R11 2 whats new by Mrx Man

SolidCAM2007 R11.2

SolidCAM

Power and Ease of Use - the winning combination

SolidCAM2007 R11.2 What’s New

WW W. S O L I D C A M . C O M

SolidCAM2007 R11.2 What’s New

Document number: SCWNENG07003

Contents

Contents 1. General

1.1 GCode Generation......................................................................................8 1.2 Coordinate Systems.....................................................................................15 1.3 Item search in the SolidCAM Manager tree.............................................20 1.4 Generating a copy of the operation..........................................................22 1.5 Sequential numbering of the operations in SolidCAM Manager.........23 1.6 Operation renaming.....................................................................................24 1.7 Split.................................................................................................................25 1.8 Adding tools in the View page...................................................................26 2. 2.5D Milling

2.1 Delta Depth option in 2.5D Milling..........................................................28 2.2 New features in Thread Milling Operation..............................................30 2.3 Defining the Lead Out strategy same as Lead In strategy.....................33 2.4 Drilling depth type.......................................................................................34 3. 3D Milling

3.1 Trochoidal milling........................................................................................36 4. High-Speed Machining Module

4.1 HSM Combined Strategy............................................................................38 4.2 Tangential pass extension...........................................................................41 4.3 Rest machining.............................................................................................42 4.4 Tool path trimming when ramp is used....................................................44 4.5 Absolute ramp height..................................................................................45 4.6 Tangential position of the tool on the working area..............................47 4.7 Miscellaneous parameters...........................................................................48

5. Simultaneous 5 Axis Machining

5.1 Tool................................................................................................................50 5.2 Levels.............................................................................................................52 5.3 Geometry.......................................................................................................54 5.4 Surface quality options in Finish parameters...........................................66 5.5 Link Macro....................................................................................................68 5.6 Tool axis control...........................................................................................71 5.7 Gouge check.................................................................................................72 5.8 Roughing........................................................................................................75 5.9 Extra Parameters..........................................................................................81 6. Turning

6.1 Generating sketch for the Material boundary..........................................84 7. Wire Cut

7.1 Definition of Insertion point using points of the CAD sketch...........86 7.2 Automatic definition of Start point for multi-chain geometry.............87 8. Machining Processes

8.1 New Turn-Mill Machining Process table type.........................................90 8.2 Tool definition and search in Machining Processes................................91 9. Automatic Feature Recognition Module

9.1 Using color information to assign technology........................................98

General

1.1 GCode Generation In the previous versions of SolidCAM, the GCode files were generated in the CAM-Part folder. A new functionality has been added to enable you to choose a location other than the CAM-Part folder and common for all the CAM-Parts, into which the GCode files will be generated. 1.1.2 Temporary GCode file generation The temporary GCode file is generated using the operation interface by clicking on the GCode button in the Operation dialog box.

In this case, the GCode file is generated in the CAM-Part folder regardless of SolidCAM Settings. The generated GCode file is opened in the text editor determined by SolidCAM Settings. When you close the Operation dialog box, the file is removed. To save the temporary GCode file, use the text editor functionality.

General

1.1.3 GCode generation using SolidCAM Manager The right-click menu available on the Operations header in the SolidCAM Manager tree contains two commands to generate the GCode file for a complete CAM-Part: Calculate & GCode All and GCode All, Generate. For one or several operations, you can generate the GCode file by right-clicking on the single operation or the group of selected operations and choosing the Calculate & GCode or GCode, Generate commands from the menu. The GCode files location defaults are found on the GCode Generation page of the SolidCAM Settings dialog box. These defaults are applied to every newly created CAM-Part. If you want to modify these settings for each Part separately, SolidCAM offers you a similar page in the Part Settings dialog box. 1.1.4 Part Settings dialog box The GCode Generation page enables you to define the parameters of the GCode generation. The Save GCode files box offers three options to define the parameters related to saving of GCode files: In the CAM-Part directory SolidCAM saves the generated GCode files in the CAM-Part directory. The path to this directory is displayed in the read-only field. This option is used by default. According to the MAC file SolidCAM saves the generated GCode files according to the parameters defined in the MAC file (see topic 1.1.5). The path to the directory that appears in the MAC file is displayed in the read-only field.

In the GCode directory SolidCAM saves the generated GCode files in the specified GCode folder location. When the GCode generation is started, SolidCAM creates a new folder with the CAM-Part name in the specified GCode directory and saves the GCode files there. If this folder already exists, SolidCAM uses it for the GCode output. This group box enables you to define the path for the GCode directory. You can enter the path or click on the Browse button and choose the destination folder using the Browse for Folder dialog box. If you have entered the path to a non-existing folder, the following message is displayed after the confirmation of the SolidCAM Settings dialog box:

The Create button enables you to create the folder that will be used for GCode directory in the specified location. The Browse button displays the browser dialog box that enables you to choose another location that will be used for the GCode directory. If the new folder cannot be created, the following message is displayed:

If the chosen folder has the read-only attribute, the following message is displayed after the confirmation of the Browse dialog box or the SolidCAM Settings dialog box:

General

By default, the GCode directory location is not defined. You have to specify it when you choose the Save GCode files in the GCode directory option for the first time. Create subfolders for split GCode files

When split marks are detected in SolidCAM Manager during the GCode generation for the entire CAM-Part, SolidCAM creates a number of GCode segment files. Each such GCode segment file is created for one or several operations enclosed by split marks. These files are named with the CAM-Part name followed by the â&#x20AC;&#x153;-â&#x20AC;? sign and an the order number of split segment. Split marks are ignored in case of GCode generation for several operations. With the In the GCode directory option, SolidCAM creates separate CAM-Part GCode folders in the specified folder location. When the Create subfolders for split GCode files check box is selected, SolidCAM creates a separate folder for each GCode segment file and saves the GCode segments files there. The folder is created in the GCode folder of the CAM-Part in the specified GCode folder location. The name of the folder is the same as the GCode segment file name. When the Create subfolders for split GCode files check box is not selected, SolidCAM generates all the GCode segment files directly in the GCode folder of the CAM-Part in the specified GCode folder location. By default, the Create subfolders for split GCode files option is not selected.

Create separate folders for each CAM-Part

When this check box is selected, SolidCAM creates a folder for each CAM-Part and saves the GCode file there. Otherwise, the GCode files for all CAM-Parts are generated into the GCode directory. Additional control of GCode When this check box is selected, you can alter the GCode file name and location. When you click one of the GCode generation commands, the Windows-style Save GCode browser is displayed with the default CAM-Part name and location that might be edited.

