Preview eagle v6 getting started guide

Eagle CD-ROM included

V6

Whether you are an electronics enthusiast or engineering professional, this book provides the reader with an introduction to the use of the CadSoft’s EAGLE PCB design software package.

EAGLE is a user-friendly, powerful and affordable software package for the efficient design of printed circuit boards. It offers the same power and functionality to all users, at a smaller cost than its competitors. A free version of EAGLE is available to enthusiasts for their own use.

The book is intended for anyone who wants an introduction to the capabilities of EAGLE. The reader may be a novice at PCB design or a professional wanting to learn about EAGLE, with the intention of migrating from another CAD package.

This book will quickly allow you to: obtain an overview of the main modules of EAGLE: the schematic editor; layout editor and autorouter in one single interface; learn to use some of the basic commands in the schematic and layout editor modules of EAGLE; apply your knowledge of EAGLE commands to a small project; learn more about some of the advanced concepts of EAGLE and its capabilities; understand how EAGLE relates to the stages of PCB manufacture; create a complete project, from design through to PCB fabrication. The project discussed in the book is a popular, proven design from the engineering team at Elektor.

GETTING STARTED GUIDE

EAGLE can be used on the main computing platforms including: Microsoft Windows (XP, Vista or Windows 7); Linux (based on kernel 2.6 or above) and Apple Mac OS X (Version 10.6 or higher). Any hardware that supports these software platforms will run the EAGLE application.

Eagle V6

Mitchell Duncan

LEARNING TO FLY WITH EAGLE GETTING STARTED GUIDE

LEARNING TO FLY WITH EAGLE

Eagle

After reading this book while practicing some of the examples, and completing the projects, the reader should feel confident about taking on more challenging endeavors.

Courtesy of CadSoft Computer GmbH (www.cadsoft.de), this book is supplied with a copy of Eagle on CD-ROM for MS Windows, Linux and Mac.

www.elektor.com Elektor International Media

Mitchell Duncan

For the more sophisticated user … a more comprehensive guide and reference to EAGLE will follow from Elektor Publishing. Stay alert and keep watching for this!

eagle

®

Eagle LEARNING TO FLY WITH EAGLE

GETTING STARTED GUIDE

V6

Mitchell Duncan

eagle

GETTING STARTED GUIDE

V6

LEARNING TO FLY WITH EAGLE

1

2

eagle V6

GETTING STARTED GUIDE LEARNING TO FLY WITH EAGLE

Mitchell Duncan

Elektor International Media www.elektor.com

3

All rights reserved. No part of this book may be reproduced in any material form, including photocopying, or storing in any medium by electronic means and whether or not transiently or incidentally to some other use of this publication, without the written permission of the copyright holder except in accordance with the provisions of the Copyright, Designs and Patents Act 1988 or under the terms of a licence issued by the Copyright Licensing Agency Ltd, 90 Tottenham Court Road, London, England W1P 9HE. Applications for the copyright holder’s written permission to reproduce any part of this publication should be addressed to the publishers.

The publishers have used their best efforts in ensuring the correctness of the information contained in this book. They do not assume, and hereby disclaim, any liability to any party for any loss or damage caused by errors or omissions in this book, whether such errors or omissions result from negligence, accident or any other cause.

British Library Cataloguing in Publication Data A catalogue record for this book is available from the British Library ISBN 978-1-907920-20-2 Prepress production: Jack Jamar | Graphic Design, Maastricht First published in the United Kingdom April 2013 Printed in the Netherlands by Wilco, Amersfoort Š Elektor International Media BV 2013 129026-1/UK

4

Table of Contents Acknowledgments

11

Part 1 - Learning to Use EAGLE

13

Chapter 1 - An Introduction to EAGLE Software

15

Introduction Conventions Used in this Guide Mouse Clicks Selection of Menu Items Use of keys What is EAGLE and what does it produce?

