

This option will vary the Cut Width distance as necessary in order to hit the endpoints of each feature of the cut shape. The Z value entered specif ies the maximum distance the tool will step over on each pass.

The Center Out Cuts option is selected so that the tool will make its f irst plunging move in the center of the groove, and then proceed to rough each side.

For this groove, the Peck Full Out option is selected because the groove is relatively deep, and in order to remove all of the chips (material), the tool will need to come all the way out of the part after the peck. The value entered in the Peck Amt text box specif ies the distance the tool will plunge into the part on each peck. The Clearance value specif ies the distance away from the remaining material the next peck will begin.

116

Lathe Tutorial

â&#x20AC;˘

For Process 2 create this Contour process with tool #4.

The No Drag option is turned on in this process so that the toolpath is created in such a way that only the positive insert angle of the tool cuts material. The designated cut shape is segmented into pieces to accomplish this.

For Process 3 create this Rough process with tool #5.

An OD approach type is selected so the tool will approach and retract along the X axis. Material Only is again selected for the Rough Style. Also, a Finished Stock amount is left on this groove that will be removed in the following f inish pass.

Plunge is selected for the Rough Type.

Exercise #1: Lathe Tutorial - Creating Operations

â&#x20AC;˘

117

Lathe Tutorial

•

Enter the information shown below in the Plunge dialog.

Exercise #1: Lathe Tutorial - Creating Operations

The Exact option is selected for the Cut Width. The tool will step over on each pass regardless of the endpoints of the cut shape. The Peck Retract option is selected for the First Plunge. The Peck Amt specif ies the depth of each plunge and the Retract amount specif ies the distance the tool will come out of the groove after each peck.

118

•

For Process #4 create this Contour Process with tool #5.

Now we will def ine the cut shape for this process list.

•

Click the part geometry as shown.

The Machining Markers will appear on the selected feature.

Lathe Tutorial

•

Right-click the last feature shown and choose Move End Feature here so the Machining Markers appear as shown.

Make sure you select the outside circle and the arrow pointing left. The blue cut shape drawn should include the V groove and O-ring.

Create the toolpath.

The toolpaths that are created will properly rough and f inish both the V groove and the O-ring. Notice that the toolpath contains no unnecessary moves. Material Only takes full advantage of multiple process programming without making unnecessary tool moves.

•

Switch to the Isometric view. (Ctrl+I)

•

Render the Operations.

During the rendering process, you will be able to better see the No Drag contour option at work. Notice the tool will f inish one side of the groove, rapid up and over, and then go down and f inish the other side of the groove, always cutting along the positive direction of the insert angle.

•

Exit Rendering mode.

•

Switch to the Top view (Ctrl+E).

•

Deselect any operations.

•

With the Process list selected choose Edit > Select All (Ctrl+A) and delete the tiles or drag them to the Trashcan.

Exercise #1: Lathe Tutorial - Creating Operations

•

Except for the thread, the OD of our part is complete.

119

Lathe Tutorial

CREATING THE OPERATIONS - ID Now, we will create the operations to drill a hole through the center of the part and rough and f inish the ID.

Multiple Process Group Op 9-11

Exercise #1: Lathe Tutorial - Creating the Operations - ID

â&#x20AC;˘

120

Create this Holes process with tool #2.

The depth the drill will feed to is specif ied by the value entered in the Sharp Tip Z text box. Values may be entered in the text boxes specifying the Full Diameter Z depth and the Spot Diameter.

These values will cause the Sharp Tip Z to be recalculated. The Sharp Tip Z is the value used in the posted output.

The drill cannot feed through the part in one pass. Therefore, the Peck, Full Out option is selected. Because it is a Peck, Full Out, the drill will rapid all the way out of the part after each peck.

The value entered in the Peck text box specif ies the amount the tool will peck into the material on each pass. The next peck will start a Clearance amount away from the material remaining after the previous peck.

Remember to use the Balloons in the Help menu if you donâ&#x20AC;&#x2122;t understand the f ields.

Drilling operations do not require the selection of geometry. In a standard lathe a drill can only feeds in at X=0. Therefore, the placement of the Machining Markers will only affect the toolpath created for the Roughing and Contouring operations.

Lathe Tutorial

â&#x20AC;˘

For Process #2 create this Rough Process with tool #6.

A Front ID approach type is selected so the tool will approach and retract from the part along the X axis. A Turn Rough Type is selected and separate stock amounts are entered for each axis.

For Process #3 create this Contour process with tool #6.

The Front ID approach type is selected and Material Only is turned on in the process.

