From Idea to Manufacture - Driving a PCB Design through CircuitStudio

Welcome to the world of electronic product development in Altium's world-class electronic design software. This tutorial will help you get started by taking you through the entire process of designing a simple PCB - from idea to outputs files. If you are new to Altium software, it is worth reading the article Exploring CircuitStudio to learn more about the interface, information on how to use panels, and an overview of managing design documents.

The Design

The design you will be capturing and designing a printed circuit board (PCB) for is a simple astable multivibrator. The circuit is shown below; it uses two general purpose NPN transistors configured as a self-running astable multivibrator.

You're ready to begin capturing (drawing) the schematic. The first step is to create a PCB project.

Creating a New PCB Project

In Altium's software, a PCB project is the set of design documents (files) required to specify and manufacture a printed circuit board. The project file, for example, Multivibrator.PrjPCB, is an ASCII text file that lists the documents that are in the project as well as other project-level settings, such as the required electrical rule checks, project preferences, and project outputs, such as print and CAM settings.

A new project is created in the Create New Project From Template dialog.

Creating a new project:

1. Select File » New PCB Project from the menus, the Create New Project from Template dialog will open.
2. Available templates are listed down the left, choose Blank PCB Project.
3. In the Name field, enter Multivibrator. There is no need to add the file extension, this will be added automatically.
4. In the Location field, type in a suitable location to save the project files, or click Browse to navigate to the required folder.
5. Enable the Create Project Subfolder option, this will create a sub-folder below the folder specified in the Location field, with the same name as the project.
6. Click OK to close the dialog and create the project file in the specified location.
7. The new project will appear in the Projects panel. If this panel is not displayed, enable it via the View | System | Projects button.

Adding a Schematic to the Project

The next step is to add a new schematic sheet to the project.

Adding a schematic:

1. On the ribbon, click the Home | Project | Project » Add New Schematic menu entry. A blank schematic sheet named Sheet1.SchDoc will open in the design window and an icon for this schematic will appear linked to the project in the Projects panel under the Source Documents folder icon.
2. To save the new schematic sheet, select File » Save As. The Save As dialog will open, ready to save the schematic in the same location as the project file. Type the name Multivibrator in the File Name field then click Save. Note that files stored in the same folder as the project file itself (or in a child/grandchild folder) are linked to the project using relative referencing, and files stored in a different location are linked using absolute referencing.
3. Since you have added a schematic to the project, the project file also has changed. Right-click on the project filename in the Projects panel then select Save Project to save the project.

Setting the Document Options

Before you start drawing your circuit, it is worth setting up the appropriate document options, including the sheet size and the Snap and Visible grids.

Configuring the Document Options:

1. On the ribbon, click Project | Content | Document Options to open the Document Options dialog.
2. For this tutorial, the only change that needs to be made is to set the sheet size to A4 in the Standard Styles field of the Sheet Options tab of the dialog.
3. Confirm that both the Snap and Visible Grids are set to 10.
4. Click OK to close the dialog and update the sheet size.
5. To make the document fill the viewing area, click View | Zoom Document.
6. Save the schematic by selecting File » Save (shortcut: Ctrl+S).

Components and Libraries in CircuitStudio

Related article: Component Management in CircuitStudio

The real-world component that gets mounted on the board is represented as a schematic symbol during design capture, and as a PCB footprint for board design. CircuitStudio components can be stored in local libraries or they can be placed directly from the Altium Content Vault, which is a globally-accessible component storage system that contains thousands of components, each with a symbol, footprint, component parameters, and links to suppliers.

The following component storage options can be used in CircuitStudio:

Library Type	Function
Schematic Library	Schematic component symbols are created in schematic libraries (*.SchLib). Each symbol can become a component by adding links to a PCB footprint and adding component parameters to detail the component's specifications.
PCB Library	PCB footprints (models) are stored in PCB libraries (*.PcbLib). The footprint includes the electrical elements, such as the pads, as well as the mechanical elements, such as the component overlay, dimensions, glue dots, etc. It also can include a 3D definition, which is created by placing 3D Body objects or by importing a STEP model.
Library Package / Integrated Library	As well as working directly from the schematic and PCB libraries, you can also compile the component elements into an integrated library (*.IntLib). Doing this results in a single, portable library that holds all the models and symbols. An integrated library is compiled from a Library package (*.LibPkg), which is essentially a special-purpose project file with the source schematic (*.SchLib) and PCB libraries (*.PcbLib) added to it as source documents. As part of the compilation process, you can also check for potential problems, such as missing models and mismatches between schematic pins and PCB pads.
Altium Content Vault	The Content Vault is much more than a library. Components stored in the cloud, accessible from anywhere with internet access. Content Vault components include: symbol, footprint(s), component parameters, and links to suppliers. They are organized into folders - by manufacturer or by package type for generics.

Accessing Components

Components are accessed through either:

• the Libraries panel (View | System | Libraries) for library components, or
• the Vaults panel (File » Vault Explorer) for Content Vault components.

Access components through either the Libraries pane, or the Vaults panel.

Making Libraries Available to Access the Components

In CircuitStudio, library-based components can be placed from Available Libraries. The libraries that are available include:

• Libraries in the current project - if a library is part of the project, the components in it are automatically available for placement within that project.
• Installed libraries - these are libraries that have been installed in CircuitStudio and their components are available for use in any open project.

Libraries are installed on the Installed tab of the Available Libraries dialog. To open the dialog, click the Libraries button at the top of the Libraries panel. If the panel is not currently visible, click View | System | Libraries to display it.

Install the required libraries to make their components available for designs.

Finding a Component in Libraries

To help you find the component you need, CircuitStudio includes powerful library searching capabilities. Although there are components that are suitable for the multivibrator design available in the pre-installed libraries, it is useful to know how to use the search feature to find components.

The Libraries Search dialog is accessed by clicking the Search button on the Libraries panel. The upper half of the dialog is used to define what you are searching for, the lower half is used to define where to search. The search can be in the libraries that are already installed (Available libraries) or it can be in libraries located on the hard drive (Libraries on path).

If you were working from libraries, the first step would be to search for a suitable general-purpose NPN transistor, such as a 2N3904.

Searching through libraries:

1. If it is not visible, display the Libraries panel (View | System | Libraries).
2. Press the Search button in the Libraries panel to open the Libraries Search dialog, as shown above.
3. Ensure that the dialog options are set as follows:
   • For the first Filter row, the Field is set to Name, the Operator is set to contains, and the Value is 3904.
   • The Scope is set to Search in Components and Libraries on path.
   • The Path is set to point to the installed Altium libraries, which will be similar to C:\Users\Public\Documents\Altium\CS\Library.
4. Click the Search button to begin the search. The Query Results are displayed in the Libraries panel. There should be one component found, as shown in the image below. It may be listed multiple times, depending on how many models it has linked to it.
5. You can only place components from Libraries that are installed in the software. If you attempt to place from a library that is not currently installed, you will be asked to Confirm the installation of that library when you attempt to place the component.

Library searching is actually performed using queries. In the Libraries Search dialog, switch to the Advanced mode to examine the query. The query generated by your search configuration should be (Name LIKE '*3904*'). If it is not, type this string then click Search again.

Locating a Component in an Available Library

Libraries that are already installed are listed in the drop-down at the top of the panel. Click to select a library and display the components stored in it. Select the Miscellaneous Devices. IntLib library from the list, then use the component Filter in the panel to locate the required 2N3904 component within the library. Since the Miscellaneous Devices library is already installed, this component is ready to place. Do not place it though; instead you will use a transistor from the Altium Content Vault.

Making the Content Vault Available to Access Components

The Altium Content Vault is completely separate from the installed CircuitStudio software. To access the components in the Content Vault, you must first connect to it. This is done by clicking the Add Altium Content Vault button in the Data Management - Vaults page of the Preferences dialog.

Finding a Component in the Content Vault

Related article: Vaults panel

Once you have connected to the Altium Content Vault, you can explore or search for a component. This is done in the Vaults panel by selecting File » Vault Explorer to display the panel. The panel includes a powerful search feature. Enter the search string into the search field at the top-right of the panel.

Searching for the general-purpose transistor BC547 in the Altium Content Vault. Each result is a hyperlink. Hover for more information and click to examine.