15

Chapter 2 - Eagle Installation & Startup

21

Windows Linux Mac OS X Starting EAGLE Projects Libraries

15 16 16 16 17

21 23 23 24 26 27

Chapter 3 - Using the EAGLE User Interface

29

EAGLE Icons and Command Toolbars Schematic Editor Toolbars The PCB Layout Editor Action Toolbars Command Toolbars

30 30 32 32

5

Table of Contents

The EAGLE Module Menus The EAGLE Module Sub-menus Schematic Editor Sub-menus The File Sub-Menu The Edit Sub-Menu The Draw Sub-Menu The View Sub-Menu PCB Layout Editor Sub-menus The File Sub-Menu The Edit Sub-Menu The Draw Sub-Menu The View Sub-Menu Navigating & Controlling EAGLE Input Alternatives within EAGLE Function Keys Eagle Commands Pan, Zoom & Screen Functions

34 34 35 35 36 37 38 39 39 40 41 42 42 42 42 44 45

Chapter 4 - Creating Your First EAGLE Project

49

Setting Up: Layers, Grids and Units Layers: the DISPLAY Command Grids and Units Creating a Schematic Drawing using basic EAGLE Commands Manipulating Objects within a Schematic The USE Command & Libraries The ADD Command Adding a Frame Adding components from a Library Working with Objects: the COPY, MOVE, and MIRROR Commands The DELETE Command The UNDO and REDO Commands Connecting Components Together The NET Command The JUNCTION Command The SHOW Command Completing the Schematic Drawing

54

6

54 55 57 57 57 58 58 59 64 65 65 66 66 68 69 70

Table of Contents

Creating a PCB Layout from a Schematic Drawing Setting up the Printed Circuit Board Dimensions Placing components on the Printed Circuit Board Inserting the tracks : the ROUTE Command Using the Autorouter Automatic Forward &Back Annotation Getting Output from EAGLE Output to a Printer Generating Image Files Using the CAM module - generating output for PCB Manufacturing Generating the output files for PCB Manufacturing

72 74 75 76 77 79 81 81 84 85 86

Chapter 5 - More Advanced Concepts & Commands in EAGLE.

89

General Commands The INFO Command The NAME Command The Value Command The Attribute Command The Change Command The Smash Command The GROUP Command Schematic Editor Commands The Gateswap Command The Pinswap Command The Bus Command The Label Command The Invoke Command PCB Layout Editor Commands & Concepts Working with Devices ROTATE Command LOCK Command Board Layers The CIRCLE Command The RECT Command Polygons

89 89 90 91 92 92 96 97 100 100 100 101 106 107 109 109 109 110 111 112 113 116

7

Table of Contents

Manual Routing The Via Command The WIRE Command The RIPUP Command The SPLIT Command The ROUTE Command The HOLE Command The DIMENSION command Restricted Areas Electrical Rule Check (ERC) Design Rule Check (DRC) Example - Design Rule Errors Mistakes to Avoid - Fatal Design Rule Errors Libraries The Library Editor EDIT an Object

121 121 122 124 125 126 129 130 131 132 133 134 136 141 142 144

Chapter 6 - An Introduction to PCB Manufacturing

147

Types of Printed Circuit Boards Single-sided Printed Circuit Board Double-sided Printed Circuit Board Multi-Layer Printed Circuit Board Fabrication of PCBs Drilling Holes Via and Hole Plating Making Tracks: Photolithography & Etching or Milling Photolithography & Etching Laser direct imaging Milling Electroplating Etching Solder Mask Screening Silk Screening Hot Air Levelling Routing and Trimming Gerber Files

147

8

147 148 149 151 152 154 154 154 158 158 159 159 162 162 163 163 170

Table of Contents

Part 2 - Using EAGLE in a Real Project

173

Chapter 7 - A Full EAGLE Project ; Creating a Radiation Meter Counter

175

Drawing the Project Schematic USEing the Libraries ADDing the components Drawing the NETS Drawing the Project PCB Layout Drawing the DIMENSIONS and adding Holes Placing the Components on the PCB Laying out the Copper Restricted Areas Routing the Signal Tracks Ground Planes and Polygons Final Design Rule Check ‘Pouring’ the Ground Planes Fabricating your PCBs Creating the PCB Manufacturing Files Finding a PCB Fabricator

175 179 180 184 185 187 191 192 192 192 193 194 195 197 197 197

Appendix 1 - System Requirements and Features of EAGLE Package Variants

203

Professional Edition General Features Schematic Editor Layout Editor Autorouter Module Standard Edition Freemium Edition Light Edition

203 203 204 205 205 206 206 206

9

10

Acknowledgments

I would like to thank my dear wife Sadhana, whose patience with my hours of work has made this small contribution to technical writing possible.

