Module 4: Schematic Capture
Module 4: Schematic Capture 4.1 Introduction to Schematic Capture.. 4-1 4.2 The Schematic Editor workspace... 4-2
4.2.1 4.2.2 4.3.1 4.3.2 4.3.3 4.3.4 4.4.1 4.4.2 4.4.3 4.4.4 Document Options...4-2 Preferences....4-8 Locating and loading libraries..4-9 Locating components...4-11 Browsing libraries....4-13 Exercises Libraries and components...4-14 Placing components...4-17 Pin-to-pin wiring....4-18 Exercise Drawing the schematic...4-19 Exercise The Sensor schematic...4-21
4.3 Libraries and components... 4-9
4.4 Placing and wiring... 4-17
Software, documentation and related materials: Copyright 2009 Altium Limited. All rights reserved. You are permitted to print this document provided that (1) the use of such is for personal use only and will not be copied or posted on any network computer or broadcast in any media, and (2) no modifications of the document is made. Unauthorized duplication, in whole or part, of this document by any means, mechanical or electronic, including translation into another language, except for brief excerpts in published reviews, is prohibited without the express written permission of Altium Limited. Unauthorized duplication of this work may also be prohibited by local statute. Violators may be subject to both criminal and civil penalties, including fines and/or imprisonment. Altium, Altium Designer, Board Insight, Design Explorer, DXP, LiveDesign, NanoBoard, NanoTalk, P-CAD, SimCode, Situs, TASKING, and Topological Autorouting and their respective logos are trademarks or registered trademarks of Altium Limited or its subsidiaries. All other registered or unregistered trademarks referenced herein are the property of their respective owners and no trademark rights to the same are claimed. Module Seq = 4
Introduction to Schematic Capture
The Schematic Capture training session covers how to create single sheet schematics and multisheet hierarchical projects from initial setup through to component placement, wiring, design verification and printing. The functionality of the Schematic Editor will be explored and a series of exercises will show you how to capture a design as a schematic, ready for PCB design. Figure 1 outlines the workflow to be followed when creating a schematic in Altium Designer. Design Concept & Specification

Create PCB Project

Add sheets & sheet symbols to build design hierarchy
Find and place components from libraries

Wire design

Annotate design
Compile and verify design

Add component parameters

Add PCB design requirements
Transfer design to PCB layout
Figure 1. The Altium Designer schematic capture workflow

Back annotate from PCB

The Schematic Editor workspace
This section describes how to set up and browse the Schematic Editor workspace, done via the Document Options and Preferences dialogs. Sheet options, such as grids and templates, as well as preferences and defaults can be set through these dialogs. To open the Schematic Editor, simply create a new schematic document (File New Schematic) or open an existing.SchDoc document in Altium Designer.

Document Options

The Document Options dialog allows you to: Set parameters relating to individual schematic files. The settings in this dialog are saved with that schematic file. The Document Options dialog is displayed by double-clicking on the sheet border, or by choosing the Design Document Options menu command.
The tabs of the Document Options dialog are described in the following sections.

4.2.1.1

Sheet Options tab
The Sheet Options tab of the Document Options dialog is shown in Figure 2. The options in each of the sections are explained below.
Figure 2. Sheet Options tab of the Document Options dialog

Template section

Displays the filename of the associated template, if any. Use the Template options in the Design menu to apply, update or remove the associated template. Set the default template in the DXP Preferences Schematic General.
Figure 3. Setting a default template to use when creating a new schematic.

Options section

Orientation Sets the sheet orientation to Landscape or Portrait. Title Block When checked, a standard title block is attached to the sheet. The format of that title block is set using the drop-down list next to this option. Note that this is typically only used when there is no associated template. Show Reference Zones When checked, the sheet has a reference grid defined in its border. A new option has also been added to have the zoning as per ASME Y14.1 standard. Show Border When checked the sheet border is displayed. Show Template Graphics When checked, any objects placed in the template file defined for the sheet will be displayed in the sheet. This is typically used to display a non-standard title block, in which case you would uncheck the Title Block option. Border Color Allows you to set the border color from the Choose Color dialog. Sheet Color Allows you to set the background color of the sheet.

Standard Style section

Allows you to select the size of the sheet from a number of standard sizes e.g. A4, A3.

Custom Style section

Allows you to define a custom sheet size and border. Use this option if you want a sheet size not covered in the Standard Style section.

Change System Font

This button allows you to change the font used to display pin numbers, pin names, port text, power port text and sheet border text.

Grids section

Grids Options allow you to set the size and turn on or off the Snap Grid and the Visible Grid.
SnapOn The Snap Grid forces the mouse click location to the closest snap grid point. The Snap Grid is set and can be turned on or off in the Document Options dialog. You can also cycle though three predefined grids by pressing the G shortcut key at any time. Visible The Visible Grid displays a grid when turned on. This is independent of the Snap Grid. The Visible Grid can also be turned on or off in the View menu (VV).

Electrical Grid section

The Electrical Grid can be turned on or off and the Electrical Grid Range can be set in the Document Options dialog. It can also be turned on or off in the View menu (VE). When the Electrical Grid is turned on and you are executing a command that supports the electrical grid, the cursor overrides the Snap Grid and jumps to key points on objects. For example, if you are using the Place Wire command and move the cursor to a certain distance within the Electrical Grid Range of a pin, the cursor will jump to the pin.