Working in the Vaults Panel

The Vaults panel includes a number of sections that can be resized as required. Take some time to explore the features and behavior of the panel; right-click for context-specific commands.

Use the Preview mode to examine the models and parameters included with the selected component.

• Components are organized in folders. Use the Vaults Folders section on the left of the panel to browse.
• There are a large number of components stored in the Altium Content Vault, therefore, it can be more efficient to search as just described.
• Search results are presented as a series of links; click on a link to examine a component in detail; use the Back button at the top right of the panel to return to the search results.
• Clicking on a specific component in the search results displays only that component in the folder in which it is stored. Select Refresh All from the menu at the top left of the panel to display all components in that folder.
• The lower region of the panel has a number of display modes, including: Summary, Supply Chain, Lifecycle, Where-used, and Preview. Use the arrow icon to select the required mode, as shown in the image above.

Placing Components on the Schematic

Components are placed onto the current schematic sheet from the Libraries or Vaults panel. This can be done by:

From the Libraries Panel

• Clicking the Place button - the component appears floating on the cursor; position it then click to place.
• Double-clicking - double-click the component in the list of components in the panel. The component appears floating on the cursor; position it then click to place.
• Click and drag - click and drag the component onto the sheet. This mode requires that the mouse button is held down; the component is placed when the mouse button is released.

From the Vaults Panel

• Right-click on the component then select Place <component>. The component appears floating on the cursor; position it then click to place. Note that if the Vaults panel is floating over the workspace, it will fade to allow you to see the schematic and place the component.
• Click and drag - click and drag the component from the Vaults panel and drop it onto the schematic. This mode requires that the mouse button is held down; the component is placed when the mouse button is released.

Multivibrator Parts

The following components were searched for and used in the Multivibrator circuit.

Designator	Description	Vault Item-Revision or Library Component Name	Comments
Q1, Q2	General purpose NPN transistor, e.g., BC547 or 2N3904	CMP-1048-01437-1	searched Vault for BC547, chose the first one
R1, R2	100K resistor, 5%, 0805	CMP-1013-00122-1	searched Vault for 100K 5% 0805
R3, R4	1K resistor, 5%, 0805	CMP-1013-00074-1	searched Vault for 1K 5% 0805, note that search also returns 1K3, 1K8, etc.
C1, C2	22nF capacitor, 10%, 16V, 0805	CMP-1036-04042-1	searched Vault for 22nF 16V 0805
Y1	2-pin header, thruhole	Header 2	searched Available Libraries for header, component found in Miscellaneous Connectors.IntLib

Once you have placed the components, the schematic should look similar to this:

All components are placed, ready for wiring.

Finding and Placing the Transistors:

1. Select View | Zoom | Zoom Document (shortcut: V, A) to ensure your schematic sheet takes up the full window.
2. Using the search techniques just described, locate the transistor BC547 in the Vaults panel.
3. When you search the Vault, it will first cluster the results to show the folders that contain possible components. For the transistor search, all results are in the same folder titled General Purpose Transistors. Click the hyperlink to open the search results for that folder then click the CMP-1048-01437-1 Item.
4. That component will be presented in the Vaults panel, where you can display the Preview at the bottom and examine the symbol, footprint and component parameters (you might need to resize the lower section to display all of the Preview content).

5. Right-click on the transistor's Item-Revision number to display the context menu (as shown above), then select Place CMP-1048-01437-1 from the menu. The cursor will change to a cross hair and you will have an image of the transistor floating on your cursor. You are now in part placement mode. If you move the cursor around, the transistor will move with it.

Do not place the transistor yet!

6. Before placing the part on the schematic you can edit its properties, which can be done for any object floating on the cursor. While the transistor is still floating on the cursor, press the Tab key to open the Component Properties dialog. Set up the dialog to appear as shown below.

7. In the Properties section of the dialog, type in the Designator Q1.
8. Enable the Visible checkbox for the Comment field.
9. Leave all other fields at their default values then click OK to close the dialog.
10. Move the cursor, with the transistor symbol attached, to position the transistor a little to the left of the middle of the sheet. Note the current snap grid that is displayed on the left of the Status bar near the bottom of the application. It defaults to 10; press the G shortcut to cycle through the available grid settings during object placement. It is strongly advised to keep the snap grid at 10 or 5 to keep the circuit neat and make it easy to attach wires to pins. For a simple design such as this, 10 is a good choice.
11. Once you are happy with the transistor's position, left mouse click or press Enter on the keyboard to place the transistor onto the schematic.
12. Move the cursor and you will find that a copy of the transistor has been placed on the schematic sheet, but you are still in part placement mode with the part outline floating on the cursor. This feature allows you to place multiple parts of the same type. Now on to placing the second transistor. This transistor is the same as the previous one, so there is no need to edit its attributes before it is placed. The software will automatically increment the component designator when you place multiple instances of the same part. In this case, the next transistor will automatically be designated Q2.
13. If you refer to the rough schematic diagram shown before, you will notice that Q2 is drawn as a mirror of Q1. To flip the orientation of the transistor that is floating on the cursor, press the X key on the keyboard. This flips the component horizontally (along the X axis).
14. Move the cursor to position the part to the right of Q1. To position the component more accurately, press the PgUp key twice to zoom in two steps. You should now be able to see the grid lines.
15. Once you have positioned the part, left mouse click or press Enter to place Q2. Once again, a copy of the transistor you are "holding" will be placed on the schematic and the next transistor will be floating on the cursor ready to be placed.
16. Since all the transistors have been placed, exit part placement mode by clicking the right mouse button or pressing the Esc key. The cursor will revert back to a standard arrow.

Finding and Placing the Resistors:

1. Using the search techniques just described, search for a suitable 100K 5% 0805 resistor in the Vaults panel. The search should return the Item CMP-1013-00122-1.
2. Right-click on the resistor's Item number to display the context menu, then select Place CMP-1013-00122-1 from the menu.
3. While the resistor is still floating on the cursor, press the Tab key to open the Component Properties dialog.
4. In the Properties section of the dialog, type in the Designator R1.
5. Enable the Visible checkbox for the Comment field.
6. Ensure that the footprint Model is set to RESC0805(2012)_N. Using the drop-down next to the model name, you will see that there are three footprint models attached to this component, IPC Low Density (_M), IPC Medium Density (_N) and IPC High Density (_L). The footprint selected will be transferred to the PCB during design synchronization.
7. Leave all other fields at their default values then click OK to close the dialog; the resistor will be floating on the cursor.
8. Press the Spacebar to rotate the component in 90° increments until it has the correct orientation.
9. Position the resistor above and to the left of the base of Q1 (refer to the schematic diagram shown earlier) then click the left mouse button or press Enter to place the part.
10. Next place the other 100k resistor, R2, above and to the right of the base of Q2. The designator will automatically increment when you place the second resistor.
11. Exit part placement mode by clicking the right mouse button or pressing the ESC key. The cursor will revert back to a standard arrow.
12. The remaining two resistors, R3 and R4, have a value of 1K; search for a suitable 1K 5% 0805 resistor in the Vaults panel.
13. This search will return all resistors whose values start with 1K, including 1K1, 1K2, 1K3, etc. Using the Description field, click in the search results to open the 1K 5% 0805 resistor, then right-click and Place it. 
14. Using the steps just given, set the Designator to R3, enable the visibility of the Comment, and set the footprint Model to RESC0805(2012)_N.
15. Position and place R3 directly above the Collector of Q1, then place R4 directly above the Collector or Q2 as shown in the image above.
16. Right-click or press ESC to exit part placement mode.

Finding and Placing the Capacitors:

1. Return to the Vaults panel and search for a suitable 22nF 16V 0805 capacitor. The search will return a number of potential capacitors. Click on Item CMP-1036-04042-1 to use in this design.
2. Right-click on the capacitor's Item number then select Place CMP-1036-04042-1 from the menu.
3. While the resistor is still floating on the cursor, press the Tab key to open the Component Properties dialog.
4. In the Properties section of the dialog, type in the Designator C1.
5. Enable the Visible checkbox for the Comment field.
6. Ensure that the footprint Model is set to CAPC0805(2012)145_N.
7. Leave all other fields at their default values then click OK to close the dialog. The capacitor will be floating on the cursor.
8. Press the Spacebar to rotate the component in 90° increments until it has the correct orientation.
9. Position the capacitor above the transistors but below the resistors (refer to the schematic diagram shown earlier) then click the left mouse button or press Enter to place the part.
10. Position and place capacitor C2.
11. Right-click or press Esc to exit placement mode.