Also, I would like to thank my friend and mentor, Dr Robert Curtis (Rob), who encouraged me to start this project, and will no doubt like to move it on to greater things with me. ‘Finally, a special note of thanks should go to Mr Richard Hammerl (at technical support, CadSoft Computer GmbH) who gracefully answered all my questions about the functionality of EAGLE’.

11

‘Author’s Note: At the time of going to press, the most recent release version of EAGLE was V6.4. Although this book was written for V6.0, the instructions contained herein will be accurate for the most recent version of EAGLE.’

12

Part 1 -

Learning to Use EAGLE

eagle V6

13

Chapter 4 -

Creating Your First EAGLE Project

You are now in a position to start creating your first EAGLE project. We’ll initially use the examples supplied with EAGLE. After you have mastered this section, you may wish to be more ambitious and work through the project in Part 2 of this book; Creating a Radiation Meter Project, where you will be guided through all of the stages in creating a complete design. This project was published in the November 2011 edition of Elektor magazine; titled ‘Improved Radiation Meter’.

We’ll start by creating a new project and the schematic drawing.

In this tutorial we will learn how to add all of the components in this drawing and connect them together. Figure 4-2 is the Schematic Drawing for this tutorial. You can use this as a template from which to draw your own schematic.

Let’s begin by starting EAGLE and expanding down to the tutorial entry in the tree view by performing the following actions: Projects, then , examples, next, tutorial Lastly,

on tutorial and you will see a similar structure to the left pane (as in Figure 4-1).

49

Chapter 4 - Creating Your First EAGLE Project

Figure 4-1. Starting a new Project

50

Creating Your First EAGLE Project

Figure 4-2. Complete Schematic Drawing for Tutorial

If you now on New Project , a new project will be created and will be displayed in the tutorial files directory tree, as shown in Figure 4-3.

51

Chapter 4 - Creating Your First EAGLE Project

Figure 4-3. Naming the New Project

Name your new project ‘My Project’ (or your preferred title) by typing in the name in the input line and then

.

This creates a sub-directory under tutorial, named My Project, containing all the files associated with your project. The last used projects and user-specific settings are also stored here, in Windows, as eaglerc.usr (~/.eaglerc for Linux and Mac) You now need to define the path for the destination of your project directories. Type Options > Directories The following dialog box will appear as illustrated in Figure 4-4.

52

Creating Your First EAGLE Project

Figure 4-4. Setting up EAGLE directories

You can now type in your desired location. For example, add the following to the end of the Projects field (preceded by a semicolon): ‘D:\My EAGLE Projects’.in the Projects field.

Now, open a new Schematic by: My Project > New > Schematic You will be presented with a new schematic window as in the Figure 4-5:

Figure 4-5. New Schematic Layout Window

53

Chapter 4 - Creating Your First EAGLE Project

Setting Up: Layers, Grids and Units Layers: the DISPLAY Command To enable the Eagle Editor modules to perform their task properly, objects within drawings need to be grouped in different and separate layers, according to their purpose. These layers can also be selected, displayed and printed as a group. In general, the default settings will suit the new user of EAGLE. To action the DISPLAY command you simply EAGLE will present the layer dialog box (see Figure 4-6), which will allow you to select and de-select layers for use. Layers will be discussed later in more detail, in Chapter 5.

Figure 4-6. Display Command dialog box

54

Grids and Units

Grids and Units Objects cannot be randomly placed on a drawing, that is, at least not on a PCB layout. So, EAGLE provides a grid basis for placing objects.

Grid size or spacing can be specified by using the menu selection: dialog box then appears, as in Figure 4-7.