All the GCode files previously generated for the current CAM-Part remain in the specified folder. When this check box is not selected, the GCode is generated and automatically saved in the defined location.

General

Do not erase old GCode when generated for CAM-Part/for operations These check boxes enable you to choose whether the old GCode file generated for the entire CAM-Part or for separate operations remain or are removed when a new one is generated. The

Do not erase old GCode when

generated for CAM-Part

check box is

not available if the Additional Control of GCode check box is not selected.

1.1.5 MAC file parameters Three new variables related to the GCode generation have been added: dir_gcode, split_gcode_folders and gcode_part_subfolder. These variables are used when the According to the MAC file option is chosen in the Part Settings dialog box. dir_gcode This string variable contains the path for the GCode location. For example, dir_gcode = C:\GCode\

When a non-existing folder is assigned to this parameter, the following message is displayed during the GCode generation attempt:

The Create button enables you to create the folder that will be used for GCode directory at the specified location.

split_gcode_folders This boolean variable controls the creation of separate folders for split GCode files. For example, split_gcode_folders = Y

When the variable is set to Y, SolidCAM creates a separate folder for each GCode segment file and saves the GCode segment files there. The folder is created in the GCode folder of the CAM-Part in the location specified by the dir_gcode parameter. The name of the folder is the same as the GCode segment file name. When the variable is set to N, SolidCAM generates all the GCode segment files directly in the GCode folder of the CAM-Part in the location specified by the dir_gcode parameter. The default value of the split_gcode_folders variable is N. gcode_part_subfolder This boolean variable controls the creation of separate folders for different CAMParts. For example, gcode_part_subfolder= Y

When the variable is set to Y, SolidCAM creates a separate folder for each CAM-Part for which you generate the GCode. This separate folder is created in the GCode folder of the CAM-Part and has the name of this CAM-Part.

G-Code Cavity Cavity.tap Mold Mold.tap Wire Wire.tap

When the variable is set to N, the GCodes for all parts are generated into the directory specified by the dir_gcode parameter in the MAC file.

G-Code Cavity.tap Mold.tap Wire.tap

General

1.2 Coordinate Systems provides you with enhancements in the definition and editing of coordinate systems for Milling and Wire Cut. You are presented with several new options related to placing the Coordinate System, picking the origin and the directions of the axes directly on the model, rotating and moving the CoordSys according to a series of parameters to be defined. SolidCAM2007 R11.2

1.2.1 Defining the CoordSys by selecting a face When you define the Coordinate System by selecting a face, the box surrounding the model is calculated. For this box, SolidCAM generates a number of sketch points to facilitate the CoordSys definition. The points are located in the box corners, in the middle of each edge and in the centers of the planes (in the intersection point of the diagonals).

Placing of the CoordSys origin Two new options related to placing of the CoordSys origin have been added. Top center of model box

After you select a face, the CoordSys origin is placed in the center of the upper plane of the model, and the Z-axis of the CoordSys is normal to the selected face.

Corner box projection on Z-level of face

After you select a face, the CoordSys origin is placed in the corner of the generated model box on the same Z-level with the selected face, and the Z-axis of the CoordSys is normal to the selected face.

General

Picking the CoordSys on the solid model and flipping the axes After the face has been selected, you have several new options that enable you to edit the Coordinate System location by picking entities on the model and changing the directions of the axes. Pick XY origin

This option enables you to define a new location for the CoordSys origin in the XY-plane by picking a point on the model. The Z-level of the CoordSys origin and the directions of the axes remain the same. Pick Y direction

This option enables you to choose a new direction for the Y-axis by picking a point on the model. Flip Around Z

You can rotate the defined CoordSys 90 degrees around the Z-axis. Moving and rotating the CoordSys Delta

This option enables you to move the CoordSys origin in the X-, Y-, and Z-coordinates relative to the point in which it was previously defined. Rotation around axis

This option enables you to rotate the defined CoordSys a given number of degrees around the X-, Y- and Z-axes, but the rotation can only be defined around each axis separately. You cannot rotate the CoordSys around more than one axis simultaneously. 17

1.2.2 Defining the CoordSys normal to current view

This option enables you to define the Coordinate System with the Z-axis normal to the model view you are facing on your screen. You may bring the model to the desired orientation by using the CAM Views toolbar or just rotate it in an arbitrary fashion; then click on the Capture Current View CoordSys button, and the Coordinate System will be generated relative to the model view you are using. The CoordSys origin will lie in the origin of the SolidWorks Coordinate System, and the Z-axis will be directed normally to the chosen view of the model. Y-axis of the Normal to current view CoordSys

X-axis of the Normal to current view CoordSys

You may change the location of the CoordSys using the placing options of the Select face mode, and then choose the Normal to current view mode to adjust the directions of the axes to the current model view.

General

1.2.3 Create planar surface at Part Lower level In some cases you need to select sketch points that do not lie on the solid model entities, such as in definition of insertion point for wire cutting. SolidWorks does not allow picking points beyond the model surface, therefore a new Create planar surface at Part Lower level option has been added to help you overcome this problem. This option enables you to generate a transparent planar surface at the minimal Z-level of the Part so that its lower level plane is visible. This planar surface is suppressed by default and not visible until you unsuppress it in the FeatureManager Design tree.

This option is available only when the Coordinate System has been defined by selecting a face.

1.3 Item search in the SolidCAM Manager tree Starting with SolidCAM2007 R11.2, you can search the SolidCAM Manager tree for items related to the CAM-Parts and their operations, geometries, and so forth. The new SolidCAM search system works similarly to a regular Windows searching functionality. To activate it, click anywhere in the SolidCAM Manager area and press Ctrl+F. The Find dialog box is displayed, and you can set the parameters for searching.

Look in You may look for the required items in the whole CAM-Part or only in its operations, coordinate systems or geometries taken separately. Whole items only Select this check box if you want to check the availability of whole items as opposed to partial output. Match case This check box enables you to determine the case sensitivity of the search. Direction You may also decide whether the search results will be displayed from bottom to top or from top to bottom of the SolidCAM Manager tree. Find Next Click this button if you want to view the search results one by one. Find All Click this button if you prefer to have all of the search results to be displayed simultaneously.

General

The whole line where the sought-for word appears is highlighted in the SolidCAM Manager tree. When you close the Find dialog box, these lines remain highlighted.