Finding and Placing the Connector:

1. The last component to be placed is the connector, which is located in Miscellaneous Connectors.IntLib. This integrated library is normally already installed. If it is not, install it then select it at the top of the Libraries panel.
2. The connector is a two-pin header; type header into the Libraries panel filter field. Note that the wildcard * is not used for this search since you are only searching for components that start with the string header. If the wildcard is included at the start of the search string, all components that have the string header anywhere in their name or description will be returned.
3. Select Header 2 from the list then click the Place button.
4. While it is floating on the cursor, press Tab to edit the attributes; set the Designator to Y1 and check that the PCB footprint model is HDR1X2.
5. Before placing the connector, press X to flip it horizontally so that it is in the correct orientation. Click to place the connector on the schematic as shown in the image above.
6. Right-click or press Esc to exit part placement mode.
7. Save your schematic (Ctrl+S).

You have now placed all the components. Note that the components shown in the image above are spaced so that there is plenty of room to wire to each component pin. This is important because you cannot place a wire across the bottom of a pin to get to a pin beyond it. If you do, both pins will connect to the wire. If you need to move a component, click-and-hold the body of the component then drag the mouse to reposition it.

Wiring the Circuit

Wiring is the process of creating connectivity between the various components of your circuit. To wire your schematic, refer to the sketch of the circuit and the animation shown below.

Use the Wiring tool to wire up your circuit.

Wiring the schematic:

1. To make sure you have a good view of the schematic sheet, press the PgUp key to zoom in or PgDn to zoom out. Alternatively, hold down the Ctrl key and roll the mouse wheel to zoom in/out or hold Ctrl + Right Mouse button down and drag the mouse up/down to zoom in/out. There are also a number of useful View commands in the right-click View submenu, such as Fit All Objects (Ctrl+PgDn).
2. First, wire the lower pin of resistor R1 to the base of transistor Q1 in the following manner. Click the button (Home | Circuit Elements | Wire) to enter the wire placement mode. The cursor will change to a cross hair.
3. Position the cursor over the bottom end of R1. When you are in the right position, a red connection marker (large cross) will appear at the cursor location. This indicates that the cursor is over a valid electrical connection point on the component.
4. Click the Left Mouse Button or press Enter to anchor the first wire point. Move the cursor and you will see a wire extend from the cursor position back to the anchor point.
5. Position the cursor over the base of Q1 until you see the cursor change to a red connection marker. Click or press Enter to connect the wire to the base of Q1. The cursor will release from that wire.
6. Note that the cursor remains a cross hair, indicating that you are ready to place another wire. To exit placement mode completely and go back to the arrow cursor, you would Right-Click or press Esc again - but don't do this just now.
7. Next, wire from the lower pin of R3 to the collector of Q1. Position the cursor over the lower pin of R3 then click or press Enter to start a new wire. Move the cursor vertically till it is over the collector of Q1 then click or press Enter to place the wire segment. Again, the cursor will release from that wire and you remain in wiring mode, ready to place another wire.
8. Wire up the rest of your circuit as shown in the animation above.
9. When you have finished placing all the wires, right-click or press Esc to exit placement mode. The cursor will revert to an arrow.

Nets and Net Labels

Each set of component pins that you have connected to each other now form what is referred to as a net. For example, one net includes the base of Q1, one pin of R1 and one pin of C1. Each net is automatically assigned a system-generated name, which is based on one of the component pins in that net.

To make it easy to identify important nets in the design, you can add Net Labels to assign names. For the multivibrator circuit, you will label the 12V and GND nets in the circuit.

Net Labels have been added to complete the schematic.

Adding net labels:

1. Click the  button (Home | Circuit Elements | Net Label). A net label will appear floating on the cursor.
2. To edit the net label before it is placed, press Tab key to open the Net Label dialog.
3. Type 12V in the Net field then click OK to close the dialog.
4. Place the net label so that the bottom left corner of the net label touches the upper most wire on the schematic as shown in the image below. The cursor will change to a red cross when the net label is correctly positioned to connect to the wire. If the cross is light gray, it means there will not be a valid connection made.

 
The net label in free space (left image) and positioned over a wire (right image), note the red cross.

5. After placing the first net label, you will still be in net label placement mode. Press the Tab key again to edit the second net label before placing it.
6. Type GND in the Net field then click OK to close the dialog.
7. Place the net label so that the bottom left of the net label touches the lower most wire on the schematic as shown in the image below. Right-click or press Esc to exit net label placement mode.
8. Save your schematic and the project as well.

Setting Up Project Options

Project-specific settings are configured in the Options for PCB Project dialog, shown below (Home | Project » Options or Project | Content | Project Options). The project options include the error checking parameters, a connectivity matrix, Class Generator, the Comparator setup, ECO generation, output paths and netlist options, Multi-Channel naming formats, Default Print setups, Search Paths, and project-level Parameters. These settings are used when you compile the project.

Project outputs, such as assembly, fabrication outputs and reports, are set up from the Outputs tab of the Ribbon. These settings are also stored in the Project file so they are always available for this project. See Documentation Outputs for more information.

Checking the Electrical Properties of the Schematic

Schematic diagrams are more than just simple drawings - they contain electrical connectivity information about the circuit. You can use this connectivity awareness to verify your design. When you compile a project, the software checks for errors according to the rules set up in the Error Reporting and Connection Matrix tabs of the Options for Project dialog. When you compile the project, any violations that are detected will display in the Messages panel.

Setting up the Error Reporting

The Error Reporting tab in the Options for Project dialog is used to set up design drafting checks. The Report Mode settings show the level of severity of a violation. If you want to change a setting, click on a Report Mode next to the violation you want to change and choose the level of severity from the drop-down list. For this tutorial, we will use the default settings in this tab.

Setting Up the Connection Matrix

When the design is compiled, a list of the pins in each net is built in memory. The type of each pin is detected (e.g., input, output, passive, etc.,) then each net is checked to see if there are pin types that should not be connected to each other, for example, an output pin connected to another output pin. The Connection Matrix tab of the Options for Project dialog is where you configure which pin types are allowed to connect to each other. For example, look down the entries on the right side of the matrix diagram and find Output Pin. Read across this row of the matrix until you find the Open Collector Pin column. The square where they intersect is orange, indicating that an Output Pin connected to an Open Collector Pin on your schematic will generate an error condition when the project is compiled.

You can set each error type with a separate error level, e.g., from no report to a fatal error. Click on a colored square to change the setting; continue to click to move to the next check-level. Set the matrix so that Unconnected Passive Pin generates an Error, as shown in the image below.

The Connection Matrix defines what electrical conditions are checked for on the schematic, note that the Unconnected - Passive Pin setting is being changed.

Changing the Connection Matrix:

1. To change one of the settings, click the colored box; it will cycle through the four possible settings. Note that you can right-click in the matrix area to display a menu that lets you toggle all settings simultaneously, including an option to restore all to their Default state (handy if you have been toggling settings and cannot remember their default state).
2. Your circuit contains only Passive Pins (on resistors, capacitors and the connector) and Input Pins (on the transistors). Let's change this so that the connection matrix detects unconnected passive pins. Find the Passive Pin row on the right. Look across the column labels to find Unconnected. The square where these entries intersect indicates the error condition when a passive pin is found to be unconnected in the schematic. The default setting is green, indicating that no report will be generated.
3. Click on this intersection box until it turns Orange (as shown in the image above) so that an error will be generated for unconnected passive pins when the project is compiled. You will purposely create an instance of this error to check this later in the tutorial.

Setting Up the Comparator

The Comparator tab in the Options for Project dialog sets which differences between files will be reported or ignored when a project is compiled. Generally, the only time you will need to change settings in this tab is when you add extra detail to the PCB, such as design rules, and do not want those settings removed during design synchronization. If you need more detailed control, you can selectively control the comparator using the individual comparison settings.

For this tutorial, it is sufficient to confirm that the Ignore Rules Defined in PCB Only option is enabled.