View > Grid. The Grid

Figure 4-7. Grid dialog box

You are able to select from the alternative grid units of inches, millimeters, mils (1/1000ths inch) and mic (microns or mm). When set, this value applies to all values in the drawing.

In the dialog box one can select: i. the grid Size (i.e. the pitch between points on the grid) and unit (the base measurement method), ii. the display Multiple or the periodicity at which grid lines are displayed, iii. an Alternative grid pitch which may be accessed by using the

key.

Using this dialog , you can also choose whether to display the grid or not, and its style as dots or a solid line.

55

Chapter 4 - Creating Your First EAGLE Project

The default settings are given in the Figure 4-7 above. You may wish to change them to, say, 0.1inch spacing (since a large number of components are based on a 0.1inch manufactured specifications) with the Alternative grid pitch set to 0.025 inch. This will allow you to adjust some items to a finer positioning.

Your settings will be reflected in the grid and co-ordinates display, located towards the upper left-hand corner of the window, just above the corner of the workspace itself (see Figure 4-8). The numbers in this display comprise the selected grid size, followed by the position of the cursor, using the selected grid unit size.

Figure 4-8. Grid Units and Cursor Co-ordinates Display

The cursor position co-ordinates are given with reference to a datum point. This point is placed, by default, in a new drawing, near the bottom left-hand corner of the workspace. This is illustrated in Figure 4-9.

Figure 4-9. Cursor position Datum indicator

56

The USE Command & Libraries

The use of grids is much more important later in the book, when we begin exploring the use of the PCB Layout Editor, since all components must be precisely positioned in order to manufacture a PCB. You may wish to use the following Table 4-1 to convert between the different bases of measurement Table 4-1. Conversion between Millmetres, Inches & Mils Millimeters (mm)

Inches (inches)

Mils (mils)

1mm

0.03937 inch

39.37mils

25.4mm

1 inch

1000 mils

0.0254mm

0.001 inch

1 mil

Of course, if you are using a very small scale, use can also use microns, where: 1 micron = 1 x 10 -6 meters =1 x 10 -3 millimeters (1/1000th millimeter)= 0.03937 mils

Creating a Schematic Drawing using basic EAGLE Commands Manipulating Objects within a Schematic The USE Command & Libraries

There are many libraries of commonly used components supplied with the EAGLE software.

So, in order to begin creating a schematic, we first have to gain access to the component information stored in the appropriate libraries. We do this by means of the USE command.

The USE command tells EAGLE which libraries to make available for searching and from which to source component data.

In your open schematic drawing, select a library to use by the following means: Libary > Use, or by

57

Chapter 4 - Creating Your First EAGLE Project

This will open a dialog box, allowing you to select the frames.lbr library. You can select the library by typing the name directly into the file name text area or, scrolling to and 2x , on the library name. (Alternatively you could simply execute the USE command by typing ‘USE frames.lbr’ into the command line).

For our first tutorial, you should now repeat the same technique as above, and USE the following component libraries: rcl.lbr, diode.lbr, microchip.lbr, linear.lbr, pinhead.lbr, supply1.lbr and special.lbr. We’ll select the needed components from these libraries shortly.

The ADD Command

To include objects in a drawing, from a library, we use the ADD command.

Adding a Frame

At this point we’ll use the ADD command to insert a frame into the drawing. (We’ll discuss this command in detail later). To do this simply in the command toolbar on the left side of the window. A panel will appear (see Figure 4-10 ) and you should expand the frames entry (by frames) and selecting the A4 landscape format frame (scroll down and Then press OK.

DINA4_L ).

Figure 4-10. Add frame dialog

EAGLE will then snap back to your schematic window, with a red outline of the frame attached to the cursor. Place the cursor at the desired bottom, left hand corner of your drawing and

58

.

Adding components from a Library

This will place a frame in to your schematic window. Then move and window.

at the top of the

(It would be preferable to place the bottom left hand corner of your frame at the drawing datum point as indicated in Figure 4-9. This will ensure the cursor co-ordinates correspond to positions within the frame.)

Your window should now look like that in the Figure 4-11.