Exercise #1: Lathe Tutorial - Creating the Operations - ID

â&#x20AC;˘

121

Exercise #1: Lathe Tutorial - Creating the Operations - ID

Lathe Tutorial

122

•

Position the Machining Markers as shown.

•

Create the toolpath.

The dashed orange line at X = 0 shows the tool rapiding out of the part after it has pecked in to the Sharp Tip Z depth in the Drilling operation.

•

Switch to the Isometric view.

•

Render the Operations.

•

Deselect the operations.

•

Clear the Process list.

We will skip stating these last two steps in the future.

•

Switch back to the Top view.

Lathe Tutorial

THREADING Op 12 Next, we will create the operation that will cut the required thread.

•

Create this Thread process with tool #7.

These values can be found in the Machinery’s Handbook, and are calculated from the values entered for an “ideal thread.”

Const Load is selected to maintain the same amount of tool pressure on each pass. The Last Cut option is selected to prevent any cut from removing less than the value entered from each side. This is also the cut depth that the threading tool will remove on the last pass.

Threading operations do not require the selection of geometry.

The information entered in the Thread dialog determines where the thread will be located on the part.

•

Create the toolpath.

Exercise #1: Lathe Tutorial - Threading

The Minor Xd will default to a calculated value according to the Nominal Xd and the desired pitch. The Thrd Ht Xr is calculated [(Major Minor)/2]. Changing the Nominal Xd will change the values in the Major Xd, Minor Xd, and Thrd Ht Xr.

123

Lathe Tutorial

CUT OFF Op 13 Finally, we will create an operation to cut off the machined part from the bar stock.

•

Create this Contour Process with tool #8.

Exercise #1: Lathe Tutorial - Cut Off

An OD approach type is selected so the tool will approach and retract along the X axis. Material Only is selected for the Rough Type with a Clearance of 0.25. The Clearance value is relatively large to ensure that no tool interference occurs with our f inished part.

124

The Cut Off option is turned on so the post processed output will contain the necessary codes for removing the part from bar stock. Not all post processors support this option.

•

Close the Contour Process dialog.

•

Select the cut off line of the part and position the Machining Markers as shown.

Ensure the end point extends past X0 and the start point begins above the stock.

Lathe Tutorial

•

Create the toolpath.

As the last step we will sort the operations to have less tool changes.

•

Right click an operation in the Operations List and choose “Sort Ops.” The only change that occurs is the Drilling operation that uses Tool #2 will be moved up in the Operation List to location #3.

•

Select the Isometric view. (Ctrl+I)

•

Render the Operations (F6).

For this case, changing the order of the operations does not cause any tool interference and does not appear to affect the eff iciency of the toolpath and positioning moves generated by the system. Had there been any problems, we would have needed to reprocess the existing operations so that the system would have recalculated the tool moves for each operation based on the new conditions. Reprocessing the operations is very easy using the Redo All Ops item in the Edit menu or the Operation list context menu.

Exercise #1: Lathe Tutorial - Cut Off

Whenever the order of operations is changed, it is good practice to verify that the positioning moves and toolpaths are still valid. When using the Auto Clearance option and/or Material Only option, the material condition is taken into account when it creates the tool moves for each operation. Changing the order of operations has the potential to change the initial material conditions for existing operations.

Rendering the part is a good way to check the validity of the toolpaths.

125

Lathe Tutorial

POST PROCESSING Now that all of the operations to machine the part have been satisfactorily created and verif ied, we need to post process the f ile. Post processing will create a text f ile that the CNC machine will use to cut the part.

•

Open Post Processor dialog.

Exercise #1: Lathe Tutorial - Post Processing

From the Post Processor dialog a post processor may be selected as well as generating a post f ile and communicating with a machine control. Refer to the Post Processing and Communications chapters for more information.

•

Click the Post Processor Selection button.

•

Select a Lathe post processor.

•

Click the Open button.

The name of the selected post processor will appear in the dialog next to the button.

•

Click the Program Name button.

The Program Name defaults to the name of the part f ile. You can change the name or leave it as it is.

•

Click the Save button.

Once you have selected a post processor and named and saved the program, the Process button at the bottom of the dialog becomes active.

•

126

Click the Text Window button.

Lathe Tutorial

This allows you to view the posted code as it is processing. â&#x20AC;˘

Click the Process button.

This will create a post f ile that can then be sent to the machine.

The program will scroll by as it is being processed. You can click the Pause button to momentarily stop the processing so that you can read the program. Once the program has f inished processing, the Print button becomes active and the posted code can be printed.