Compiling the Project to Check for Errors

Compiling a project checks for drafting and electrical rules errors in the design documents and details all warnings and errors in the Messages panel. You have set up the rules in the Error Checking and Connection Matrix tabs of the Options for Project dialog and you are now ready to check the design.

To compile the project and check for errors, select Home | Project » Compile.

Use the Messages panel to locate and resolve design errors; double-click on an error to pan and zoom to that object.

Compiling and checking for errors:

1. To compile the Multivibrator project, select Home | Project | Project » Compile.
2. When the project is compiled, all warnings and errors are displayed in the Messages panel. The panel will only appear automatically if there are errors detected (not when there are only warnings). To open it manually, click View | System | Messages.
3. If your circuit is drawn correctly, the Messages panel should not contain any errors, only the message Compile successful, no errors found. If there are errors, work through each one, checking your circuit and ensuring that all wiring and connections are correct.

4. You will now deliberately introduce an error into the circuit and recompile the project:

5. Click on the Multivibrator.SchDoc tab at the top of the design window to make the schematic sheet the active document.
6. Click in the middle of the wire that connects R1 to the base wire of Q1. Small, square editing handles will appear at each end of the wire and the selection color will display as a dotted line along the wire to indicate that it is selected. Press the Delete key on the keyboard to delete the wire.
7. Recompile the project (Home | Project | Project » Compile) to check for errors. The Messages panel will display warning messages indicating you have unconnected pins in your circuit.
8. The Messages panel is divided horizontally into two regions, as shown in the image above. The upper region lists all messages, which can be saved, copied, cross probed to, or cleared via the right-click menu. The lower region details the warning/error currently selected in the upper region of the panel.
9. When you double-click on an error or warning in either region of the Messages panel, the schematic view will pan and zoom to the object with the error.

10. Before you finish this section of the tutorial, let's fix the error in our schematic.

11. Make the schematic sheet the active document.
12. Undo the delete action (Ctrl+Z) to restore the deleted wire.
13. To check that there are no longer any errors, recompile the project (Home | Project | Project » Compile).The Messages panel should show no errors.
14. Save the schematic and the project file as well.

Creating a New PCB

Before you transfer the design from the Schematic Editor to the PCB Editor, you need to create the blank PCB, name it and save it as part of the project.

The blank PCB has been added to the project.

Adding a New Board to the Project:

1. A new PCB can be added to the project using the Home | Project | Project » Add new PCB command.

2. The PCB will appear as a Source Document in the Project as shown below. Right-click on the PCB icon in the Projects panel to select the Save As command and name it Multivibrator.CSPcbDoc. Note that you do not need to enter the file extension in the Save As dialog; this is automatically appended.

3. Adding the PCB has changed the project. Save the project (right-click on the project filename in the Projects panel then select Save Project).

Configuring the Board Shape and Location

There are a number of attributes of this blank board that need to be changed before transferring the design from the schematic editor including:

Task	Process
Setting the origin	The PCB editor has two origins, the Absolute Origin, which is the lower left of the workspace, and the user-definable Relative Origin, which is used to determine the current workspace location. A common approach is to set the Relative Origin to the lower-left corner of the board shape. The Origin is set in the Grids and Units section of the Home tab on the Ribbon.
Change from Imperial to Metric units	The current workspace units are displayed on the Status bar, which is displayed at the bottom left of the workspace and also in the Grids and Units section of the Home tab on the Ribbon. For this tutorial, metric units will be used; to change the units, either press Q on the keyboard to toggle back and forth between Imperial and Metric units or click the  button on the Ribbon.
Selecting a suitable snap grid	You may have noticed that the current snap grid is 0.127mm, which is the old 10mil imperial snap grid, converted to metric. To change the snap grid at any time, select or type a new value in the Snap Grid setting in the Home | Grids and Units section of the Ribbon. Since you are about to define the overall size of the board, a very coarse grid can be used; enter a value of . Grids are also discussed in more detail later in the tutorial.
Redefining the board shape to the required size	The board shape is shown by the black region with a grid in it. The default size for a new board is 4x4 inches; the tutorial board is 30mm x 30mm. Details for the process of defining a new shape for the board are outlined below.
Configuring the layers used in the design	As well as the copper, or electrical layers, on which you route, there are also general purpose mechanical layers, and special-purpose layers such as the component overlays (silkscreens), solder mask, paste mask, etc. The electrical and other layers will be configured shortly.

Setting the Origin and the Grid:

1. There are two origins used in the software: the Absolute Origin, which is the lower left of the workspace, and the user-definable Relative Origin, which is used to determine the current workspace location. Before setting the origin, keep zooming in to the lower left of the current board shape until you can easily see the grid. To do this, position the cursor over the lower-left corner of the board shape then press PgUp until both the Coarse and Fine grids are visible as shown in the images below.
2. To set the Relative Origin, select Home | Grids and Units | Origin » Set, position the cursor over the bottom left corner of the board shape then left click to set it.

Select the command, position the cursor over the lower-left corner of the board shape (left image), then click to define the origin (right image).

3. The next step is to select a suitable snap grid, which is summarized in the table above. The grid is set in the Grids and Units section of the Home tab of the Ribbon. During the course of design, it is quite common to change grids. For example, you might use a coarse grid during component placement, and a finer grid for routing. Grids can be changed by selecting a new value from the Snap Grid drop-down list or typing the required value directly in the Snap Grid field then pressing Enter to have your value accepted.
4. For this tutorial, you will be using a Metric grid; click the button to switch to Metric.
5. The first grid you will be using is 5mm; enter this value into the Snap Grid field.

Redefining the Board Shape:

1. The default board shape is 4x4 inch. For this tutorial, the board size is 30mm x 30mm. 
2. To zoom back out and show the all of the workspace currently being used, click View | Zoom | Zoom All (Ctrl+PgDn). Your design should look much like the left image below.
3. The next step is to change the board shape to 30mm x 30mm. Your choice now is to either redefine the board shape (draw it again, or edit the existing board shape. For a simple square or rectangle, it is more efficient to edit the existing board shape. To do this, select Home | Board | Board Shape » Edit Board Shape.

4. The board display will change, with the shape shown in green. Editing handles will appear at each corner and the center of each edge, as shown below.

Note that clicking anywhere other than on an editing handle or an edge of the shape will drop you out of board shape editing mode.

5. The objective is to resize the shape to create a 30mm by 30mm board. The Coarse visible grid is 25mm (5x the snap grid), and the Fine visible grid is 5mm - this will be used as a guide. You can now either slide the upper and right edges down and in to create the correct size or move three of the corners in, leaving the one that is at the origin in its current location.
6. To slide the top edge down, position the cursor over the edge (but not over a handle), then when the cursor changes to a double-headed arrow, click and hold, then drag the edge to the new location so that the Y cursor location is 30mm on the Status bar.
7. Repeat the process to move the right-hand edge in, positioning it when the X cursor location is 30mm on the Status bar.

Use the current grid location information on the bottom left of the Status bar to guide you as you reshape the board.

The board shape has been resized to 30mm x 30mm as indicated by the current grid locations shown on the Status bar.

8. Click anywhere in the workspace to drop out of board shape editing mode.
9. Save the board.

Transferring the Design

The process of transferring a design from the capture stage to the board layout stage is launched using the Update command (Home | Project | Project » Update PCB Document Multivibrator.CSPcbDoc) on the schematic editor Ribbon (or Home | Project | Project » Import Changes from Multivibrator.PrjPcb from the PCB editor Ribbon).

When you run this command, the design is compiled and a set of Engineering Change Orders is created that:

• Lists all components used in the design and the footprint required for each. When the ECOs are executed, the software will attempt to locate each footprint in the currently available libraries or available Content Vault, and place each into the PCB workspace. If the footprint is not available, an error will occur.
• A list of all nets (connected component pins) in the design is created. When the ECOs are executed, the software will add each net to the PCB then attempt to add the pins that belong to each net. If a pin cannot be added, an error will occur - this most often happens when the footprint was not found or the pads on the footprint do not map to the pins on the symbol.
• Addition design data is then transferred, such as net and component classes.

Transferring the design from schematic capture to PCB layout:

1. Ensure Multivibrator.SchDoc is the active document.

2. Select Home | Project | Project » Update PCB Document Multivibrator.CSPcbDoc from the Ribbon. The project will compile and the Engineering Change Order dialog will open.