Figure 4-11. New Schematic Editor Window with Frame Adding components from a Library

We can now proceed to add components or devices to our schematic. Again, in the command toolbar on the left-hand side of the window. The dialog box, as in Figure 4-12, will appear showing the libraries available for use.

59

Chapter 4 - Creating Your First EAGLE Project

Figure 4-12. Add device / select library dialog box

We are now going to add the components that comprise the project, and are listed in Table 4-2, to the schematic. As you can see these components are in different libraries, so we’ll have to add them from those libraries.

Table 4-2. Components List of Tutorial Project Part

Value

Device

Package

Library

C1

30p

C-EUC1206

C1206

rcl

C2

30p

C-EUC1206

C1206

rcl

C3

10n

C-EU025-025X050

C025-025X050

rcl

C4

47u/25V

CPOL-EUTAP5-45

TAP5-45

rcl

C5

47u

CPOL-EUTAP5-45

TAP5-45

rcl

D1

1N4148DO35-7

1N4148DO35-7

DO35-7

diode

IC1

PIC16F84AP

PIC16F84AP

DIL18

microchip 1

IC2

78L05Z

78L05Z

TO92

linear

JP1

PROG

PINHD-1X4

1X04

pinhead

JP2

APPL

PINHD-1X17

1X17

pinhead

XTAL/S

QS

special

R-EU_R1206

R1206

Q1 R1

60

2,2k

rcl

+5V

+5V

supply1

GND

GND

supply1

Adding components from a Library

We’ll start by adding the first component; a capacitor, labeled C1.

Now,`

rcl. This will open the library rcl.lbr directory tree within the dialog box (as in the

Figure 4-13). Expand the section C-EU by

.

You’ll now see, by scrolling down, the capacitor named C-EUC1026, together with descriptive information in the right-hand panes of this dialog. Select it by

on the correct component.

Figure 4-13. Add device dialog box

Now . EAGLE will skip back to the schematic window with the symbol for the capacitor highlighted in red, and connected & floating with your moving cursor. As you move your cursor you will see the coordinates in the upper left-hand of the window change. These give the cursor position, and therefore your component placement relative to the drawing datum.

Place your cursor, and the component in the desired location and simply command).

(to end the ADD

The capacitor has now been added to the drawing.

An alternate method of adding a component is from the EAGLE Control Panel. If you have a schematic drawing open you can use this technique.

61

Chapter 4 - Creating Your First EAGLE Project

Expand the libraries tree by

Libraries . Scroll down, using the middle scroll bar until you

see the rcl.lbr library. Expand it with .rcl.lbr. Now select the device C-EU by on it.

You will see a symbol diagram, a package diagram and some descriptions appear in the right-hand pane of the window as shown in Figure 4-14.

Figure 4-14. Component Description and Package in the Library

Move your cursor over to the right-hand pane and the first Device in the list (for example).

The word ADD should appear, underlined, to the right of the Device name (as in Figure 4-15).

Now, scroll down in the right-hand pane until you see ‘EUC1206’, then on ADD (see Figure 4-15 ). Now move your mouse to to the schematic drawing with that device ‘attached’ to the cursor, ready for placement. Place the device with

62

.

Adding components from a Library

Figure 4-15. Selecting a Device to add to a schematic

However, you may change the orientation of the component before placing it by repeatedly

.

The component will rotate through 90째 with each click.

You should now proceed to place all of the components from Table 4-2 into the drawing. After completing this, your drawing should look something like Figure 4-16.

Figure 4-16. Tutorial Schematic with only components

63

Chapter 4 - Creating Your First EAGLE Project

Working with Objects: the COPY, MOVE, and MIRROR Commands

You can manipulate objects in your drawing by using a set of commands designed for that purpose.

These are the the COPY, MOVE, ROTATE and MIRROR commands. They perform as their names suggest.

Using these commands you can correct any positioning of components. When using a command and you need to select a component, you should on the ‘+’ approximately in the centre of the component. This point is used to indicate the center of the device for manipulation.

To terminate a command at any time use

.