1.4 Generating a copy of the operation enables you to generate a copy of a specific operation inside the Operation dialog box. SolidCAM2007 R11.2

The Save & Copy command saves the current operation data and automatically creates a new operation with the same parameters. The new operation is automatically opened for editing. Using the Save & Copy functionality you can quickly create a new similar operation where most parameters are identical.

General

1.5 Sequential numbering of the operations in SolidCAM Manager enables you to assign sequential numbers for items (operations, splits and fixtures) in the SolidCAM Manager tree. SolidCAM2007 R11.2

When the

Use automatic numbering of SolidCAM

Manager items option is activated in the SolidCAM

Manager page of the SolidCAM Settings dialog box, all the items in the SolidCAM Manager will be numbered.

When a new item is defined between two existing items, SolidCAM performs renumbering in order to assign to each item an updated sequential number.

1.6 Operation renaming SolidCAM2007 R11.2 enables

you to rename a specific operation.

To rename a specific operation, right click on the operation name in the SolidCAM Manager and choose the Rename command from the menu. The Operation name dialog box is displayed. This dialog box enables you to assign a new name for the operation.

General

1.7 Split provides you with extended functionality of splits; by giving a name to the split it can act as a folder containing operations, fixtures etc. SolidCAM2007 R11.2

When a split is added, SolidCAM displays the Split dialog box where you enter the name of the split. The (-) icon located near the Split icon in the SolidCAM Manager enables you to collapse/expand all the items (operations and fixtures) that are located under the split. The right-click menu available on split items provides you with the capabilities to rename the actual split (the Rename command) and to suppress/unsuppress all the items (operations and fixtures) that belong to the split (the Suppress/Unsuppress commands).

1.8 Adding tools in the View page In previous SolidCAM versions it was possible to add a new tool into a tool table only in the Edit page of the Tool table dialog box. SolidCAM2007 R11.2 enables you to add tools into a tool table also in the View page.

When you click on the Add button, a new tool is created. The Tool Table dialog box is switched to the Edit page which displays the parameters of the new tool.

2.5D Milling

2.1 Delta Depth option in 2.5D Milling In previous SolidCAM versions, to assign an offset to the cutting depth defined associatively to the model, the user had to break the associativity and change the depth value. SolidCAM2007 R11.2 provides you with the ability to define an offset for the cutting depth. By adding this parameter, SolidCAM enables you to change the cutting depth while preserving its associativity.

is always relative to the Depth defined for the operation. Suppose the depth of your pocket is 12 mm, and you want to mill it 0.5 mm above its floor. If you define an offset of 0.5 mm for the Delta depth, even if the model changes and the depth of the pocket becomes greater, the pocket will be milled 0.5 mm above the floor. Delta depth

2.5D Milling

If the value of Delta depth is positive, a blue arrow is displayed near its field indicating a positive offset value (in the positive direction of the Z-axis).

If the value of Delta depth is negative, a red arrow is displayed near its field indicating a negative offset value (in the negative direction of the Z-axis).

2.2 New features in Thread Milling Operation 2.2.1 Tool technology tables offers you a quick and efficient solution in terms of thread pitch definition. You do not need to use external sources to find the Pitch values conforming to the ISO, Whitworth and other standards. The table of Standard values is embedded into the SolidCAM tool definition interface. SolidCAM2007 R11.2

When a thread tool is chosen in the Part Tool Table, the Pitch/Standard field becomes available. In this field, there is a list of Standard tables according to which you may want to define the thread pitch.

When you choose one of the standards from the list, the corresponding table is displayed in a separate window.

2.5D Milling

You may open the threading table as an Excel file and edit its content. The location of this file can be found on the User directories page of the SolidCAM Settings dialog box.

2.2.2 Support of conical tools Starting with the current version, SolidCAM has extended its capabilities for support of various tool types by adding conical thread tools into the existing list of supported tools. This enhancement enables you to cut threads in taper holes as well as in cylindrical holes.

2.2.3 Deepening the existing thread If the depth you have defined for threading of hole is insufficient, SolidCAM provides you with a new option that enables you to deepen the threading by a certain value. On the Levels page of the Thread Mill Operation dialog box, there is a new Additional depth section in which you may define the deepening of your thread.

In the Deeper field, enter the additional depth value required. Start from beginning When you have added a certain depth to be thread-milled, there is in some cases a need to start the cutting of the thread from the beginning. This is possible with the Start from beginning check box in the Additional depth field. For example, you thread-milled one drill hole out of 10 identical holes to a certain depth. Then you found that the threading is not deep enough, and added a certain additional depth. Then you thread-milled the hole again (without starting from the beginning, because there is no point in cutting the thread again where it is already cut) and made sure that the depth is now satisfactory. To thread-mill the rest of the holes, you need to start cutting from the very beginning, because these holes were not previously machined, as the first hole. 32

2.5D Milling

2.3 Defining the Lead Out strategy same as Lead In strategy SolidCAM2007 R11.2 provides you with the capability to define the Lead Out strategy

same as Lead In strategy.

The Same as Lead in option is available in the dialog box of 2.5D Milling operations.

Lead out

group of the Operation

With this option, SolidCAM uses for the Lead Out the same strategy and parameters that are defined for Lead In.

2.4 Drilling depth type provides you with an updated functionality of the Depth type option in the Drill operations (formerly Use Chamfer option). SolidCAM2007 R11.2

The following Depth types are available: • Cutter tip.

With this option the drill tip reaches the defined Drill Depth.

• Full diameter.

With this option the drill reaches the defined with the full diameter.

Drill Depth

• Diameter value.

With this option the drill reaches the defined Drill Depth with the drill cone diameter specified by the Diameter value parameter. The Diameter value can vary from 0 all the way up to the drill tool diameter. A value greater than the drill tool diameter is automatically decreased to the drill tool diameter. Drill depth

Drill depth

Diameter value Cutter tip

Full diameter

Diameter value

3D Milling

3.1 Trochoidal milling provides you with the advanced functionality in the Trochoidal milling feature. The algorithm of the trochoidal milling is improved taking into account a new Engagement angle parameter located in the Trochoidal dialog box. SolidCAM2007 R11.2

The Engagement angle is the angle measured between two vectors describing the area of contact between the tool and the machined material.

Engagement angle

During the calculation, SolidCAM checks the engagement angle at each tool position defined by Step parameter. If the engagement angle is greater than the specified Engagement angle value, SolidCAM at this position performs a circular tool movement with the radius defined by the Radius parameter. If the engagement angle is smaller than the specified Engagement angle, SolidCAM does not generate a circular movement at this position; the tool is moved to next position.