Exercise #1: Lathe Tutorial - Post Processing 127

Lathe Tutorial

EXERCISE #2: FORM TOOLS This exercise introduces you to creating and using Form Tools in GibbsCAM. We will start with an existing, very simple part f ile, create a Form Tool and apply a machining operation using the Form Tool.

•

Open the part file Form Tool.vnc located in the Tutorial Parts folder that was installed with the software.

Exercise #2: Form Tools - Post Processing

The f ile contains geometry for the part, a tool and two roughing operations. The existing operations face and rough the part. First we need to create geometry for the Form Tool.

128

•

Create a new workgroup for the Form Tool.

•

Use the data in “Form Tool Blueprint” on page 136 to create the geometry for the form tool.

Remember that the system uses the origin as the tool’s touch-off point. The tool should look like this image.

•

Open the tool dialog.

•

Select Form tool as the tool type.

Lathe Tutorial

You are prompted to select a shape to use for the tool’s prof ile.

•

Double click the Form Tool geometry and click Apply.

The shape of the tool is displayed in the Tool dialog. Note the touch-off point is shown in the tool diagram.

We will now make a contour process using the form tool.

•

Create this Contour Process with the form tool.

Exercise #2: Form Tools - Form Tool Contour

FORM TOOL CONTOUR

129

Lathe Tutorial

â&#x20AC;˘

Position the machining markers as shown.

Exercise #2: Form Tools - Form Tool Contour

We have placed the start point marker above the roughed surface. The end point marker should be on the connecting point to drive the tip of the tool to that point.

130

Since we are contouring on a single line some options become disabled when using a Form tool. â&#x20AC;˘

Create the toolpath.

Lathe Tutorial

The result should be a single feed line into the part.

Switch to the Isometric view and render the results.

â&#x20AC;˘

Save this part, it is complete.

Exercise #2: Form Tools - Form Tool Contour

â&#x20AC;˘

131

Exercise #2: Form Tools - Form Tool Contour Lathe Tutorial

132

PART PRINTS

135

Part Print 1: Tutorial Part Blueprint

136

Part Print 2: Form Tool Blueprint

INDEX

Index

SYMBOLS % of Body’s Chord Height: 79

C C.A.T.: 3 Canned Cycles: 40, 44, 46, 55–56, 61

NUMERICS 3D Real Time Cut Part Rendering: 73

A Advanced CS Module: 8 Air Cutting: 26, 34, 39, 61 Approach Type: 9, 56 Changing: 56 Contour: 31 Front Face: 56 Front ID: 56 OD: 56 Roughing: 36 Thread: 42

Chord Height: 79 Circular Threads: 80 Clearance Auto, see Auto Clearance Contour operations: 31 Data: 7 Diagrams: 56 Fixed: 9 Fixed, see Fixed Clearance Master: 31 Moves: 55 Clearance Moves: 9, 39, 55 Approach From Tool Change: 57 Exit To Tool Change: 58 Same Tool Moves: 59 Clearance Positioning: 55

Auto Clearance: 9, 27, 31, 39–40, 45, 55–56, 61, 98

Clearance Positions, Entry and Exit: 56 Close File: 8

B

CNC, Communication with: 92

Balloons: 98

Collision Alerts: 79 Tolerance: 80

Bar Stock: 32

Collision, Flash CPR: 79

Body Chord Height: 79

Com Set-Up dialog: 91

Button Close: 8 Do It: 26 Document Control: 7 Machining: 25 Material: 44, 46 New: 8 Open: 8 Post Processor: 83 Receive: 93 Redo: 26 Save: 8 Save As: 8 Save Copy: 8 Send: 92 Tool List: 13

Comment: 9

Back & Forth Roughing: 36

Communication Stop: 92 Communication dialog: 92 Communication Protocol Change: 92 New: 91 Remove: 92 Constant Cut: 43 Constant Load: 43 Constant Surface Speed, see CSS Contour Cutter Compensation: 20 Contour Feed: 35 Contour process: 31 Contour Style: 34 139

Index

Rigid Tap: 44 Sharp Tip Z: 45 Spot Diameter: 45 Surface Z: 45 Tap: 44

Full: 34 Material Only: 34 Contouring function: 27, 31 Control Receiving files from: 93 Sending files to: 91

Drilling Function: 27, 44

Coolant: 35, 40, 46

Drilling Process: 44

Corner Break: 34, 40

Dwell: 46

CPR: 74 Controls: 74

E

CPR palette: 74 CRC: 20, 34 CSS: 35, 40 Current Display (CPR): 74 Cut Depth: 37 Thread: 43