4.2.1.2

Parameters tab
The Parameters tab is used as a convenient method of editing sheet-level text. Each parameter is automatically linked to a text string on the sheet, where the text string is the same as the parameter name, except that it is preceded by an equals sign. For example, the Parameter Address1 is automatically linked to the text string =Address1. The equals sign is an instruction to the schematic editor to automatically replace the text string on the sheet with the value of a parameter with a name of Address1. Any number of these parameters can be added to a document, either a schematic template or a schematic sheet. Using these special strings allows template text properties, such as font, size and color, to be predefined in the template, while the actual text string value is defined when that template is applied to a schematic. This replacement occurs automatically during printing, it can also be performed on screen by enabling the Convert Special Strings option in the Graphical Editing tab of the Preferences dialog (Tools Schematic Preferences).

Figure 4. Parameters tab of the Document Options dialog
The default special strings are listed in the table below, but you can create custom parameters to suit your document and design requirements. Special String
=Address1 =Address2 =Address3

Description

Line of an address Line of an address Line of an address

Special String

=Engineer =ImagePath =Modified Date
Engineers name Path to image file Computer system date of last modification to file (value entered automatically) Organization name Revision number Rule description if added using Add as Rule option Schematic sheet number Total number of sheets in the project Time (not automatically updated) Title of schematic sheet Engineers name Path to image file
=Address4 =ApprovedBy =Author =Checked By =CompanyName =CurrentDate =CurrentTime =Date =DocumentFullPath AndName =DocumentName
Line of an address Approvers name Authors name Checkers name Company name Computer system date (value entered automatically) Computer system time (value entered automatically) Date (not automatically updated) Filename with full path of the schematic sheet (value entered automatically) Filename without the path (value entered automatically) Document number Draftspersons name
=Organization =Revision =Rule =SheetNumber =SheetTotal =Time =Title =Engineer =ImagePath

=Modified Date

Computer system date of last modification to file (value entered automatically)

=DocumentNumber =DrawnBy

Table 1. List of default parameters when creating a new schematic
Figure 5 shows how Special Strings are entered in a title block. Text entered as the value of a parameter in the Parameter tab will display where the special string is placed. The properties of the special strings (i.e. font, color) determine the properties of the text that is displayed. You place special strings by selecting Place Text String and then pressing the TAB key. The Annotation dialog displays. Clicking on the down arrow in the name field lists a special string for each of the parameters defined. Click on the string required and place it. Special strings display their content when the Convert Special Strings option is selected in the Graphical Editing tab of the Preferences dialog (Tools Schematic Preferences), or when the schematic is printed or plotted.
Figure 5. Special strings in a title block, with and without the Convert Special Strings option enabled

4.2.1.3

Units tab
The Units tab allows you to define the various units used in the Schematic Editor. Grids will be a multiples of these units so for example, using the DXP Default Units in which each unit is equal to 10 mils, a Snap Grid value of 5 (or 5 units) would equate to 50 mils, 10 units = 100 mils, etc. when printed actual size or 1:1.
Figure 6. Units tab of the Document Options dialog

Imperial Unit System Section
Use Imperial Unit System Check this option to use imperial units in your schematic(s). You will also want to specify which imperial units to be used (DXP defaults - 10 mil, mils, inches and auto imperial units) in the Imperial unit used drop down list. Imperial unit used This option is used to select from one of the available imperial units; mils, inches, DXP default units (10 mils) and auto imperial. If the Auto-Imperial unit is selected, the system will switch from mils to inches when the value is greater than 500 mils.
Metric Unit System Section
Use Metric Unit System Check this option to use metric units in your schematic(s). You will also want to specify which metric units to be used (millimeters, centimeters, meters, and Auto-Metric units) in the Metric unit used drop down list. Metric unit used This option is used to select from one of the available metric units; millimeters, centimeters, meters, and Auto-Metric. If the Auto-Metric unit is selected, the system will switch from millimeters to centimeters when the value is greater than 100 centimeters.

4.2.1.4

Using templates
Standard sheet templates (*.SchDot) are supplied with Altium Designer and are accessible in the \Altium Designer Summer 09\Templates\folder. You can also create your own templates and store them anywhere. Select Design Template Set Template File Name. This option removes any existing template and uses the one you choose. Select Design Template Update. Use this command when a template is modified and you need to refresh the sheets which use it. Select Design Template Remove Current Template. This option removes the template but retains the old sheet size from the old template.
For each of these commands you will be prompted to indicate if the change is to apply to the current sheet, all open, or all in project.

Preferences

The Schematic section of the Preferences dialog allows you to set up parameters relating to the Schematic Editor workspace. This dialog is displayed using the Tools Schematic Preferences menu command. Settings in this dialog are saved in the Altium Designer environment and therefore remain the same when you change active schematic documents. For help with the options available in the preferences, use the then click on the option more information is required on. button in the preferences dialog;

Libraries and components

This section explores the Altium Designer libraries and how to find schematic components within them.
Locating and loading libraries
The supplied components are stored within a set of Integrated Libraries. An integrated library includes the schematic symbols, plus it can also include all associated models, such as footprints, spice models, signal integrity models, and so on. Most of the supplied integrated libraries are manufacturer-specific. Integrated libraries are compiled from separate source schematic libraries, PCB footprint libraries, etc. The components in an integrated library cannot be edited, to change a component the source library is edited and recompiled to produce an updated integrated library. There are a number of other special purpose integrated libraries, e.g. special function simulation components. Components can also be placed directly from schematic symbol libraries if this is preferred to integrated libraries, and you can also place them from Protel 99 SE format schematic symbol libraries. Available components are listed in the Libraries panel. The libraries presented in this panel include: Libraries in the active project. If the project that the currently active document belongs to includes any libraries, they are automatically listed.
Figure 7. Available Libraries dialog, showing the project tab which is libraries in the current project
Installed libraries. Installed libraries are those that have been made available in the environment. Use this option for company libraries that are used across different projects.
Figure 8. Available Libraries dialog, showing the installed tab which is available to any open project.
Libraries found down the defined project search path. This option is particularly useful for accessing simulation models. Search paths are defined in the Project Options dialog.