High-Speed Machining Module

4.1 HSM Combined Strategy SolidCAM2007 R11.1 has introduced the new option to combine two machining strategies in a single HSM operation: the combination of the Constant Z strategy supplemented with the secondary Horizontal strategy. offers two additional combined strategies: or Constant StepOver machining.

SolidCAM2007 R11.2 Linear

Constant Z

with

To activate any of the combined strategies, do the following: In the Technology box of the HSM Operation dialog box, choose the Combine Constant Z and then the relevant item from the submenu.

The two combined machining strategies share the Geometry, Tool and Constraint boundaries data. The technological parameters for the passes calculation and linking are defined separately for each strategy.

High-Speed Machining Module

The Constant Z Passes page defines the parameters of the Constant Z machining strategy.

The Linear Passes and Constant Stepover Passes pages define the parameters of the Linear/ 3D Constant Stepover strategies.

The following parameters, defined on the Constant Z Passes page, are automatically assigned the same values on the Linear passes / Constant Stepover passes pages: •

Thickness

•

Axial thickness

•

Tolerance

•

Z_Top

•

Z_Bottom

When these parameters are edited in the Constant Z Passes page, their values are updated automatically in the Linear passes / Constant Stepover passes page. But when edited in the Linear passes / Constant Stepover passes pages, the values in the Constant Z Passes page remain unchanged. Two Link pages, located under the Constant Z Passes and Linear passes / Constant Stepover passes pages, define the links relevant for each of these strategies. In the Link page for Linear passes / Constant Stepover passes, there is a Machining order tab that enables you to define the order in which the Constant Z and Linear / Constant Stepover machining will be performed. The default option is Constant Z first. When the tool has finished performing the passes of the first machining strategy, it goes up to the Clearance level, then descends back to the machining surface to continue with the next strategy.

High-Speed Machining Module

4.2 Tangential pass extension provides you with the new Tangential extension option that enables you to extend the passes tangentially to the model faces by a length defined by the Passes extension parameter. This option is available for Linear and Radial machining technologies. SolidCAM2007 R11.2

When the Tangential extension option is not active, the extension passes are generated as a projection of the initial pattern (either linear or radial) on the solid model faces. When the Tangential extension option is activated, the extension passes are generated tangentially to the solid model faces. Extension

Extension

Extension Tangent extension is turned off

Tangent extension is turned on

4.3 Rest machining 4.3.1 Spiral on surface machining strategy An additional strategy to machine shallow areas has been added. The Spiral on surface strategy links the passes with smooth curved paths resulting in continuous passes and reducing the rapid moves. The spiral linking move is projected into the rest corner up to the maximal depth of the cut specified.

High-Speed Machining Module

4.3.2 Machining steep or shallow areas separately In the previous SolidCAM version, SolidCAM enabled you to determine steep and shallow areas of the model using the Steep threshold parameter. The machining of the steep and shallow areas was performed using different strategies inside a single Rest machining operation. provides you with the Areas option. This option enables you to decide whether to perform the machining in the steep areas only, in the shallow areas only or in both of them.. SolidCAM2007 R11.2

• Shallow. With this option, the machining is performed only in the shallow

areas (the surface inclination is less than the Steep threshold value).

• Steep.

With this option, the machining is performed only in the steep areas (the surface inclination is greater than the Steep threshold value).

• All.

The machining is performed in both steep and shallow areas.

4.4 Tool path trimming when ramp is used provides you with a new option enabling you to control ramp movements connecting Constant Z passes. The Trim to ramp advance option enables you generate a helical style finish when linking Constant Z passes. SolidCAM2007 R11.2

When this option is chosen, the Constant Z pass above which a ramp linking movement is performed is trimmed by the length of the ramping move. In such a way a helical style tool path is generated, avoiding the unnecessary cutting moves at the already machined areas and maintaining a constant tool load. Constant Z passes

Ramp movements

If the Trim to ramp advance option is not chosen, the whole Constant Z passes are linked with the ramp movements.

Constant Z passes

Ramp movements

High-Speed Machining Module

4.5 Absolute ramp height provides you with a new functionality for the definition of the height from which the ramping motion is started for the upper profile of the 3D Constant Stepover tool path. SolidCAM2007 R11.2

In previous SolidCAM versions, this height was defined relative to the upper profile height with the Ramp height offset parameter. SolidCAM2007 R11.2 enables you to define also the absolute start position for the ramp motion with the Ramp height parameter measured from the Coordinate System origin.

The following options are available: â&#x20AC;˘ Relative height. With this option

the start position of the ramp motion for the upper Constant Stepover pass is defined relative to the first point of the pass using the Ramp height offset parameter.

Ramp height offset

â&#x20AC;˘ Absolute height.

With this option, the start position of the ramp motion is defined with the absolute Ramp height value measured from the Coordinate System origin.

Ramp height

CoordSys

These options are available only for the strategies.

Helix

and

Profile ramping

High-Speed Machining Module

4.6 Tangential position of the tool on the working area provides you with a new option that enables you to control how the tool is positioned relative to the boundaries of the working area. SolidCAM2007 R11.2

When the Tangent option is chosen, the tool path is limited in such a way that the tool is tangent to the model faces at the boundary. This option enables you to machine the exact working area, taking into account the 3D model geometry. Tool on working area: Tangent

4.7 Miscellaneous parameters With SolidCAM2007 R11.2, the new to the HSM Operation dialog box.

Miscellaneous parameters

page has been added

This page contains the following options: â&#x20AC;˘ Extra Parameters

In case there are special operation options implemented in the postprocessor used for the current CAM-Part, the Parameters List button enables you to display the list of additional parameters defined in the post-processor. â&#x20AC;˘ Message

This option enables you to enter a message that will appear in the generated Gcode.

Simultaneous 5 Axis Machining

5.1 Tool 5.1.1 Use Rapid feed Some 5-axis CNC machines do not support synchronization between axis motors when the rapid movement (G0) is performed. The absence of synchronization causes the deviation between the calculated path and the real tool movements. SolidCAM2007 R11.2 provides you with a new functionality that enables you to avoid the problems described above by replacing all rapid movements (G0) with nonrapid ones using a particular feed rate.

Select the Feed rates check box on the Tool page of the 5 Axis Operation dialog box and click on the Feed rates button. The Change feed rate according to surface radius dialog box is displayed.