An ECO is created for each change that needs to be made to the PCB so that it matches the schematic.

3. Click on Validate Changes. If all changes are validated, a green check will appear next to each change in the Status list. If the changes are not validated, close the dialog, check the Messages panel and resolve any errors.
4. Click on Execute Changes to send the changes to the PCB editor.
5. When completed, the target PCB opens with the Engineering Change Order dialog open on top of it, and the Done column entries become checked as shown in the image below.
6. Click to Close the dialog and complete the transfer process.

7. The components will have been positioned outside of the board, ready for placing on the board. There are a few steps before starting the component process, such as configuring the placement grid, the layers and the design rules.

You can create a report of the ECOs by clicking the Report Changes button in the Engineering Change Order dialog.

Setting Up the PCB Workspace

Once all of the ECOs have been executed, the components and nets will appear in the PCB workspace to the right of the board outline.

Before we start positioning the components on the board, we need to configure certain PCB workspace and board settings, such as the layers, grids and design rules.

Configuring the Display of Layers

As well as the the layers used to fabricate the board including: signal, power plane, mask and silkscreen layers, the PCB Editor also supports numerous other non-electrical layers. The layers are often grouped in the following way:

• Electrical layers - includes the 32 signal layers and 16 internal power plane layers.
• Mechanical layers - there are 32 general purpose mechanical layers, which are used for design tasks such as dimensions, fabrication details, assembly instructions, or special purpose tasks, such as glue dot layers. These layers can be selectively included in print and Gerber output generation. They can also be paired, meaning that objects placed on one of the paired layers in the library editor will flip to the other layer in the pair when the component is flipped to the bottom side of the board.
• Special layers - these include the top and bottom silkscreen layers, the solder and paste mask layers, drill layers, the Keep-Out layer (used to define the electrical boundaries), the multilayer (used for multilayer pads and vias), the connection layer, DRC error layer, grid layers, hole layers, and other display-type layers.

The display attributes of all layers are configured in the View Configurations dialog. To open the dialog:

• Select View | View | Switch to 3D » View Configurations » View Configuration or
• Click the current layer icon at the bottom-left of the workspace.

As well as the layer display state and color settings, the View Configurations dialog also gives access to other display settings including:

• How each type of object is displayed (solid, draft or hidden)oin the Show/Hide tab of the dialog.
• Various view options, such as if Pad Net names and Pad Numbers are to be displayed, the Origin Marker, if Special Strings should be converted, etc. These are configured on the View Options tab of the dialog.

Configuring the Layer Visibility:

1. Open the View Configurations dialog (View | View | Switch to 3D » View Configurations » View Configuration).
2. On the Board Layers And Colors tab, confirm that the two signal layers are visible.
3. Note that this dialog is where you control the display of the mask layers, the silkscreen layers and the system layers, such as DRC and grids.
4. To have less visual "clutter" during placement and routing, disable the display of the Mechanical Layers, all of the Mask Layers, and the Drill Guide and Drill Drawing layers.
5. Switch to the View Options tab.
6. Confirm that the Show Pad Nets option is enabled, and the Net Names on Tracks Display is set to Single and Centered.
7. Click OK to accept the settings and close the dialog.

Physical Layers and the Layer Stack Manager

As well as the signal and power plane (solid copper) layers, the PCB Editor includes soldermask and silkscreen physical layers - these are all fabricated to make the physical board. The arrangement of these layers is referred to as the Layer Stack. The layer stack is configured in the Layer Stack Manager. Click Home | Board | Layer Stack Manager to open the dialog.

The Layer Stack Manager dialog is used to:

• Add/remove signal and power plane layers.
• Add/remove dielectric layers.
• Change the order of the layers.
• Configure the Material type for non-copper layers.
• Set the layer Thickness, Dielectric Material and Dielectric Constant.
• Define the Pullback amount (clearance from plane edge to board edge) for plane layers.
• Define the component orientation for that layer (advanced feature available in certain Altium products).

The tutorial PCB is a simple design and can be routed as a single-sided or double-sided board. The layer thicknesses shown below have been edited to use sensible metric values.

Configuring the board layer stack:

1. Open the Layer Stack Manager. For a new board, the default stack comprises: a dielectric core, two copper layers, as well as the top and bottom soldermask (coverlay) and overlay (silkscreen) layers as shown in the image above.
2. New layers and planes are added below the currently selected layer, which is done using the Add Layer button or the right-click menu.
3. Layer properties, such as material, copper thickness and dielectric properties, are included when a Layer Stack Table is placed and are also used for signal integrity analysis. Double-click in a cell to configure that setting. For example, the Thickness settings shown in the image below have been changed slightly to more suitable metric values.
4. When you have finished exploring the layer stack options, restore the values to those shown in the image below then click OK to close the dialog.

Imperial or Metric Grid?

The next step is to select a grid that is suitable placing and routing the components. All the objects placed in the PCB workspace are placed on the current snap grid.

Traditionally, the grid was selected to suit the component pin pitch and the routing technology that you planned to use for the board - i.e. how wide do the tracks need to be and what clearance is needed between tracks. The basic idea is to have both the tracks and clearances as wide as possible to lower the costs and improve the reliability. Ultimately, the selection of track/clearance is driven by what can be achieved on each design, which comes down to how tightly the components and routing must be packed to get the board placed and routed.

Over time, components and their pins have dramatically shrunk in size, as has the spacing of their pins. The component dimensions and spacing of their pins has moved from being predominantly imperial with thru-hole pins to being more-often metric dimensions with surface mount pins. If you are starting out a new board design, unless there is a strong reason, such as designed a replacement board to fit into an existing (imperial) product, you are better off working in metric.

Why?

Because the older, imperial components have big pins with lots of room between them. On the other hand, the small, surface mount devices are built using metric measurements - they are the ones that need a high level of accuracy to ensure that the fabricated/assembled/functional product works and is reliable. Also, the PCB editor can easily handle routing to off-grid pins, so working with imperial components is not onerous.

Suitable Grid Settings

For a design such as this simple tutorial circuit, practical grid and design rule settings would be:

Setting	Value	Where
Routing width	0.25 mm	Routing Width design rule
Clearance	0.25 mm	Electrical Clearance design rule
Board definition grid	5 mm	Cartesian Grid Editor
Component placement grid	1 mm	Cartesian Grid Editor
Routing grid	0.25 mm	Cartesian Grid Editor
Via size	1 mm	Routing Via Style design rule
Via hole	0.6 mm	Routing Via Style design rule

This routing grid is chosen not just to allow tracks to be placed as close as possible and still satisfy the clearance; the PCB editor manages this automatically. The point of setting the grid to be equal to, or a fraction of, the track+clearance is not just to ensure that the clearance is maintained, it is to ensure tracks are placed so that they do not waste potential routing space, which can easily happen if a very fine grid is used.

Setting the Snap Grid

The value of the snap grid can be configured directly in the Home tab of the Ribbon, or it can be configured in the Cartesian Grid Editor dialog (Home | Grids and Units | Properties).

Set the Snap Grid to 1 mm, ready to position the components.

Defining the component placement snap grid:

1. Click Home | Grids and Units | Properties to open the Cartesian Grid Editor dialog. You can also access the Cartesian Grid Editor dialog directly using the Ctrl+G shortcut keys.
2. Type the value 1mm into the Step X field. Because the X and Y fields are linked, there is no need to define the Step Y value.
3. To make the grid visible at lower zoom levels, set the Multiplier to 5x Grid Step. To make it easier to distinguish between the two grids, set the Fine grid to display as lighter colored Dots.
4. Click OK to close the dialog.

Setting Up the Design Rules

Main article: PCB Design Rules References

The PCB Editor is a rules-driven environment, meaning that as you perform actions that change the design, such as placing tracks, moving components, or autorouting the board, the software monitors each action and checks to see if the design still complies with the design rules. If it does not, the error is immediately highlighted as a violation. Setting up the design rules before you start working on the board allows you to remain focused on the task of designing, confident in the knowledge that any design errors will immediately be flagged for your attention.

Design rules are configured in the PCB Rules and Constraints Editor dialog as shown below (Home | Design Rules | Design Rules). The rules fall into 6 categories, which can then be further divided into design rule types. The rules cover electrical, routing, mask, plane, manufacturing, and placement requirements.