Entry Clearance Contouring: 32 Position: 56 Roughing: 39 Entry Move 90° arc: 32 Contour operation: 34 Line: 32

Cut Direction: 36 Cut Direction Axes: 35, 41 Cut Off: 32 Cut Part Chord Height: 79 Cut Shape: 26

Exit Clearance Contouring: 32 Roughing: 39

CutDATA: 8, 64 Cutter Radius Compensation, see CRC Cycle Start Point: 38

F Face Relief: 18

D Decimal Slope: 47 Depth Of Cut: 43

Feed Move: 56 Plunge rate: 46 File Send to Control: 92

Diameter Relief: 18

File Extension: 84

Diameters, part size: 9

File Management: 7

Do It: 52

Find Operation: 67

Document Control dialog: 7, 31, 39, 55, 97, 99

Finish Stock ±: 34, 40

Drill Entry/Exit Cycle: 44

Fixed Clearance: 40, 55–56

Drilling: 120 Diagram: 45 Dwell: 46 Feed In-Feed Out: 44 Feed In-Rapid Out: 44 Full Diameter Z: 45 Peck Chip Breaker: 44 Peck Full Out: 44

Form Tool: 17

140

Forward: 32 From Tool Center (CRC): 20 From Tool Edge (CRC): 20 Front Face Approach Contour: 31 Roughing: 36

Index

Width: 16

Front ID Approach Contour: 31 Roughing: 36

Insert Comments (Post): 84 Insert Type: 14

Full Radius: 16

Invisible Tool (CPR): 74

Function Tile: 31

Isometric view: 98

G G50 Offset: 9

L Last Cut: 43

G50 offset: 19

Lathe Inserts: 14

G-code: 26

List

Gouge Avoidance, see Cut Shape

H

Operation: 25 Process: 25 Scroll Arrows: 104 Tool: 13

Help: 3 Holder Diagram: 18 Specs: 18

M Machine Type: 8

Holders Boring Bars: 15 None: 15 Tool Holder: 15

Machinery’s Handbook: 49, 123

Hole Diameter: 45

Machining palette: 25, 27

Machining Markers: 25–26, 62, 107 How To Use: 62 On Geometry: 63

I ID (Inner Diameter) Thread: 42–43 In Feed: 43 Balanced thread: 48 Insert Face Angle: 16 IC (inscribed circle): 16 Insert Type: 16 Material: 19 Orientation diagram: 18 Positive Angle Direction: 32 Size: 16 Specifications: 15 Specifications of: 14 Thickness: 16 Thread Style: 17 Tip Width: 17 TPI: 17

Making Operations Geometry: 25 Material Database: 8, 19, 44, 64 Material Only: 9, 26–27, 34, 39, 61 Clearance: 39 Material Only, Clearance: 34 Max RPM: 35 Measurement Units: 8 Mill Class, back end holder: 9 Mill Module: 8 Mill Tools: 14 Mill/Turn Module: 14 Minimize (Post): 84 Mouse-Line: 100 Move Operation: 67 Multi-Level Sort: 68 Multiple Process Creation: 26 Multi-Task Machining Module: 8, 14 141

Index

N NC program: 27 NCF file: 92 New File: 8 Next Operation (CPR): 74 No Air Cutting, see Air Cutting No Drag: 32 Nominal Thread diameter, see Thread, Nominal Xd NPT: 47 Chart: 50 Cutting: 49

Cycle Start Point: 38 Fixed: 38 Passes: 38 Square Corners: 38 Xr Cut: 38 Z Cut: 38 Pause Posting: 83 Peck Amount: 45 Chip Breaker: 45 Clearance: 46 Full Out: 45 Retract: 45 Play (CPR): 74–75

O

Operation List: 25–27

Plunge Angle: 37 Center Out Cuts: 37 Clearance: 38 Cut Width: 37 Feed: 37 First Plunge: 37, 39 Peck Amount: 38 Peck Full Out: 38–39 Peck Retract: 38–39 Retract: 38

Operation Tile: 27

Plunge dialog: 37

Operations: 109 Deselecting: 26 Order of: 27 Reprocessing: 13, 27

Post From Part File: 83 Name: 84 Output: 84 Requirements: 84 Selection: 84 Unit Conversion: 8

OD (Outer Diameter) Thread: 42 OD Approach Contour: 31 Roughing: 36 Offset # (Tool): 18 One Finish Pass: 43 Open File: 8 Operation Data: 65