Simultaneous 5 Axis Machining

The Rapid (G0).

move parameters

group enables you to control the use of rapid feed

â&#x20AC;˘ When the Use rapid feed option is not selected, the resulting Gcode contains rapid movements (G0). Example:

G0 X-2.942 Y75.567 Z24.402 A-88.436 B-26.482 M116

When the Use rapid feed option is chosen, the resulting Gcode does not contain G0 commands. The rapid movements are performed using the feed rate defined by the Rapid feed rate parameter. Example:

G1 X-2.942 Y75.567 Z24.402 A-88.436 B-26.482 F9998 M116

5.2 Levels 5.2.1 Angle step for rapid moves SolidCAM2007 R11.2 enables you to approximate by lines the curved rapid movements performed at the spherical or cylindrical clearance area.

Initial motion

The approximation is controlled by the illustrated below.

Approximated motion

Angle step for rapid moves

parameter

Simultaneous 5 Axis Machining

Angle step for rapid moves

Initial motion Approximated motion

Small values of the Angle step for rapid moves parameter cause less deviation between the initial curve and the approximated path, but may cause some machines to slow down. Using larger values of the Angle step for rapid moves parameter, you can reduce the number of approximation lines thus increasing the motion speed; however then there is a danger of collision, since the curved motion is simplified (when the Angle step for rapid moves is set to 90째 the circular movement is approximated to a square).

5.3 Geometry 5.3.1 Advanced parameter for margins Tool path strategies that use edge curves and surfaces sometimes encounter difficulties since CAD systems deliver the drive surfaces and the edge geometry (curves or surfaces) only within accuracy. If you would like to start the tool path exactly at the zero distance to the edge geometry, then this is problematic, because the geometry can never be exactly aligned. To avoid this problem, SolidCAM2007 R11.2 provides you with the Additional parameter for margins option. This option is available only for the Morph between two curves, Parallel to curve, Morph between two surfaces and Parallel to surface strategies, when the Area type is Full, start and end on exact surface edges. To activate it, click on the Data button in the Area field of the 5 Axis Operation dialog box.

The Margins dialog box is displayed. In this dialog box, you may set the Start and End Margin value. The Additional margin to overcome surface edge inaccuracies parameter enables you to compensate the inaccuracy of the CAD model edges. For example, to get the tool path at the 5 mm distance from the geometry, set the margin to 4.97 mm and the Additional margin to overcome surface edge inaccuracies to 0.03.

Simultaneous 5 Axis Machining

5.3.2 Machining of shallow and steep areas SolidCAM2007 R11.2

shallow areas.

enables you to perform a separate machining of steep and

Select the Shallow/Steep check box and click the Shallow/Steep button.

The Parameters to define the shallow and steep areas dialog box is displayed. This dialog box enables you to define parameters determining the steep/shallow area to be machined.

â&#x20AC;˘ View direction.

SolidCAM enables you to define a vector from where the slope angle start and end are referenced. SolidCAM enables you to choose one of the Coordinate System axis (X-axis, Y-axis and Z-axis) or define a vector by an end point (the start point is automatically considered to be in the Coordinate System origin).

â&#x20AC;˘

Slope angles.

The Slope angle start and Slope angle end parameters define the limit angles around the View direction vector. The surfaces with the inclination angles enclosed by the range defined by the slope angles are considered as the steep areas. All the surfaces with the inclination angles outside of the range are considered as shallow areas.

Shallow area Steep area Slope end angle Slope start angle

View orientation axis

â&#x20AC;˘

Machining areas.

This option enables you to determine the area to be machined. When the Machine steep areas option is chosen, the machining will be performed only at the steep areas (surfaces with inclination angles within the range defined by Slope Start and Slope End angles). When the Machine shallow areas option is chosen, the machining will be performed only at the shallow areas (surfaces with inclination angles outside the range defined by Slope Start and Slope End angles). Note that shallow and steep calculation is purely based on surface contact points. In other words, some portions of the surface geometry are virtually trimmed in order to split the part into shallow and steep regions.

Simultaneous 5 Axis Machining

5.3.3 2D Containment boundaries provides you with a functionality to limit the machining to specific model areas. The machining limitation is performed by a planar boundary that is projected on the model. The projected boundary is â&#x20AC;&#x153;virtuallyâ&#x20AC;? trimming the drive surfaces. All the contact points of the tool and drive surfaces are enclosed by this projected boundary. SolidCAM2007 R11.2

Select the 2D Containment check box, and click on the 2D Containment button.

The 2D Containment dialog box is displayed enabling you to define the boundaries.

2D Containment curves

SolidCAM enables you to define a boundary based on a Working area geometry (closed loop of model edges as well as sketch entities). For more information on Working area geometry, refer to the SolidCAM User Guide book. The Define button displays the you to define the geometry.

Geometry Edit

dialog box that enables

The Show button enables you to display the already defined boundary directly on the solid model. Projection direction

When a planar boundary is defined, SolidCAM automatically projects the geometry onto the solid model. The direction of the projection is defined by a vector. SolidCAM enables you to choose an axis of the Coordinate System as a projection direction vector or define a vector by an end point (the start point is automatically considered to be in the Coordinate System origin.

2D Containment boundary

Projection direction axis

Machining area

Simultaneous 5 Axis Machining

5.3.4 Max. projection distance When the Project curves tool path strategy is chosen, the system expects to get projections curves lying on the drive surfaces. Due to tolerance issues in CAD systems, sometimes the curves do not lie exactly on the drive surfaces. SolidCAM2007 R11.2 enables you to compensate the mismatches between the drive surfaces and projection curves using the Maximal projection distance parameter.

All the deviations between the drive surfaces and projection curves that are less than the specified Maximal projection distance value are compensated. When a deviation is equal or greater than the parameter value, the tool path is not calculated.

5.3.5 Spiral cutting method Previous SolidCAM versions provided you with a capability to convert a Parallel cuts passes into a spiral path. SolidCAM2007 R11.2 provides you with a new Spiral Cutting method. This cutting method is available for use with all the Pattern types, except the Project curves pattern.

With the Spiral Cutting method, SolidCAM generates a spiral tool path around the drive surface according to the chosen Pattern. The spiral pitch is defined by the Step over parameter.

Step over

Simultaneous 5 Axis Machining

5.3.6 Machining order SolidCAM2007 R11.2 enables you to define the machining order for a Sim. 5-axis operation. The Machine by edit box located at the Geometry page enables you to choose the order of machining of certain areas; it defines whether the surface will be machined by Lanes or by Regions.

The generated tool path usually has a topology of multiple contours (lanes) on the drive surfaces. When the tool path is generated in many zones, it might be preferable to machine all the regions independently.