The COPY command allows you to replicate objects already in a drawing. Simply then on the object you wish to copy. To place the new device, where you would like the copied object to be placed.

and

on the point in the drawing

The MOVE command simply allows you to move an object to another point. You just then on the object you wish to move. Then, move the cursor to the desired position and place the object.

ROTATE allows you to rotate a device by With each

and then repeatedly

to

on the device.

the device rotates though 90°, anticlockwise.

The MIRROR command essentially ‘flips’ a device on its vertical axis, producing a mirror image of itself. All connections remain intact. The MIRROR command could be used when placing components on the ‘underside’ of a PCB, but when viewed from the top. To action the MIRROR command and then the PCB layout Editor.

64

on the device you wish to ‘flip’. This command is mainly used in

The UNDO and REDO Commands

The DELETE Command

The DELETE command is used to delete objects from a drawing or PCB layout.

If you’ve made some mistakes in the previous section while adding components to your drawing; don’t worry, they can be removed quite easily with the DELETE command.

You can use the DELETE command on most objects in a drawing including; components, wires, nets and buses. Simply and then be removed from the drawing.

on the object or component to be deleted. It will then

When using the DELETE command on nets, wires or buses, it deletes one segment at a time.

To delete the whole construct, press the while deleting the object. With the DELETE command you can also delete groups of objects (more about this later).

Similar principles apply to the use of the DELETE command in the PCB Layout Editor. You can delete any and all objects including; component devices, wires, pads, vias and text.

The UNDO and REDO Commands

The UNDO and REDO commands are the EAGLE user’s best friends.

They are executed using these icons: . for UNDO and to run the REDO command.

EAGLE keeps an unlimited undo function. This allow you to either immediately correct a inadvertent mistake, or “backtrack” through a long series of actions to a prior configuration.

The REDO command allows you to reverse an action performed by the UNDO command.

A very convenient facility within EAGLE is the UNDO LIST. You start the facility by Edit > Undo/Redo list...

A dialog box will then open similar that in Figure 4-17, displaying a list of actions that can be selectively done/undone. You should experiment with this function to become familiar with it.

65

Chapter 4 - Creating Your First EAGLE Project

Figure 4-17. Undo List The reader should note that all of the above commands can be used in the same way within the PCB Layout Editor.

Connecting Components Together The NET Command

The NET command is used to “draw” ‘signal’ connections between points e.g. between a pin on a semiconductor component and a connector pin. A ‘pin’ has a specific meaning in EAGLE, and defines a net connection point. A net defines the relationship between interconnected points on the same functional ‘signal’ or ‘electrical’ net(work). However, the net may not resemble the final, physical layout of any subsequent, wiring in the finished PCB. To show the pins in a schematic, use the DISPLAY command, and

. The familiar dialog

box will appear, as described above. Now 93 Pins and then . The drawing’s components’ pins should now be highlighted with a green circle. An enlarged section of the drawing illustrates this, in Figure 4-18.

66

The NET Command

Figure 4-18. Schematic with components & pins

Start the NET command by window.

. A small cross-hair cursor will appear in the schematic

You can now begin connecting the pins on each component, by using the NET command, to complete the schematic. on the first pin of the connection you wish to make, then navigate towards the terminating pin. The process looks like the Figure 4-19.

Figure 4-19. Drawing with the NET command

67

Chapter 4 - Creating Your First EAGLE Project

After starting the NET command, you will also see a new toolbar appear in the main toolbar area, across the top of the schematic. It looks like Figure 4-20.

Figure 4-20. The NET parameter toolbar

This toolbar allows you to change attributes before and while drawing the net. For the moment we’ll leave the default settings as they are. The left-most part of this toolbar has a series of angled and curved lines on it. These are known as ‘bend modes’. While using a NET command (i.e. the crosshair cursor is visible), you can change the bend mode of the net line by repeatedly the style indicator change across the toolbar.

. You will see

End the NET command by on the terminating pin. Try experimenting with this command, as it will be helpful when we deal with another command later in the PCB layout editor. If you make a mistake in connecting a net you can always remove it with the DELETE command.