Routing Width Design Rules

The tutorial design includes a number of signal nets and two power nets. The default routing width rule (rule scope of All) will be configured at 0.25mm for the signal nets, and two more rules will be added to target the power nets.

Three Routing Width design rules have been defined: the lowest priority rule targets All nets, the two higher priority rules target the 12V and GND nets.

Configuring the Routing Width Rule for the signal nets:

1. With the PCB as the active document, open the PCB Rules and Constraints Editor.
2. Each rules category is displayed under the Design Rules folder (left hand side) of the dialog. Double-click on the Routing category to expand the category and see the related routing rules. Then double-click on Width to display the currently defined width rules.
3. Click once on the existing Width rule to select it. When you click on the rule, the right hand side of the dialog displays the settings for that rule including: the rule's Where the Object Matches (also referred to as the rule's scope - what you want this rule to target) in the top section and the rule's Constraints below that.
4. Since this rule is to target the majority of nets in the design (the signal nets), confirm that the Where the Object Matches setting is set to All.
5. The settings in this rule are the defaults for a new PCB. Edit the Min Width, Preferred Width & Max Width values and set them to 0.25mm. Note that the settings are reflected in the individual layers shown at the bottom of the dialog. You can also configure the requirements on a per-layer basis.
6. The rule is now defined. Click Apply to save it and keep the dialog open.

Adding Routing Width Rules for the power nets:

1. The next step is to add and configure two new design rules to specify the routing width for the power nets. To add and configure these rules, open the PCB Rules and Constraints Editor.
2. With the existing Width rule selected in the Design Rules tree on the left of the dialog, right-click then select New Rule to add a new Width constraint rule.

3. A new rule named Width_1 appears. Click on the new rule in the Design Rules tree to configure its properties.
4. Click in the Name field on the right and enter the name Width_12V in the field.
5. In the Where the Object Matches setting, select Net from the drop-down, then choose the 12V net from the second drop-down as shown below.

6. The last step is to set the Constraints for the rule. Edit the Min Width / Preferred Width / Max Width values 0.25 / 0.5 / 0.5, respectively, to allow power net routing widths in the range 0.25mm to 0.5mm, as shown below.

7. Repeat this sequence of steps to define another Routing Width Design Rule that targets the GND net, with the same Constraints values. The easiest way to do this is to use the Duplicate Rule command in the right-click menu, then change the Name of this new rule to Width_GND, and the Net to GND.
8. Click Apply to save the rules and keep the dialog open.

Defining the Electrical Clearance Constraint

The next step is to define how close electrical objects that belong to different nets can be to each other. This requirement is handled by the Electrical Clearance Constraint. For the tutorial, a clearance of 0.25mm between all objects is suitable. Note that entering a value into the Minimum Clearance field will automatically apply that value to all of the fields in the grid region at the bottom of the dialog. You only need to edit in the grid region when you need to define a clearance based on the object-type.

Defining the Electrical Clearance Constraint:

1. Expand the Electrical category in the tree of Design Rules, then expand the Clearance rule-type.
2. Click to select the existing Clearance constraint. Note that this rule has two Full Query fields, that is because it is a Binary rule. The rules engine checks each object targeted by the setting Where the First Object Matches and checks it against the objects targeted by the Where the Second Object Matches setting to confirm that they satisfy the specified Constraints settings. For this design, it is suitable to define a single clearance between All objects.
3. In the Constraints region of the dialog, set the Minimum Clearance to 0.25mm.
4. Click Apply to save the rule and keep the dialog open.

Defining the Routing Via Style

If you place a via from the Ribbon, its values are defined by the built-in default primitive settings. As you route and change layers, a via is automatically added. In this situation, the via properties are defined by the applicable Routing Via Style design rule.

Defining the Routing Via Style Design Rule:

1. Expand the Routing category in the tree of Design Rules then select the default RoutingVias design rule under Routing Via Style.
2. Since it is highly likely that the power nets can be routed on a single side of the board, it is not necessary to define a routing via style rule for signal nets and another routing via style rule for power nets. Edit the rule settings to the values suggested earlier in the tutorial, that is a Via Diameter = 1mm and a Via Hole Size = 0.6mm. Set all fields (Minimum, Maximum, Preferred) to the same size. Note that you can press Tab on the keyboard to move from one dialog field to the next.
3. Click OK to close the PCB Rules and Constraints Editor.
4. Save the PCB file.

Existing Design Rule Violation

You might have noticed that the transistor pads are showing that there is a violation. Right-click over a violation and select Violations in the right-click menu. The details show that there is a:

• Clearance Constraint violation
• Between a Pad on the MultiLayer, and a Pad on the MultiLayer
• Where the clearance is 0.22mm, which is less than the specified 0.25mm

Positioning the Components on the PCB

There is a saying that PCB design is 90% placement and 10% routing. While you could argue about the percentage of each, it is generally accepted that good component placement is critical for good board design. Keep in mind that you may need to tune the placement as you route too.

Component Positioning and Placement options

The default behavior when moving a component is to hold it by the reference point (Snap To Center) option defined in the PCB Library editor, rather than where you happened to click on it. The Smart Component Snap option allows you to override this behavior and snap to the nearest component pad, which is handy when you need to position a specific pad in a specific location.

Setting the component positioning options:

1. Select File » System Preferences to open the Preferences dialog.
2. Open the PCB Editor - General page of the dialog, in the Editing Options section, make sure the Snap To Center option is enabled. This ensures that when you "grab" a component to position it, the cursor will hold the component by its reference point.
3. Note the Smart Component Snap option. If this is enabled, you can force the software to snap to a pad center instead of the reference point by clicking and holding closer to the required pad than the component's reference point. This is very handy if you require a specific pad to be on a specific grid point. It can work against you if you are working with small surface mount components though, as it can make it harder to "grab" them by their reference point.

Positioning Components

You can now position the components in suitable locations on the board.

To move a component either:

• Click and Hold the left mouse button on the component, move it to the required location, then release the mouse button to place it, or
• Run the Tools | Arrange | Move » Component command, then single-click to pick up a component, move it to the required location, then click once to place it. When you are finished, right-click to drop out of the Move Component command.

Components positioned on the board.

Positioning the components:

1. Zoom to display the board and the component. One way to do this is to zoom out (PgDn) so the board and the components are all visible, right-click and choose View » View Area then click to define the top left and bottom right of the exact area you want to view.
2. The components will be positioned on the current Snap Grid. For a simple design such as this, there are no specific design requirements that dictate what placement grid should be used. As the designer, you decide what a suitable placement grid would be. To simplify the process of positioning the components, you can work with a coarse placement grid, for example, 1mm. Confirm that the Snap Grid is set to 1mm in the Home tab of the Ribbon.
3. The components in the tutorial can be placed as shown in the image above. To place connector Y1, position the cursor over the middle of the outline of the connector then Click-and-Hold the left mouse button. The cursor will change to a cross hair and jump to the reference point for the part. While continuing to hold down the mouse button, move the mouse to drag the component.
4. Position the footprint towards the left-hand side of the board (ensuring that the whole of the component stays within the board boundary) as shown in the figure above.
5. When the connector component is in position, release the mouse button to drop it into place. Note how the connection lines drag with the component.
6. Reposition the remaining components using the figure above as a guide. Use the Spacebar to rotate components (in increments of 90º counterclockwise) as you drag them so that the connection lines are as shown in the figure.
7. Component text can be repositioned in a similar fashion - click-and-drag the text then press the Spacebar to rotate it.
8. The PCB editor also includes powerful interactive placement tools. Let's use these to ensure that the four resistors are correctly aligned and spaced.
9. Holding the Shift key, click on each of the four resistors to select them or click and drag the selection box around all four of them. A shaded selection box will display around each of the selected components in the color set for the system color Selections (set in the 2D System Colors dialog).
10. Right-click on any of the selected components then choose Align » Align to open the Align Objects dialog.
11. Select Space Equally in the Horizontal section and Bottom in the Vertical section; click OK to apply these changes. The four resistors are now aligned (with the lowest component) and equally spaced.

 

12. Click elsewhere in the design window to de-select all the resistors. If required, you also can align the capacitors and transistors, although this might not be required since you currently have a coarse Snap Grid.

With everything positioned, it's time to do some routing!