6 1

Lanes

2 1

Regions

5.3.7 Start point definition provides you with a new interface and extended functionality for the Start point definition. SolidCAM2007 R11.2

Generally, SolidCAM automatically determines the start point for the tool path taking into account the path shape. To define the start point manually, select the Start point checkbox at the Geometry page and click on the related button.

The Start point parameters dialog box will be displayed.

This dialog box enables you to define the Start point for the first cut; it can be defined either by entering coordinates in the related editboxes or by picking the Start point position directly on the solid model using the button.

Simultaneous 5 Axis Machining

The Start point will be applied in subsequent cuts as following group enables you to define the start position of the subsequent passes. The for the Two new options related to the definition of geometry start point have been added. These options are available in the Start point parameters dialog box that is displayed by clicking on the Start point button in the 5 Axis Operation dialog box. â&#x20AC;˘ Shift by value

This option added in SolidCAM2007 R11.2, enables you to start the next cut at a specified distance from the previous start point. The distance defined in related editbox is measured along the path. Value

Start point

â&#x20AC;˘ Rotate by [deg]

With this option SolidCAM enables you to rotate the start position of the cuts relative to the Start point start position of the first cut. The Rotate by value defines the rotating angle for the start position for subsequent cuts.

â&#x20AC;˘ Minimize surface normal change (new option)

With this option, SolidCAM automatically chooses the start points for passes in such a way, that the change of the direction between surface normals at the start points will be minimal.

Normals Start point

Simultaneous 5 Axis Machining

5.3.8 Show surface normals direction When transferring model files from one CAD system to another, the direction of some of the surface normals might be reversed. For this reason, SolidCAM2007 R11.2 provides you with the capability to display and edit the normals of model surfaces during the geometry selection. The Show Direction for highlighted faces only check box enables you to display the surface normals for the specific highlighted faces in the faces list. The Show Direction for selected faces check box enables you to display the normals direction for all the faces in the list.

The right-click menu available on the items in the selected faces list, enables you to reverse the direction of the surface normals of the chosen faces (the Reverse command) or of all the selected faces (the Reverse all command)

5.4 Surface quality options in Finish parameters SolidCAM2007 R11.2 provides you with the several new features related to the quality

of the surface to be machined.

5.4.1 Surface edge merge distance SolidCAM generates first tool paths for individual surfaces. Then they are merged together to form the complete tool path. The decision about the merging is based on the Surface edge merge distance parameter introduced in SolidCAM2007 R11.2. If all surface paths on a tool path slice are merged, then a check is made if a closed surface path can be built by connecting the start to the end. The Surface edge merge distance parameter is used for deciding this. The Surface edge merge distance parameter can be defined either as a numeric value (the As value option) or as a percentage of the tool diameter (the % of tool diameter option). In both cases, this limit value must be greater than or equal to the Cut tolerance value. 5.4.2 Advanced options for surface quality The Chaining tolerance parameter defines the tolerance of the initial grid used for the tool path calculation. The recommended value is from 1 to 10 times the Cut tolerance. In some cases, for simple untrimmed surfaces, the Chaining tolerance value can be defined upto 100 times the Cut tolerance and would increase the calculation speed significantly.

Simultaneous 5 Axis Machining

The surface contact paths are created while analyzing and slicing the surface patches. If due to slicing the tool path topology becomes very complex (for example, patches parallel to curve and surface are very large), sometimes the surface contact paths cannot be constructed safely. provides you with an additional functionality to control the surface quality. If the Slow and safe path creation check box is selected, a finer grid (based on the maximal step over value) is applied for initial analysis of surface patches, thus delivering slow but safe results for surface contact points. SolidCAM2007 R11.2

5.5 Link Macro 5.5.1 Macro Entry/Exit strategies provides you with two new strategies of Macro entry and exit: Reverse tangential line and Reverse vertical tangential arc. SolidCAM2007 R11.2

Reverse tangential line

With this option SolidCAM performs an approach/retreat movement with a line tangential to the cutting pass like the Tangential line option, but the direction of the approach/retreat line is reversed.

Simultaneous 5 Axis Machining

Reverse vertical tangential arc

SolidCAM performs an approach/retreat movement with an arc tangential to the drive surface, located in the plane of the tool axis, like the Vertical Tangential arc option, but the direction of the approach/ retreat arc is reversed.

5.5.2 Maximal angle change

When the Tangential option is chosen for the Tool axis orientation, the tool axis orientation is continuously changed during the approach/retreat movement. This option enables you to avoid marks on the part surface caused by the tool rotation at the start/end point of the cutting pass. In case of large macro moves, the total change of tool axis orientation might be great. Therefore, SolidCAM enables you to limit the total change of tool axis orientation along a macro move with the Max. angle change parameter.

Simultaneous 5 Axis Machining

5.6 Tool axis control provides with an additional functionality used when the side tilting direction is defined with the Use tilt line definition option. SolidCAM2007 R11.2

The Tilting lines maximum snap distance parameter defines the maximum distance between tilt line end points and the machining contour. When tilting is applied to a contour, then only lines within this distance will be used, while other lines that are far from the contour will be ignored. Note, that the tilt lines are snapped to the machining contour via the shortest distance from the line to the contour.

5.7 Gouge check 5.7.1 Collision control provides you with new collision control options available in the Gouge Check page of the 5 Axis Operation dialog box: SolidCAM2007 R11.2

Extend tool to infinity This option enables you to consider the tool as being extended to infinity during collision check in order to make sure that all active surfaces are checked for collision, no matter where they are located in space.

Check link motions for collision When this option is chosen SolidCAM automatically performs the gouge checking for link movements in order to avoid possible collisions.

Simultaneous 5 Axis Machining

5.7.2 Split contour within distance Generally, SolidCAM tries to find a solution to avoid a possible gouges for a complete pass. In case of long passes it is very difficult to find a solution that will be relevant along all the pass length. To simplify this task, SolidCAM2007 R11.2 provides you with the Split contour within distance option that is enabled when you avoid the possible collisions using tilting in the cutting direction and side tilting. The option is located in the Advanced parameters for tilting tool away with max angle using lead/lag and side tilt angles dialog box. It enables you to split the original contour into multiple contours, with the length defined as percentage of the whole contour length. When the initial passes are split into a number of smaller passes, SolidCAM calculates the solution for avoiding collision for each pass.

This option is available only if the Make tool axis orientation continuously if distance is smaller than check box is selected.

5.7.3 Using STL files for gouge checking SolidCAM2007 R11.2 provides you with the functionality to define the check surfaces

used for the gouge checking with an STL file.