4.3.1.1

Adding a library to make its components available
1. To add a library, press the Libraries button in the Libraries panel or select Design Add/Remove Library. The Available Libraries dialog displays. 2. Click on the Install button at the bottom of the Installed Tab of the dialog. 3. Navigate to the required libraries directory and click on a library to select it. The library you selected will now be listed in the Installed Libraries list in the dialog. 4. Click Close when you have installed the libraries you need.

Figure 9. Available Libraries dialog, use the Installed tab to install or
Note: The supplied integrated libraries are located in the: \Program Files\Altium Designer Summer 09\Library\ folder.

4 - 10

Locating components
When the location of the library isnt known, use the Search button in the Libraries panel or the Tools Find Component menu command. The Libraries Search dialog displays. The first time this dialog is executed, the dialog shown in Figure 10. is displayed. This initial mode is referred to as Simple mode. In Simple mode each searchable field has to be entered either manually or from a list of drop down items found within the currently installed libraries. After the field data is entered such as Name for example, an operator and value needs to be entered. The operator can be selected from a drop down list of Equals, contains, starts with and ends with. The value field can also be selected via a drop down of values found within the currently installed libraries or typed manually.
Figure 10. Simple view for library search dialog
Once data is entered, press the search button and a search starts. Going back to the search dialog and press the Advanced hyperlink button, the query string for the filter created in Simple mode is displayed. Depending on current knowledge of the query language in Altium Designer, it is recommended, new uses use the Simple mode and users familiar with the query language use the advanced mode to manually type the exact search query.

4 - 11

Figure 11. Advanced view for Search Libraries dialog
Tips for finding components: The search dialog uses a standard query to search the libraries if the string you type does not include a query keyword it is assumed that the text is either part of the component Name or Description and a query is built automatically, as shown in Figure 11. The default search Scope is Available libraries that are those libraries currently listed in the Libraries panel. Change this to Libraries on path to search across all the supplied libraries. Search results are presented in the Libraries panel note that the drop down where you select the current library will change to Query Results. If you attempt to place a component in the query results from a library that is not currently installed you will be asked if you wish to install that library now, you can still place without installing the library if you wish. The search can be terminated as soon as an instance of the part is found by clicking the button on the Libraries panel. If your search does not produce results, check that the search path is correct. Also, try searching for a component you know exists in a library to check that everything is set correctly
Note: When you are searching libraries, check that the Filter field at the top of the Libraries panel has nothing in it. If there is any thing other than a *, then the search results will be further filtered, as shown in Figure 12.

Figure 12. Ensure that the filter field is clear during searching.
. Module 4: Schematic Capture 4 - 12

Browsing libraries

The Libraries panel gives access to all components that are currently available to be placed. In the Panel control, bottom right, select System Libraries. Click the Libraries button to display the Available Libraries dialog. This dialog displays all components currently available to be placed in the active project. Select the Installed tab, and click the Install button to add libraries to the library list. Components contained in the selected library are listed in the box below the Filter field. The Filter allows you to control what component names are listed, e.g. RES* will display only component names starting with RES. You can also type directly in the list of components, the type-ahead feature will automatically jump through the list as you type. Press ESC to stop performing a typeahead action. Clicking on the name of a component will: display that component symbol in the viewer in the middle of the panel, list the associated models below that, and show the selected footprint model below that. The Place button places the component currently selected. Double-clicking on the name of a component also achieves this. The Search button is a powerful searching tool, allowing you to search through libraries for parts. Clicking this button pops up the Libraries Search dialog.
Figure 13. Browsing libraries with the Schematic Editor Panel
If a component has several parts, the sub-parts will be shown in the symbol mini-viewer. You can control what columns are displayed in the component or model lists, right-click and choose Select Columns to do this. Using this with database libraries is especially useful as there is the ability to sort by a particular column like shown in Figure 14. Database libraries are covered in more detail in the Advanced PCB training course.

4 - 13

Figure 14. Using a database library and the sort by column feature to sort by Value. n

4.3.4.1

Exercises Libraries and components
Locating and loading libraries when the required library is known
The training design is a microcontroller driven temperature sensor. To install one of the supplied libraries and see if it includes a PIC microcontroller library, complete the following steps: 1. Open a schematic document to activate the Schematic Editor. 2. Click the Libraries button on the Libraries panel to display the Available Libraries dialog. 3. Select the Installed tab of dialog, then click the Install button and navigate to the \Program Files\Altium Designer Summer 09\Library\directory. This directory contains sub directories containing the integrated libraries supplied with Altium Designers Schematic Editor. 4. Scroll down through the library directories. Open the Microchip folder, select and add the Microchip Microcontroller 8-Bit PIC16.IntLib. 5. Click the Close button to close the Available Libraries dialog. 6. Select this Microchip library in the list of libraries at the top of the Libraries panel. The librarys contents will be displayed in the box below the Filter field section. Confirm that the library includes a PIC16C773/SO.

4.3.4.2

Finding components when their library is unknown
Often you will want to locate a component but do not know which library it is in, or you may want to see what family types are available in the libraries. To search for components, we use the Search button or the Tools Find Component menu command. 1. Click on the Search button and the Libraries Search dialog will appear. 2. For this exercise, Advanced mode is going to be used on the Library search dialog. Click on the Advanced Hyperlink button. 3. Set the Scope to Libraries on path and set the search Path to C:\Program Files\Altium Designer Summer 09\Library (the Include subdirectories option should be on).