Interactively Routing the Board

Routing is the process of laying tracks and vias on the board to connect the component pins. The PCB editor makes this job easy by providing sophisticated interactive routing tools, as well as the topological autorouter that optimally routes the whole or part of a board at the click of a button. While autorouting provides an easy and powerful way to route a board, there will be situations where you will need exact control over the placement of tracks. In these situations you can manually route part or all of your board.

In this section of the tutorial, you will manually route the entire board single-sided, with all tracks on the top layer. The Interactive Routing tools help maximize routing efficiency and flexibility in an intuitive way, including cursor guidance for track placement, single-click routing of the connection, pushing obstacles, and automatically following existing connections, all in accordance with applicable design rules.

Preparing for Interactive Routing

Before starting to route, it is important to configure the Interactive Routing options found in the PCB Editor - Interactive Routing page of the Preferences dialog.

Preparing for interactive routing:

1. Set the Routing Conflict Resolution Current Mode drop-down to Stop At First Obstacle. You can cycle through the enabled modes interactively as you route by pressing Shift+R.
2. In the Interactive Routing Options region, confirm that the Automatically Remove Loops option is enabled. This option allows you to change existing routing by routing an alternate path, i.e. you route a new path until it meets the old path (creating a loop), then right-click to indicate it is complete. The software then automatically removes the old, redundant part of the routing.
3. Confirm that the Interactive Routing Width / Via Size Sources options are both set to Rule Preferred.
4. Set the Snap Grid to 0.25mm in the Home | Grids and Units | Snap Grid.

Time to Route

• Interactive routing is launched by clicking the Route button -  _-  on the Home tab (or press the Shortcut key R). You only need to use the drop-down menu if you need to select one of the other routing options.
• Since the components are mostly surface mount, the board will be routed on the top layer. As you place tracks on the top layer of the board, you use the ratsnest (connection lines) to guide you.
• Tracks on a PCB are made from a series of straight segments. Each time there is a change of direction, a new track segment begins. Also, by default, the PCB editor constrains tracks to a vertical, horizontal or 45° orientation, which allows you to easily produce professional results. This behavior can be customized to suit your needs; for this tutorial we will use the default.
• After reaching the target pad, right-click or press Esc to release that connection - you will remain in Interactive Routing mode, ready to click on the next connection line.

A simple animation showing the board being routed. Note that many of the connections are finished using the Ctrl+Click to autocomplete feature.

Interactively routing the board:

1. Check which layers are currently visible by looking at the layer tabs at the bottom of the workspace. If the Bottom Layer is not visible, press the L shortcut to open the View Configurations dialog and enable the Bottom Layer.
2. Click on the Top Layer tab at the bottom of the workspace to make it the current, or active layer, on which to route.
3. It is often easier to route in single layer mode. You can press Shift+S to toggle to in and out of single layer mode.
4. Click Home | Routing | Route » Interactive Routing or right-click then choose Interactive Routing from the context menu. The cursor will change to a crosshair indicating you are in interactive routing mode.
5. Position the cursor over the lower pad on connector Y1. As you move the cursor close to the pad, it will automatically snap to the center of the pad; this is the Snap To Object Hotspot feature pulling the cursor to the center of the nearest electrical object (configure the Range of attraction in the Board Options dialog). Sometimes the Snap To Object Hotspot feature pulls the cursor when you do not want it to. In this situation, press the Ctrl key to temporarily inhibit this feature.
6. Left-Click or press Enter to anchor the first point of the track.
7. Move the cursor towards the bottom pad of the resistor R1 then click to place a vertical segment. Note how track segments are displayed in different ways (as shown in the image below). During routing, the segments are shown as:
   • Solid - the segment has been placed.
   • Hatched - hatched segments are proposed but uncommitted; they will be placed when you left-click.
   • Hollow - this is referred to as the look-ahead segment. It allows you to work out where the last proposed segment should end. This segment is not placed when you click. The look-ahead mode can be toggled on/off using the 1 shortcut during routing.

Note how the segments are displayed differently.

8. Manually route by Left-Clicking to commit track segments, finishing on the lower pad of R1. Note how each mouse click places the hatched segment(s). For the connection that you are currently routing, press Backspace to rip up (remove) the last-placed segment.
9. Rather than routing all the way to the target pad, you can also press Ctrl+Left Click to use the Auto-Complete function and immediately route the entire connection. Auto-complete behaves in the following way:
   • It takes the shortest path, which may not the best path since you need to always consider paths for other connections yet to be routed. If you are in Push mode (shown on the Status bar when routing), Auto-complete can push existing routes to reach the target.
   • On longer connections, the Auto-Complete path may not always be available since the routing path is mapped section by section and, therefore, complete mapping between source and target pads may not be possible.
   • You also can Auto-complete directly on a pad or connection line.
10. Continue to route all the connections on the board.
11. Use the techniques detailed above to route between the other components on the board. The simple animation above shows the board being interactively routed.
12. There is no single solution to routing a board, therefore, it is inevitable that you will want to change the routing. The PCB editor includes features and tools to help you do this and they are discussed in the following sections.
13. Save the design when you are finished routing.

Routing Tips

Keep in mind the following points as you are routing:

Keystroke	Behavior
~ (tilda)  or  Shift+F1	Pop up a menu  of interactive shortcuts - most settings can be changed on the fly by pressing the appropriate shortcut or selecting from the menu.
*  or  Ctrl+Shift+WheelRoll	Switch to the next available signal layer. A via is automatically added in accordance with the applicable Routing Via Style design rule.
Shift+R	Cycle through the enabled conflict resolution modes. Enable the required modes on the PCB Editor - Interactive Routing Preferences page.
Shift+S	Toggle single layer mode on and off. This is ideal when there are many objects on multiple layers.
Spacebar	Toggle the current corner direction.
Shift+Spacebar	Cycle through the various track corner modes. The styles are: any angle, 45°, 45° with arc, 90°, and 90° with arc. There is an option to limit this to 45° and 90° on the PCB Editor - Interactive Routing Preferences page.
Ctrl+Left-Click	Auto-complete the connection being routed. Auto-complete will not succeed if there are unresolvable conflicts with obstacles.
Ctrl	Temporarily suspend the Hotspot Snap, or press Shift + E to cycle through the three available modes (off / on for current layer / on for all layers).
End	Redraw the screen.
PgUp / PgDn	Zoom in / out centered around the current cursor position. Alternatively, use the standard Windows mouse wheel zoom and pan shortcuts.
Backspace	Remove the last committed track segment.
Right-click  or  ESC	Drop the current connection, remaining in Interactive Routing mode.

Interactive Routing Modes

The PCB editor's Interactive Routing engine supports a number of different modes, with each mode helping you to deal with particular situations. Press the Shift+R shortcut to cycle through these modes as you interactively route. Note that the current mode is displayed on the Status bar.

The available interactive routing modes include:

• Ignore - this mode lets you place tracks anywhere, including over existing objects, displaying but allowing potential violations.
• Stop at first obstacle - in this mode, the routing is essentially manual; as soon as an obstacle is encountered, the track segment will be clipped to avoid a violation.
• Push - this mode will attempt to move objects (tracks and vias) that are capable of being repositioned without violation to accommodate the new routing.

Modifying and Rerouting

To modify an existing route, there are two approaches: reroute or re-arrange.

Reroute an Existing Route

• There is no need to un-route a connection to redefine its path. Click the Route button and start routing the new path.
• The Loop Removal feature will automatically remove any redundant track segments (and vias) as soon as you close the loop and right-click to indicate you are complete (Loop Removal was enabled earlier in the tutorial).
• You can start and end the new route path at any point, swapping layers as required.
• You can also create temporary violations by switching to Ignore Obstacle mode (as shown in the animation below), which you later resolve.

A simple animation showing the Loop Removal feature being used to modify existing routing.

Re-arrange Existing Routes

• To interactively slide or drag track segments across the board, click, hold and drag as shown in the animation below.
• The PCB editor will automatically maintain the 45/90 degree angles with connected segments, shortening and lengthening them as required.

An animation showing track dragging being used to tidy up existing routing.