The JUNCTION Command

If you connect one net line onto another , EAGLE generates a connection between the two nets. This can be set to occur automatically or be turned off by: Options > Set > Misc and selecting the Auto set junction option.

If the option is de-selected (set to manual) then you can create a junction between nets by using the JUNCTION Command. To do this: and a cross-hair cursor will appear in the drawing, associated with a light green dot. You can see this in action in Figure 4-21.

68

The NET Command

Figure 4-21. Using the JUNCTION command

Move the dot onto the intersection of nets you wish to join, and a dialog box with a warning will appear, similar to that in Figure 4-22.

Figure 4-22. NET merge warning dialog

This displays the net segment you wish to merge with an existing net. If this is what you want, then respond by

. This will place a connecting node at the junction selected.

The SHOW Command

The SHOW command is used to display names and other details of objects. It can be used on nets, signals, devices and components.

By way of example, to show the net ‘GND’, simply :

and then move the cursor to the

connection point of IC1 pin 5 (VSS) and . EAGLE will highlight the net wires and each pin connected by this net, as well as the pin name of each part to which it is connected. Also, the status bar (at the very bottom of the drawing window) will display ‘Net: GND, Class :1 power’. These are the details of this net.

69

Chapter 4 - Creating Your First EAGLE Project

The SHOW command remains active until terminated, which you can do by

or

.

You can also SHOW an object by activating the SHOW command and typing the name of the object in the command line, then . EAGLE searches for, and highlights, the object when it is found.

If EAGLE fails to find the object, a window appears with a ‘-‘ in the Sheet column of the display.

You can also select additional objects without the need to reactivate the SHOW command. You can cumulatively select objects by + on each object to be highlighted. ( highlighted object to remove the highlight).

again on a

Completing the Schematic Drawing

You should now, with a combination of the above commands and techniques, be able to complete the schematic drawing, as illustrated in Figure 4-23.

Figure 4-23. Tutorial Schematic Complete

There is one final step to finalizing the schematic, and to make sure is can be used to prepare a printed circuit board layout; the Electrical Rule Check (ERC).

The Electrical Rule Check (ERC) is used to test schematic drawings to ensure they are free from electrical errors, and to indicate possible sources of error before fabrication. This should be performed on every schematic drawing before finalizing it for other work. The ERC does not

70

The NET Command

diagnose errors - unfortunately that is up to you !

To invoke the ERC command as in Figure 4-24.

. The check will find 4 warnings in our demonstration file

Figure 4-24. Electrical Rule Check Warnings and Errors

These are: POWER Pin IC1 VDD connected to +5V POWER Pin IC1 VSS connected to GND Part F1 has no value Part Q1 has no value

The messages inform you that: i. the power pins are connected to signals other than expected. The power pins were named VSS or VDD in the library but are connected to GND and +5V. In the tutorial this has been done on purpose; ii. components F1 and Q1 have no assigned values. This is not critical, since F1 is the Frame around the drawing, and Q1 is the crystal. We can assign its value at a later time, if necessary.

It will not prevent us laying out a PCB, since we know its package type.

If you now on the first entry, EAGLE will show you, by using a line and box, the location of the reason for the problem in the schematic. We can remove them by each one in turn. However, this is not advised as a working technique, since warnings should be avoided or resolved.

71

Chapter 4 - Creating Your First EAGLE Project

If you haven’t been able to complete the demo drawing yourself, you may just simply keep it by File > Save as. A dialog box will open and you can save your tutorial at this point with whatever name you choose and EAGLE user interface skills.

. You can open it at any time to practice your

Creating a PCB Layout from a Schematic Drawing You may create a PCB (Printed Circuit Board) layout starting from either a schematic drawing or using only the PCB Layout Editor. We’ll continue our tutorial by choosing the option of using a schematic drawing as the starting point. In doing so we’ll use the EAGLE PCB Layout editor after, deriving all required information from the schematic.

If you haven’t already got the demonstration schematic file (demo1.sch) open, you should open it now by using File > Open, and then navigating to the file under projects > examples > tutorial. You’ll see the, now familiar, diagram as in Figure 4-25.

Figure 4-25. demo1 schematic drawing

72