4 - 14

4. The power supply in the training design uses a LM317MSTT3 adjustable regulator. To search the supplied libraries for a suitable device type the string LM317 in the Search field at the top of the dialog and click the Search button. 5. Note that the library currently being searched is listed in the Libraries panel. Depending on the speed of the PC it will take a few minutes to search the entire 90,000+ components for the required part. 6. The result set should include components in the ON Semi Power Mgt Voltage Regulator.IntLib, confirm that the LM317MSTT3 part is listed. 7. To install this library so that component will be available later you can either right-click in the result list and select Add or Remove Libraries (this will simply open the Available Libraries dialog), or you can double-click on the component name in the list to place it (you can easily delete it if it is the wrong sheet), when you do the Confirm dialog will appear, giving you an opportunity to Install the library.

4.3.4.3

Locating components within an open library
1. Select the library Miscellaneous Devices.IntLib in the Libraries panel. This library is one of two PCB libraries installed by default when the software is installed. It includes a variety of discrete components, including resistors, capacitors, diodes, etc. 2. Type cap into the Filter field. Notice that only the capacitor-type components are listed. 3. Try diode in the Filter field. The only components listed now are the diodes whose library reference starts with the string diode. 4. Now try *diode, this time components that include the word diode anywhere in their name or description will be listed.

4.3.4.4

Finding footprints when their library is unknown
1. Footprints can be searched for in the same way as component symbols; the only difference is that you need to set the Search in, in the Libraries Search dialog to Footprints before pressing the Search button. 2. Set the Search Path to C:\Program Files\Altium Designer Summer 09\Library\Pcb\IPC-7350 Series\.

4 - 15

Figure 15. Searching for a footprint
3. Enter the string 2012 and click Search. The search results will include a number of libraries, including IPC-7352 Chip_Resistor_N.PcbLib. 4. Double-click on the RESC2012N footprint in the query results, a dialog will appear letting you know that the library is not currently installed, click Yes to install the library.

4.3.4.5

Setting the library search order
When you type in a component name, for example in the Place Part dialog, or when you type in a footprint name in the Footprint Model dialog, the available libraries are searched in a defined order. This search order is the order that the libraries are listed in the Available Libraries dialog. To configure the search order: 1. Click the Libraries button in the Libraries panel to display the Available Libraries dialog. 2. Click on the Installed tab, then in the list of Installed Libraries click to select the IPC-7352 Chip_Resistor_N.PcbLib to highlight it, and then click the Move Up button to move it to the top of the list. 3. Close the Available Libraries dialog. You now have all the components and footprints required to complete the training design. Note: Refer to the PDF, AR0104 Component, Model and Library Concepts article in the online documentation for further information on definitions, library search order and component to model linking.

4 - 16

Placing and wiring
This section looks at how to place components and then wire them together. The exercise takes you through the creation of a complete schematic sheet.

Placing components

To place a component, double-click on its name in the Libraries panel. To edit a components properties before you place it, press the TAB key. The Component Properties dialog displays. To step through the fields in the dialog press TAB (down), or SHIFT+TAB (up). New text will overwrite text that is selected. If you set the component designator before placing the component, then subsequent components will be automatically designated with the next designator value. You can also use the Place Part menu command if you know the name of a component. When you select this command, you are prompted for the name of the component. Once you type the component name in, the open libraries are searched and if the component is located, it becomes attached to the cursor for placement.
Figure 16. Place part dialog

4.4.1.1

Auto-incrementing designators
When placing a component, if the initial designator is set before placing, its designator will be assigned by incrementing the designator of the last component placed. This will only occur for subsequent parts placed after the TAB key was pressed to assign the initial designator. Once you stop placing this type of part, the next designator in the sequence is no longer remembered.

4 - 17

Generally it is easier to leave the annotation of designators until the design is complete to allow the designators to be assigned in a logical and controlled manner on each sheet. Annotation is covered in detail later in Module 6 - Building the Project.

Pin-to-pin wiring

Wires are used to create an electrical connection between points. Be careful to use Place Wire and not place lines by mistake. Press SHIFT+SPACEBAR to change the wire placement mode. Press SPACEBAR to toggle between start and end corner modes. Press BACKSPACE to delete the last vertex placed. A point on a wire must touch on the connection point of an electrical object to be connected to it, e.g. the wire must touch on the hot end of a pin to connect to it. Use buses to graphically represent how a group of related signals, such as a data bus, are connected on a sheet. Also, use buses to connect related signals to ports and sheet entries. Buses must use the bus name / bus element referencing system as shown in Figure 20, and must include the individual net labels and the bus net label. The bus range can increment [0.7], or decrement [7.0]. To move a component on the schematic and maintain the wiring (referred to as dragging), hold the CTRL key as you click, hold and move the mouse (release the CTRL key once you start dragging). Press the SPACEBAR or SHIFT+SPACEBAR while dragging to change the wiring mode. Press the M shortcut to drag a selection. If you are having trouble seeing the grid in schematic goto Tools Schematic Preferences Schematic Grids and change the Grid Color to one that is not so white.
Figure 17. Grids setting in preferences

4 - 18

Exercise Drawing the schematic
Figure 18. MCU schematic example
1. If it is not already open, re-open the project created during the Module 1 - Getting Started With Altium Designer, \Program Files\Altium Designer Summer 09\Examples\Training\PCB Training\Temperature Sensor\Temperature Sensor.PrjPcb. 2. Add a new schematic document to the project, to do this right-click on the project file name in the Projects panel and select Add New to Project Schematic. 3. Right-click on the new schematic sheet in the Projects panel, and select Save As from the context menu. Save the schematic as MCU.SchDoc in the \Program Files\Altium Designer Summer 09\Examples\Training\PCB Training\Temperature Sensor folder. 4. Set the template for your schematic to A4.SchDot by choosing Design Template Set Template File Name and choosing the A4 size template from \Program Files\Altium Designer Summer 09\Templates folder. 5. Verify that the electrical grid is on and set to 4 and that the snap grip is on and set to 10 before placing any objects (double-click in the sheet border to open the Document Options dialog). 6. Draw up the schematic shown in Figure 18 above. When placing the components, press TAB to define the Designator and Comment (component value) before placing the component. Component Microcontroller Resistors Capacitor Library Reference PIC16C773/SO Res1 Cap