Optional Stops (Post): 84

P Part Comment: 9 Material: 8 Set Up: 7–8 Stock: 9

Post Output Preferences: 85 Post Processing: 83 Post Processor Coolant: 46 Custom: 32, 35, 40, 44, 46 Drilling Cycles: 44

Part Clearance Master: 56

Prefer Canned: 40, 44, 46, 55, 61 Auto Finish: 40

Part Surface in Z: 45

Preset Point: 19 see also Touch-off Point

Part X Dimension: 9 Pattern Shift 142

Print Post: 83

Index

Printing: 21, 80

S

Process Loading Saved: 52 Post: 83 Stock Amount: 20

Save Duplicate Copy: 8 File: 8 File As: 8 Special: 21

Process dialogs: 31 Contour: 31 Rough: 36 Thread: 42

Saving Processes: 52 Saving Tool Data: 52

Process Group: 52 Pre-defined: 52

Selected Ops (Post): 84 Send Mode: 92

Process List: 25–27, 31, 67

Sending a File: 92

Program Name button: 92 Program Name, post: 83

Sequence from (Post): 84 Set Op Stop #: 75

Prompting: 3

Shank Size: 9

Protocols: 91

Slope, see Thread, Taper Sort Operations: 27, 67

R Radii, part size: 9 Radius Move, contouring: 32 Rapid Move: 56 Step: 39–40

Speed: 44 Spindle Speed: 35, 40 Spring Pass: 43 Square Corners: 32, 38 Start Side Extension: 36 Starting Program Number (Post): 84

Redo: 13

Statistics, Flash CPR: 80

Redo All Ops: 27, 34, 39, 125

Step Forward (CPR): 74–75

Render, checking the part: 27

Steps Per Update: 79

Rewind (CPR): 74

Stock Finish: 34 Xr: 34 Z: 34

Rough process: 36 Rough Style: 39 Full: 38–40, 61 Material Only: 39–40

Stock Size: 7, 9

Rough Type: 37 Cut Depth: 110 Pattern Shift: 37–38, 40, 56 Plunge: 37 Plunge Rough: 37 Turn: 37, 40, 56

Stop (CPR): 74–75

Roughing function: 27, 36

Theoretical Tool Tip, see Touch-off Point

RPM: 44, 46

Thread # of Starts: 43, 47 1st Xr: 48 Actual End: 44

Run In: 42, 44 Run Out: 42, 44

Surface Z: 45

T Text Window, post: 83

143

Index

Actual Start: 44 Alternate In Feed: 43, 48 Approach Type: 47 Balanced In Feed: 43, 47 Constant Cut: 48 Constant Load: 48 Cut Direction: 42, 47 Depth of Cut: 43, 48 End Z: 48 Front ID: 42 Height Xr: 43, 47 ID: 47 Last Cut: 48 Major & Minor Xd: 43, 47 Nominal Xd: 42–43, 47 OD: 42, 47 One Finish Pass: 48 Run In: 48–49 Run Out: 49 Spring Pass: 48 Start Z: 48 Style: 42, 47 Taper: 42, 47 Thread Angle In Feed: 43, 48 TPI: 42, 47

Summary: 21, 105 Tool Movement: 55 Tool Specifications, modifying: 13 Tool Tile: 25, 31 Tool Type Toggle: 14 Toolpath: 26 Cutter Side and Direction: 62 End Feature: 62 End Point: 62 Recalculate: 27 Start and End Points: 62 Start Feature: 62 Start Point: 62 Touch-off Point: 17–18 Transparent Tool (CPR): 74 Trashcan: 109 Turret Shift: 19, 55

U Undo: 52 Units of Measurement: 8 Utility data: 65

Thread Angle: 43

V

Thread Clearance: 42 Thread Load: 43

Visible Tool (CPR): 74

Thread Process: 42

VNC file: 92

Threading: 42, 47 Threading function: 27

W

Threads Per Inch, see Thread, TPI Throttle Control (CPR): 74 Tool Comment: 19 Custom, see Form Tool Offset: 20 Other: 16 Radius Offset: 20

Work Fixture Offset: 9

X X Dimension Style: 9 X Stock Start, roughing: 39 Xr Stock: 34, 40

Tool Change: 9, 55, 98 Tool Change Position: 7, 19 Primary: 55 Tool Creation dialog: 13–14 Tool List 144

Z Z Depth Full Drill Diameter: 45

Index

Tool Tip: 45 Z Stock: 34, 40

145

Index

146