When the Use STL file checkbox is activated the Check surfaces group enables you to choose a check surfaces geometry from an STL file.

The Define button enables you to display the dialog box.

Choose STL

The Browse button in the dialog box enables you to choose the necessary STL file. The full name (including the path) of the chosen STL file is displayed in the STL file editbox. The Show on model and Show buttons enable you to display the chosen STL triangles either directly on the solid model or in a separate window.

Simultaneous 5 Axis Machining

5.8 Roughing 5.8.1 Area roughing SolidCAM2007 R11.2 provides you with a new functionality for simultaneous 5axis roughing. The main target of this functionality is impeller machining. With the Area roughing strategy, the roughing tool path is created inside the initial tool path. E.g. the floor area between impeller blades can be machined using this strategy if the initial tool path describes the left and right side of the area limitations.

Initial tool path

Area roughing tool path

In the Roughing page, check the Area roughing checkbox and click on the related button.

The Area roughing dialog box is displayed enabling you to define the parameters of the area roughing.

• Rotary axis around.

This parameter defines the rotary axis. SolidCAM enables you to choose an axis of the Coordinate System (X, Y, Z) or define a rotary axis vector by an end point (the start point is automatically considered to be in the Coordinate System origin).

• Rotary axis base point.

With this option, SolidCAM enables you to define the position of the rotary axis directly on the solid model.

• SolidCAM enables you to define a number of cuts either by the Maximum Step over parameter (the distance between two successive cutting passes) or by the Number of cuts per section parameter. • SolidCAM enables you to machine the area enclosed between two main blades and containing a splitter blade. The Area option enables you to define the area when the machining will be performed. Complete.

The machining is performed in the complete area between the two main blades. Left.

The machining is performed in the area between the left main blade and the splitter blade. Right.

The machining is performed in the area between the right main blade and the splitter blade. 76

Main blades Splitter blade

Simultaneous 5 Axis Machining

• The Cutting method options enable you to define the passes direction and the way how the single passes will be connected into a complete tool path. The following options are available: One way (along rotary axis).

With this option, the machining of the pass starts at the upper edge of the impeller floor face, continues along the blades and stops at the lower edge of the floor. Then the tool retracts to the start position of the next cutting pass. One way (along reverse rotary axis).

With this option, the machining of the pass starts at the lower edge of the impeller floor face, continues along the blades and stops at the upper edge of the floor. Then the tool retracts to the start position of the next cutting pass. Zig zag.

With this option, the machining starts at the edge of the impeller floor face, continues along the blades to the other edge, steps over to the next cut at the same edge and continues machining to the first edge. The sequence for the cuts is from the left to the right. Zig zag (climb only). With this option, the machining begins in the center

of the surface and progresses outwards to the sides. •

Alternate direction to reduce path length.

With this option, SolidCAM changes the start position of the cut in order to minimize air cuts. This option is available only when the

Zig zag (climb only) Cutting

method is chosen.

•

Calculation applied.

With this option, SolidCAM enables you to define when the calculation of the area roughing is performed. The area roughing calculation can be performed either before the tilting calculation (the Before tilting option) or after the collision control (the After collisions control option). If the area roughing calculation is performed after the collision control, the resulting tool path is checked again for collisions. When the After collisions control option is used, SolidCAM enables you to extend the tool path using Extension at start and Extension at end parameters.

5.8.2 Tool path rotation SolidCAM2007 R11.2 offers you a new functionality for tool path rotation; this option

is useful for parts with multiple identical elements arranged in a circular pattern. Instead of adding a separate operation and defining the same parameters for each of these patterns, you can have the same tool path repeated a given number of times by rotation around a specific axis.

To use this option, select the appropriate check box in the 5 Axis Operation dialog box and click on the Rotate button.

The Rotate toolpath dialog box enables you to define the parameters of rotation.

Simultaneous 5 Axis Machining

•

Rotary axis around. This option provides you the choice of

the axis around which your tool path will be rotated. You may choose between the X-, Yor Z-axis of the current Coordinate System or define a rotary axis vector by an end point (the start point is automatically considered to be in the Coordinate System origin).

•

Rotary axis base point.

•

Number of steps.

•

Start angle.

•

Rotation angle.

•

Sort by.

This option enables you to define the position of the rotation axis. When you click on the Select point button, the Select point dialog box is displayed and shows the coordinates of the point you pick on the model. This parameter enables you to define the number of instances of the circular pattern. In other word it defines how many times the initial tool path will be repeated around the rotation axis. This parameter enables you to define the rotation angle for the first tool path instance of the circular pattern. This parameter enables you to define the angle between the two adjacent instances of the circular pattern. This option enables you to choose whether the whole tool path will be rotated or only a certain part of it. The following options are available: •

Complete tool path.

•

Passes.

•

Slices. With this option the whole tool path will be rotated.

•

Partial tool path.

will be rotated.

With this option the whole tool path

With this option the whole tool path will be rotated. The resulting tool path will be sorted and linked by passes. The resulting tool path will be sorted and linked by slices.

With this option the portion of tool path specified by a percentage is rotated. The percentage is specified by the Perc. of whole tool path parameter.

5.8.3 Check for collision between stock and tool elements enables you to prevent the collisions between the tool/holder components and the machined stock model. SolidCAM2007 R11.2

• Tool shaft

Select this check box to check for collision between the tool shaft and the machined stock. • Tool arbor

Select this check box to check for collision between the tool arbor and the machined stock. • Tool holder

Select this check box to check for collision between the tool holder and the machined stock.

Simultaneous 5 Axis Machining

5.9 Extra Parameters With

SolidCAM2007 R11.2,

Miscellaneous parameters

the Extra parameters option has been added to the page of the 5 Axis Operation dialog box.

In case there are special operation options implemented in the post-processor used for the current CAM-Part, the Parameters List button enables you to display the list of additional parameters defined in the post-processor.

Turning

6.1 Generating sketch for the Material boundary enables you to generate a sketch containing the material boundary of the part after the machining by a specific turning operation. SolidCAM2007 R11.2

Right click on a specific turning operation (Turning, Drilling, Grooving and Threading) and choose the Generate Material boundary command from the menu. This command automatically creates a new sketch in the CAM component of the CAMPart assembly and generates in this sketch the geometry of the updated material boundary after the chosen operation.

The generated updated material boundary is not associative to the model geometry and operations.