7. To rotate a component press the SPACEBAR, press the Y key to flip it vertically, and the X key to flip it horizontally. 8. Set the Port I/O Type to match their display Style. Set the Ground Style power port net attribute to GND. 9. Set the bus name and port name to RB[0.7] so as to connect nets RB0 through to RB7 into a bus. Module 4: Schematic Capture 4 - 19
10. To build up the nets in the bus, first create the port on the right. Copy the port and run Edit Smart Paste. Select Ports from the left side and select net labels and wires on the right side. On the bottom section of the dialog select expand buses for signal names. You can also set the wire length to suit. Note that the spacing between the wires well be as per the current grid setting which should be on 10 so the wires and netlabels line up to the pins of the component.
Figure 19. Smart paste dialog to create the netlabels and wires that make up the signals on a bus.
Figure 20. Buses are defined using the referencing system shown.

4 - 20

11. While placing the resistors and capacitors you can use the component cut wires feature to quickly cut into the wires rather than wiring around them. 12. While placing some of the ports and power ports hold down the ctrl key and drag to extend the wires with the object. This can save a lot of time when getting to the wiring stage. 13. Enter the necessary document information in the Parameters tab of the Document Options dialog. Enter the title as PIC Microcontroller. Dont worry about setting the sheet/Document No. at this time as there is a feature that can do this automatically over your whole project.
Exercise The Sensor schematic
At this stage in the training, your Temperature Sensor project should look like Figure 21. However, the Sensor.SchDoc and the project libraries are not there as yet. To complete it: 1. Create a new schematic and call it Sensor.schdoc if you havent done so already. 2. Save and close the Sensor.SchDoc sheet. Note that this sheet is just a blank schematic for now. Itll be completed later in the training. 3. Also youll need to add the library files as shown in Figure 21 to the project and save the project PCB. At this point we are only going to create a blank sheet. In Module 15 - Schematic Library Editor, we will create the sensor sheet after creating a new component. The last step to complete the sensor design is to add the top schematic sheet which is done in the next module Module 5 - MultiSheet Design.
Figure 21. Project structure after completing the MCU schematic.

4 - 21

Module 1: Getting Started With Altium Designer
Module 1: Getting Started With Altium Designer 1.1 Introduction to Altium Designer.. 1-1
1.1.1 1.2.1 1.2.2 1.2.3 1.2.4 1.3.1 1.4.1 1.4.2 1.4.3 1.4.4 1.4.5 1.4.6 1.4.7 1.4.8 1.4.9 1.4.10 The Altium Designer Integration Platform..1-1 The Altium Designer Project...1-3 Demo Opening an existing Project..1-3 Editor View....1-4 Exercises Navigating around Altium Designer..1-5 Working in a document editor..1-6 Creating a new project...1-10 Adding a new document to the project..1-11 Adding an existing document to a project...1-11 Moving or copying a document between projects..1-11 Removing a document from the project..1-11 File management with the Storage Manager..1-12 Including other files in the Altium Designer project..1-12 Libraries....1-13 Project Packager...1-13 Exercise Working with projects and documents..1-14
1.2 The Altium Designer environment.. 1-2
1.3 Document Editor Overview.. 1-6 1.4 Working with projects and documents... 1-10
Software, documentation and related materials: Copyright 2009 Altium Limited. All rights reserved. You are permitted to print this document provided that (1) the use of such is for personal use only and will not be copied or posted on any network computer or broadcast in any media, and (2) no modifications of the document is made. Unauthorized duplication, in whole or part, of this document by any means, mechanical or electronic, including translation into another language, except for brief excerpts in published reviews, is prohibited without the express written permission of Altium Limited. Unauthorized duplication of this work may also be prohibited by local statute. Violators may be subject to both criminal and civil penalties, including fines and/or imprisonment. Altium, Altium Designer, Board Insight, Design Explorer, DXP, LiveDesign, NanoBoard, NanoTalk, P-CAD, SimCode, Situs, TASKING, and Topological Autorouting and their respective logos are trademarks or registered trademarks of Altium Limited or its subsidiaries. All other registered or unregistered trademarks referenced herein are the property of their respective owners and no trademark rights to the same are claimed. Module Seq = 1
Introduction to Altium Designer
Underlying the Altium Designer environment is a software integration platform that brings together all the tools necessary to create a complete environment for electronic product development, in a single application. Altium Designer includes tools for all design tasks: from schematic and HDL design capture, circuit simulation, signal integrity analysis, PCB design, and FPGA-based embedded system design and development. In addition, the Altium Designer environment can be customized to meet a wide variety of user requirements.
The Altium Designer Integration Platform
When you select All Programs Altium Designer Summer 09 from the Windows Start menu to run Altium Designer, you are actually launching DXP.EXE. The DXP platform underlies Altium Designer, supporting each of the editors that you use to create your design. The application interface is automatically configured to suit the document you are working on. For example, if you open a schematic sheet, appropriate toolbars, menus and shortcut keys are activated. This feature means that you can switch from routing a PCB, to producing a Bill of Materials report, to running a transient circuit analysis, and so on and the correct menus, toolbars and shortcuts will be readily available. Also, all toolbars, menus and shortcut keys can also be configured to suit how you like to configure your design environment.

Figure 1. Altium Designers software integration architecture
Module 1: Getting started With Altium Designer
The Altium Designer environment
The main document editing area of Altium Designer, shown on the right side in Figure 2. The Workspace Panels. There are a number of panels in Altium Designer, the default is that some are docked on the left side of the application, some are available in pop-out mode on the right side, some are floating, and others are hidden.
The Altium Designer environment consists of two main elements:
When you open Altium Designer, the most common initial tasks are displayed for easy selection in a special view, called the Home Page.
DXP System Menu Use this menu to set up system preferences and customize the environment. All other menus and toolbars automatically change to suit the document being edited.
Document bar A tab appears for each open document.
View Navigation Click on the arrows to go back and forth between views.
Workspace panels More pop out panels are displayed by clicking on these tabs. These panels can also be moved, docked or clipped.
Workspace panels These include Files and Projects panels. These panels can be moved, docked or clipped by clicking on the panel title and dragging it to a new location. Click on the tab at the bottom of the panel to display its contents.
Home Page Design View Common tasks are listed to get started quickly.
Panel Control Editor specific and shared panels can be displayed using these Panel buttons.
Figure 2. Altium Designer with the DXP Home Page displayed.
Note: To move an individual panel, click and hold on the panel name. To move a set of panels, click and hold on the panel caption bar away from the panel name. To prevent panels stacking together, hold the CTRL key. To change a docked panel to pop-out mode click the small pin icon at the top of the panel, to change it back to docked click the pin icon again.
Note: If you manage to completely ruin your panel layout and wish to revert back to the factory settings, this can be done by going to the View Desktop Layouts Default. Its best to restart Altium Designer when you run this. To save a custom layout go to View Desktop Layouts Save Layout. To reload existing layouts go to View Desktop Layouts Load Layout.
The Altium Designer Project
The basis of every electronic product design is the project. The project links the elements of your design together, including the source schematics, the PCB, the netlist, and any libraries or models you want to keep in the project. The project also stores the project-level options, such as the error checking settings, the multi-sheet connectivity mode, and the multi-channel annotation scheme. There are six project types PCB projects, FPGA projects, Core Projects, Embedded Projects, Script Projects and Library Packages (the source for an integrated library). Altium Designer allows you to access all documents related to a project via the Projects panel. Related projects can also be linked under a common Workspace, giving easy access to all files related to a particular product your company is developing. When you add documents to a project, such as a schematic sheet, a link to each document is entered into the project file. The documents can be stored anywhere on your network; they do not need to be in the same folder as the project file. If they do exist in a directory outside where the project exists or its sub-directories, then a small arrow symbol appears on the documents icon in the Projects panel.

Demo Opening an existing Project
1. Select the File Open Project menu to display the Choose Project to Open dialog. 2. Navigate to the project folder, 4 Port Serial Interface, located in the \Altium Designer Summer 09\Examples\Reference Designs directory. Locate 4 Port Serial Interface.PRJPCB (the project file) and double-click on it to open it. 3. The design will now be listed in the navigation tree of the Projects panel. 4. Click on the signs to contract the folders. 5. Click on + (plus) signs to expand folders. 6. Right-click on the project name (4 Port Serial Interface.PrjPcb) to display the context sensitive Projects menu.
Figure 3. The open project is displayed in the Projects panel.

Editor View

Each different document kind is edited in an appropriate Document Editor, for example the PCB Editor for a PCB document, Schematic Editor for a schematic document, or VHDL Editor for a VHDL document. Figure 4 shows a schematic open for editing in the Schematic Editor.
Figure 4. A schematic open for editing in the Schematic Editor View.

1.2.3.1

Document Tabs in the Documents Bar
Documents that are open are allocated a tab at the top of the application. Click on the relevant tab to display that document and make it the active document for editing. To switch between documents the Ctrl + Tab shortcut can be used. You can also tweak how Ctrl + Tab works in the preferences.
Figure 5. Tabs showing various documents open, note how the PCB tab is highlighted, indicating that it is the document currently being edited.
Right-click menu in the Documents Bar 1. Right-click on any document tab in the Documents bar. 2. Select Tile All from the floating menu that appears. All the opened documents are tiled in multiple screen regions. Note: The number of opened documents determines the number of regions. 3. Right-click on a document tab. 4. Select Close from the menu.
5. Position the cursor at the point where two regions of a split screen meet and a doubleheaded arrow will display. Click and drag to resize. 6. Right-click on any one of the tabs in the tiled display and choose Merge All. Notice that you have converted a split screen back to a single view. Note: Altium Designer supports multiple monitors. If your PC has multiple monitors you can use the Open in New Window command when you right-click on a document, or just drag and drop on to the second monitor and this will cause it to open in a separate Altium Designer application frame.

The right click menu also has options for saving and hiding individual documents as well as groups of documents like groups of schematics. Note: There are a few options that you can tweak to gain more control of how the document bar works in Altium Designer. To do this go select DXP Preferences and open the System View page. At the bottom right is the Documents Bar section where things like auto hide, multiline, ctrl-tab to switch can be set up.
Figure 6. Document Bar options in Preferences

1.2.4.1

Exercises Navigating around Altium Designer

Using the Projects panel

1. Open 4 Port Serial Interface.PRJPCB, located in the \Altium Designer Summer 09\Examples\Reference Designs\4 Port Serial Interface folder. 2. Expand and then contract the contents of the navigation tree. 3. Double-click on a document in the Projects panel to open it. 4. Double-click on a few more documents in the Projects panel to open them. 5. Right click on the documents bar to see all the options. 6. Tweak some of the settings in preferences and see the results.