Wire Cut

7.1 Definition of Insertion point using points of the CAD sketch introduces a new option related to definition of the point where the wire is inserted into the workpiece. This option enables you to use the points of the CAD sketch to define the insertion point for the model geometry. SolidCAM2007 R11.2

Choose the By Sketch Point option in the Insertion point section of the Initial Points dialog box for single-chain profiles or in the Insertion points section of the Chains Selection dialog box for multiple-chain profiles. The sketch point closest to the start point of the chain will be chosen as the insertion point for the wire. Sketch points

Insertion Point

Start Point

You can display the multiple-chain geometry with the defined insertion point by clicking on the View Chains button at the bottom of the Chains Selection dialog box.

Wire Cut

7.2 Automatic definition of Start point for multi-chain geometry In the previous SolidCAM versions, the automatic definition of the start point was supported only for single-chain profile geometries. The current release provides you with the option to define the start point automatically for geometries consisting of multiple chains as well. In the

dialog box, there is a new Start points section that contains two possibilities of automatic definition of the chain start point: Chains Selection

â&#x20AC;˘ Auto

The start point is defined automatically at the closest point on the geometry to the insertion point by dropping a normal from the insertion point to the profile. Insertion Point

Start Point

â&#x20AC;˘ At Angle

The start point is defined automatically at the intersection of the profile and the line drawn from the insertion point, at the selected angle. Insertion Point Angle Start Point

Machining Processes

8.1 New Turn-Mill Machining Process table type Previous versions of SolidCAM enabled three types of Machining Process tables: Milling, Turning and Wire Cut. SolidCAM2007 R11.2 provides you the fourth type of Machining Process table that can be defined for your CAM-Part: Mill-Turn.

In the Machining Process Machining Processes.

Table Manager,

you may add both Milling and Turning

Machining Processes

8.2 Tool definition and search in Machining Processes In previous SolidCAM versions the when a Machining Process was defined, the tool number was assigned to a tool automatically and the user had no control over it. When the Machining Process was inserted into a CAM-Part, SolidCAM performed a tool search according to the tool data in the Machining Process. The tool search was performed in the Part Tool table and Current tool table. If a tool, whose data matched the data of the tool as defined in the Machining Process, was found then it was chosen; if no such tool was found, then a new tool was created with the first available number. provides you with more advanced functionality for the tool number definition inside the Machining Process and for the tool search during the Machining Process insertion. SolidCAM2007 R11.2

8.2.1 Parametric tool definition enables you to define the tool number as a variable, similar to the other tool data that can be defined parametrically in the Operation templates. The expression for the tool number variable can vary in the different Default sets. The tool number variable is assigned its value during the insertion of a MP into the CAM-Part. SolidCAM2007 R11.2

By default, this option is disabled when you define the tool for an operation template in a MP. To enable it and define the tool number parametrically, rightclick on the tool name in the Tool list area of the Part Tool table and choose User-defined tool number.

The Tool number field becomes available for parametric definition; all other tool parameters are disabled.

You may switch back to the method where the Tool number is assigned automatically by right-clicking on the tool name in the list and choosing Automatically-assigned tool number.

Machining Processes

When you insert the MP into the CAM-Part, you have to assign values for the tool parameters that were defined as variables in the MP. If the tool was defined with the User-defined tool number option, SolidCAM automatically checks the existence of the tool with the specified number in the Part Tool table and Current Tool table; if a tool with this number is not found, the number is not acceptable.

The parametric menu available for the tool number variables contains three options: • Tool select from Current Tool table

This option displays the Current Tool table from which you may choose a tool for the MP insertion. When you have selected a tool, its tool number from the Current Tool table appears in the Expression field of the MP Insert Manager. This option is available only when the Current Tool table is defined. • Tool select from Part Tool table

This option displays the Part Tool table from which you may choose a tool for the MP insertion. When you have selected a tool, its tool number from the Part Tool table appears in the Expression field of the MP Insert Manager. • Edit – View

This option displays the expression manually.

Edit

dialog box in which you may enter the

8.2.2 Tool search during the insertion of Machining Process automatically performs a tool search during of the machining process insertion. The tool search is performed according to the User-defined tool number / Automatically-assigned tool number property of the tool used in the Operation template. SolidCAM2007 R11.2

When the User-defined tool number option is used for the tool definition, the tool search for this tool is performed using the tool number only. The tool search is first performed in the Part Tool table; if the tool is found, it is used. If the tool with the defined number is not found in the Part Tool Table, SolidCAM performs an additional search in the Current Tool Table. If the tool with the defined tool number is found in the Current Tool Table, it is copied into the Part Tool Table (with the same number) and used. When the Automatically-assigned tool number option is used for the tool definition, the tool search is performed using the tool parameters. The tool parameters used for the tool search are defined in the SolidCAM Settings (see topic 8.2.3). The tool search is first performed in the Part Tool table; if the tool is found, it is used. If the tool is not found in the Part Tool Table, SolidCAM performs an additional search in the Current Tool Table. If the tool is found in the Current Tool Table, it is copied into the Part Tool Table and used. If the tool is not found in the Current Tool Table, a new tool with the defined parameters is created in the Part Tool Table. SolidCAM automatically chooses the first available tool number for the newly created tool.

Machining Processes

8.2.3 Tool search settings The Tool search page in the SolidCAM Settings dialog box enables you to define the parameters that will be used as search criteria when the tool search is performed by tool parameters.

This page contains two sets of tool data for Milling and Turning tool search. To define the parameters you want to include in the search, select the relevant check boxes. The Check All and Clear All buttons enable you to select or clear all the check boxes in each section separately.

Automatic Feature Recognition Module

9.1 Using color information to assign technology In SolidCAM2007 R11.2 the AFRM recognizes the color as an additional parameter of the hole feature. When you have a solid model where different colors were assigned to different families of similar hole features, SolidCAM AFRM enables you to use the color data to assign the technology. The color information of each hole segment is available with other parameters in the Hole Feature Parameters dialog box. In the Value field, the color is presented as numerical values of the RGB color model. When a hole feature segments are converted to the machinable hole feature, the color is stored in the hr_segm_color parameter.

9.1.1 Setting color as condition for machining You may use color as a criterion for machining of different hole features. In case you want to perform a particular operation only on a given set of holes with the same color, you need first to set the color parameter as the condition for a specific machining solution.

Automatic Feature Recognition Module

You have then to assign this parameter a relevant color value by using Select Color dialog box. This dialog box enables you to either choose a color from the palette or choose the color from the solid model faces. When you pick a color, SolidCAM generates a numerical value for this color to be assigned to the appropriate variable.

100