Document Editor Overview

To display a document in its editor, double-click on a document icon in the Projects panel. The document will be opened in the appropriate editor, e.g. Schematic Editor, PCB Editor or the Library Editors. When you create a new document in a design you are required to select a document type, e.g. Schematic or PCB. The document type you select determines which editor is assigned to the document.
Working in a document editor
The sections below describe various elements in the user interface of the Altium Designer document editors.
Toolbars Schematic Editor displaying the active schematic document.
The Projects panel shows all open projects, and all documents in each project. Icons to the right of each document indicate if that document is open, hidden and/or modified.
Context-sensitive right-click pop-up menu
The Mask Level button allows you to change the level of dimming of unmasked objects. Click Clear to clear the current mask. The Selection Memory button saves selections. The Highlight button allows you to click to highlight nets, press Space or Shift Space to change the behavior.
The Clear button will clear any filter that has been applied to the document.

Status bar

Workspace panels Click on these buttons to display the various workspace panels.
Figure 7. Schematic Editor Workspace

1.3.1.1

Altium Designer menus are similar to standard Windows menus. Standard operations, e.g. opening, saving, cut, paste, etc. are consistent across editors. Right-click on an empty space on the menu bar or a toolbar caption to open the Customization Editor and customize any of the resources for that editor.

1.3.1.2

Shortcut keys and pop-up menus
Menu commands can also be accessed using shortcut keys. The underlined letter indicates the shortcut key for a menu command, e.g. press F for the File menu. 1-6
Special shortcut keys give direct access to both menus and sub-menus in the graphical editors, e.g. pressing F in the Schematic Editor will pop up the File menu and pressing S will pop up the Select sub-menu. Note : You can gain a list of every shortcut that is available in Altium Designer by looking for a document named GU0104 Shortcut Keys.PDF located in the Help directory of the Altium Designer Installation.

1.3.1.3

Toolbars
Toolbars can be fixed to any side of the workspace or they can be floated. Click and drag to move a toolbar. The cursor must be within the toolbar but not actually on a button. Toolbars can be reshaped, hold the cursor over the edge of the toolbar and when the resizing cursor appears click and hold to reshape. New toolbars can be created and existing toolbars edited. Multiple toolbars can be active, right-click on a toolbar to pop up the toolbar display control menu.

1.3.1.4

System and Editor Panels
Altium Designer uses two types of panels system-type panels, such as the Files, Messages or Projects panels that are always available, and editor panels, such as the PCB, schematic library or PCB library panels that are only available when a document of that type is active. Panels can float, or be docked, on any edge of the Altium Designer workspace. Docked panels can be pinned open, or set to unpinned, where they pop out when their name button is clicked. Panels can be clipped together in a set by dragging and dropping one on another, and then dragged around as a set by clicking and dragging on the area of panel title bar that contains no text or icons. A panel can be unclipped from a set by clicking and dragging on the panel name. Panels can be prevented from docking on particular edges. Right-click on a panel title bar to configure this. Note : The hide and display speed of unpinned panels is configured in the System View page of the Preferences dialog (DXP Preferences). It can be useful to turn off the animation of panels on slower machines.

Figure 8. Configuration for panel control

1.3.1.5

Status Bar
The Status Bar is used to display information to the user. The Status Bar consists of three display fields divided by separators and a set of panel display buttons. These three display fields are: Cursor position Prompt Options.
The fields can be re-sized by clicking and dragging on the separators.
The Status Bar is turned on and off using the menu command View Status Bar. The panel display buttons can be added or removed from the Status bar by clicking on the arrow button in the far bottom left.

1.3.1.6

Tool Tips
Tool Tips provide a brief description of how to use a particular function. Position the cursor over a toolbar button and leave it stationary for about a second and the Tool Tip will appear.

1.3.1.7

Right mouse click context sensitive pop-up menus
Altium Designer makes extensive use of context sensitive right mouse menus, including in panels and dialogs. Right-click anywhere in the environment to pop up a context sensitive menu of commands at the current cursor position. Supported right-click locations include: in a document editor, on an object in a document editor, in free space in the different sections of a panel on the Status bar on a toolbar or menu bar In dialogs, especially those with a grid of information.
Figure 9. Context sensitive right mouse menus are available throughout Altium Designer

1.3.1.8

Dialogs
Dialogs are used to set the parameters for various commands and objects.

SHIFT+TAB

To move from one field to another in a dialog, press the Tab key or use the mouse. takes you in the reverse direction.
Most fields will have an underlined character associated with them that can be pressed (in combination with the ALT key) as an alternative to a mouse click. When a field is highlighted, typing can overwrite it. Youll find nearly all dialogs will have a question mark icon in the top right hand corner. Clicking on this icon activates the Whats This Help (WTH) feature and will display a brief pop-up help message from the next control that you click on. For example, Figure 10 shows the WTH for the Type control in the component properties dialog.
Figure 10. Using the Whats This Help icon to gain help in a dialog

1.3.1.9

Undo/Redo
Most commands can be undone or then redone using the Undo and Redo toolbar buttons. The number of schematic editor and PCB editor undos is set in the Preferences dialog (DXP Preferences). The shortcut keys for Undo are CTRL+Z or ALT+BACKSPACE, and CTRL+Y or CTRL+BACKSPACE for Redo.

Working with projects and documents
A project is a set of documents that together define all aspects of your design: including schematic sheets, PCB documents, database link definition files, output job definition documents, netlists, and so on. Each project results in a single implementation, for example a PCB project results in one PCB design, and a library package project results in a single integrated library. Each document in the project is stored as a separate file on the hard drive. The project file itself is also an ASCII document, which includes links to the documents in the project, as well as storing project-level settings.

Creating a new project

To create a new PCB project: 1. From the Main Menu, select File New Project PCB Project.
Figure 11. The new project is displayed in the Projects panel
2. Select Save Project As from the File menu to name and save the project document or you can right click on the project in the Projects Panel and select Save Project As. 3. The new project is ready to add new or existing documents to.

1 - 10

Adding a new document to the project
To add a new document to the project: 1. Right-click on the Project name in the Projects panel, and from the Add New to Project sub-menu, select the document kind, for example, Schematic. 2. Right-click on the new schematic document in the Projects panel and select Save As to name and save the schematic.
Adding an existing document to a project
Figure 12. New schematic added to the
To add an existing document to a project: 1. Right-click on the Project name in the Projects panel. 2. Select Add Existing to Project in the menu to display the Choose Document to Add to Project dialog. 3. Navigate to locate required file and select it. 4. Click on Open to add it. The document is added into the currently active project. Note that when you add a document to a project a link is added in the project file to that document. The document can be located anywhere on the hard disk (or network). The document icon graphic indicates which Editor will be used to edit the document, e.g. a PCB document will have a PCB icon, indicating that it will be opened by the PCB Editor. Note: You can add a document to a project using a two step process. First drag the document from the Windows File Explorer into the Altium Designer Projects panel and then when it appears as a Free Document, click and drag it into the project.
Moving or copying a document between projects
1. Since documents are only linked into the project, you can easily move a document from one project to another simply by clicking and dragging it. 2. To copy a document to another project, hold the CTRL key as you click and drag.

Removing a document from the project
To remove a document from a project, right-click on the document icon in the Project panel and select Remove from Project. Note: The document is not deleted from the hard disk, but it is no longer linked into the project.

1 - 11

File management with the Storage Manager
The Storage Manager is a system panel that allows you to perform a variety of file management tasks. When you open the Storage Manager (View Workspace Panels System Storage Manager) it presents a folder/file view of the active projects documents. The Storage Manager can be used for: General everyday file management functions such as renaming and deleting files in the project or within the active projects folder structure. Management of Altium Designer backups, using the Local History feature. As a Subversion compliant interface for your Altium Designer projects. Note: Right-click in the different regions of the panel for options. As a CVS compliant (Concurrent Versions System) interface for your Altium Designer projects. As an SCC (Source Code Control) compliant version control interface for your Altium Designer projects. Performing a physical and electrical comparison of any 2 versions in the Local History, or the CVS Revision list.
The Folders view on the left gives access to documents stored in the project folder hierarchy. Next to this the File list shows all documents in the selected folder. A number of highlighting modes are used to indicate the state of each document, press F1 when the cursor is over the panel for information on highlighting.
Figure 13. Use the Storage Manager to manage project files on the hard disk, and to interface to your Version control system.
Note: Press F1 over the panel for access to detailed help.
Including other files in the Altium Designer project
You can include any file in your Altium Designer project, as long as the Microsoft Windows operating system is aware of the files associated editor. Add it to the project as described in section 1.4.3 (you will need to change the file filter to see non-Altium file types). The file will appear in the Project structure in the Projects panel, under a folder icon titled Documentation. 1 - 12

Libraries

Libraries can exist as individual documents, for example, schematic libraries containing schematic symbols, PCB libraries containing PCB footprint models, discrete SPICE models (MDL and CKT), and so on. Altium Designer also supports the creation of integrated libraries. An integrated library is the compiled output from a library package. It includes all the schematic libraries in the original library package, plus any referenced models, including footprint, simulation and signal integrity models. Most of the supplied libraries are provided as integrated libraries and are stored within the \Program Files\Altium Designer Summer 09\Library folder. Integrated libraries can be converted back to their constituent libraries; simply open them in Altium Designer to do this. PCB libraries are also provided in the \Program Files\Altium Designer Summer 09\Library\Pcb folder. The Schematic Library Editor and PCB Library Editor are covered during the Schematic Capture and PCB Design training sessions. The basics of creating an integrated library are also covered. Note: You can use Protel 99 SE libraries directly in Altium Designer. Add them to the Libraries panel to use them without converting them to the Altium Designer format. Note that you will not get all the benefits of the enhanced parameter and model support.

Project Packager

An Altium Designer project can include many and varied files - source files, libraries, reports, data sheets, manufacturing files, etc. The Project Packager Wizard simplifies the task of managing and transferring the complete fileset. Guided by the settings you define the Project Packager Wizard gathers and packages the project into a portable time and date stamped ZIP file. The Project Packager supports: Any situation where your project must be moved, for example is moving it from one site to another, or backing up your project for secure storage. Packaging a complete Altium Designer project tree - ideal for linked PCB + FPGA + Embedded projects. Packaging a complete Altium Designer Workspace - ideal for designers that include all the board designs destined for a company product, in a single Workspace. Managing how directory paths are handled during packaging. Managing how files outside the project folder are handled during packaging. Including/excluding Generated files, such as reports, in the project package. Including/excluding History files (created by Altium Designer's built-in file history/restore system).

1 - 13

Figure 14. Project packager project choice page

1.4.10

Exercise Working with projects and documents
This exercise looks at creating a new project and adding documents to it. 1. Create a new PCB project in the \Altium Designer Summer 09\Examples\Training\PCB Training\Temperature Sensor folder and name it Temperature Sensor.PrjPCB. We will use this project later during the Schematic Capture training session. 2. Add the following two schematic documents to the project from the \Altium Designer Summer 09\Examples\Training\PCB Training\Temperature Sensor folder: LCD.SchDoc and Power.SchDoc. Use Add Existing to Project command from the right click menu in the Projects panel. 3. Save and close the new project Temperature Sensor.PrjPCB. 4. Check that the documents exist on the hard drive using the Windows Explorer

1 - 14