Track Dragging Tips

• During dragging, the routing conflict resolution modes also apply (Ignore, Push). Press Shift+R to cycle through the modes as you drag a track segment.
• Existing pads and vias will be jumped, or vias will be pushed if necessary and possible.  
• To convert a 90 degree corner to a 45 degree route, start dragging on the corner vertex. If a chooser window pops up (as shown in the animation above), you can select either track segment.
• While dragging you can move the cursor and hotspot snap it to an existing, non-moving object such as a pad (shown above). Use this to help align the new segment location with an existing object and avoid very small segments being added.
• To break a single segment, select the segment first, then position the cursor over the center vertex to add in new segments (shown above).
• Change the default select-then-drag mode using the Unselected via/track and Selected via/track options on the PCB Editor - Interactive Routing page of the Preferences dialog.

Automatically Routing the Board

Configuring the Autorouter

CircuitStudio also includes a topological autorouter. A topological autorouter uses a different method of mapping the routing space - one that is not geometrically constrained. Rather than using workspace coordinate information as a frame of reference (dividing it into a grid), a topological autorouter builds a map using only the relative positions of the obstacles in the space, without reference to their coordinates.

Topological mapping is a spatial-analysis technique that triangulates the space between adjacent obstacles. This triangulated map is then used by the routing algorithms to "weave" between the obstacle pairs from the start route point to the end route point. The greatest strengths of this approach are that the map is shape independent (the obstacles and routing paths can be any shape) and the space can be traversed at any angle - the routing algorithms are not restricted to purely vertical or horizontal paths as with a rectilinear expansion routers.

Translating this into a user interface, the router has a number of different routing passes available, such as Fan Out to Plane, Main, Memory, Spread, Recorner, etc. These are bundled together to create a Routing Strategy, which you can then run on their board. There are a number of pre-defined strategies already available in the Routing Strategies dialog, and new ones are easily created using the Strategy Editor.

Select an existing routing strategy, or create a new one in the Strategy Editor.

Running the Autorouter

• The autorouter is configured and run from the Tools | Autoroute | Autoroute menu on the Ribbon. Selecting All from the menu opens the Routing Strategies dialog, which is used to configure the strategies, select the required strategy, and run the autorouter.
• The autorouter will route on the layers allowed by the Routing Layers design rule in the directions specified in the autorouter Layer Directions dialog (where possible).

The images below show the autorouting results using the Default two Layer Board Strategy on the left, and a user-defined strategy on the right (the chosen routing passes are shown in the image above).

Autorouting results for the default two layer strategy (left image), and a user-defined strategy (right image).

Exploring the capabilities of the autorouter:

1. Un-route the board by selecting Home | Routing | Unroute » All from the Ribbon.
2. Select Tools | Autoroute | Autoroute » All. The Situs Routing Strategies dialog opens. The top region of the dialog displays the Routing Setup Report; warnings and errors are shown in red. Always check for warnings and errors! The lower half of the dialog shows the available Routing Strategies; the selected one will be highlighted. For this board, it should default to the Default 2 Layer Board strategy.
3. Click the Route All button in the Situs Routing Strategies dialog. The Messages panel displays the process of the autorouting. Because it routes your board directly in the PCB editing window, there is no need to wrestle with exporting and importing route files.
4. To route the board single-sided, click the Edit Layer Directions button in the Situs Routing Strategies dialog and modify the Current Setting field. Alternatively, you can modify the Routing Layers design rule.
5. Interestingly, the autorouter prefers a challenging board, often giving better results on a dense, more complex design than on a simple board. To improve the quality of the finished result, select Autoroute » All again, except this time select the Cleanup routing strategy. This strategy will attempt to straighten the routes, reducing the number of corners. You can run the Cleanup strategy multiple times if required. If nothing changes you might want to interactively re-route a connection in a convoluted pattern, then try the Cleanup strategy.
6. If you want to keep the autorouting results, save the PCB document. Otherwise, use Undo or close/open to return the board to the required routed state.

Configuring the Display of Rule Violations

CircuitStudio has two techniques for displaying design rule violations, each with their own advantages. These are configured on the PCB Editor - DRC Violations Display page of the Preferences dialog:

• Violation Overlay - Violations are identifed by the primitive-in-error being highlighted in the color chosen for the DRC Error Markers (configured in the View Configurations dialog; press L to open). The default behavior is to show the primitives in a solid color when zoomed out, changing to the selected Violation Overlay Style as you zoom. The default is Style B, i.e. a circle with a cross in it.
• Violation Details - As you zoom further in, Violation Detail is added (if enabled) that details the nature of the error. Use the Show Violation Detail slider to define at what zoom level the Violation Details start to display. Enable the required Display options in the Preferences dialog.

Violations are shown in solid red (left image); as you zoom in, this changes to an Overlay (center image) and as you zoom in further, Violation Details are added.

Preparing to run a Design Rule Check (DRC):

1. Open the View Configurations dialog (View|View |Switch to 3D » View Configurations » View Configuration). On the Board Layers And Colors tab, ensure the Show checkbox next to the DRC Error Markers option in the System Colors region is enabled (checked) so that DRC error markers will be displayed.
2. Confirm that the Online DRC (Design Rule Checking) system is enabled on the PCB Editor - General page of the Preferences dialog. Keep the Preferences dialog open; switch to the PCB Editor - DRC Violations Display page of the dialog.
3. The PCB Editor - DRC Violations Display page of the Preferences dialog is used to configure how violations are displayed in the workspace. There are two different methods available for displaying violations, each with their own strengths.
4. For the tutorial, right-click in the Display area of the PCB Editor - DRC Violations Display page of the Preferences dialog then select Show Violation Details - Used; right-click again then select Show Violation Overlay - Used (shown in the image above).
5. You are now ready to check the design for errors.

Configuring the Rule Checker

The design is checked for violations by running the Design Rule Checker. Click the Design Rule Check button - - on the Home tab of the Ribbon to open the dialog. Both online and batch DRC are configured in this dialog.

DRC Report Options

• By default, the dialog opens showing the DRC Report Options page selected in the tree on the left of the dialog (shown below).
• The right side of the dialog displays a list of general reporting options. For more information about the options, press F1 when the cursor is over the dialog (try a second time if it fails to load the first time). Leave these options at their defaults.

DRC Rules to Check

• The testing of specific rules is configured in the Rules to Check region of the dialog. Select this page in the tree on the left of the dialog to list all of the rule types (shown below). You can also examine them by type, for example, Electrical, by selecting that page on the left of the dialog.
• For most rule types, there are checkboxes for Online (check as you work) and Batch (check this rule when the Run Design Rule Check button is clicked).
• Click to enable/disable the rules as required. Alternatively, right-click to display the context menu. This menu allows you to quickly toggle the Online and Batch settings. Select the Batch DRC - Used On entry as shown in the image below.

Running a Design Rule Check (DRC)

When the Run Design Rule Check button at the bottom of the dialog is clicked, the DRC will run.

• The Messages panel will appear and list all detected errors.
• If the Create Report File option was enabled in the Report Options page of the dialog, a Design Rule Verification Report will open in a separate document tab. A sample report is shown below.
• Below the summary of violating rules will be specific details about each violation.
• The links in the report are live. Click on an error to jump back to the board and examine that error on the board. Note that the zoom level for this click action is configured on the System - General Settings page of the Preferences dialog. You can experiment to find a zoom level that suits you.

Identifying the Error Condition

When you are new to the software, a long list of violations can initially seem overwhelming. A good approach to managing this is to disable and enable rules in the Design Rule Check dialog at different stages of the design process. It is not advisable to disable the design rules themselves, just the checking of them. For example, you would always disable the Un-Routed Net check until the board is fully routed.

• When a batch DRC is run on the tutorial board, there are four clearance constraint violations, which means the measured values are less than the minimum amounts specified in the applicable design rule(s). You now know how to locate those violations (click the link in the report file or double-click in the Messages panel), and using the Violation Details, you can understand the error condition.
• The image below shows the Violation Details for one of the clearance constraint errors, which is indicated by the white arrows and the 0.25mm text. The next step is to work out what the actual value is so you know by how much it has failed.

The Violation Details show that the clearance between these two pads
is less that 0.25mm; it does not detail the actual clearance.

Apart from actually measuring the distance, there are two approaches to working out by how much the rule has failed:

• the right-click Violations submenu, or
• the PCB Rules and Violations panel.

The Violations Submenu

The right-click Violations submenu was described earlier in the Existing Design Rule Violation section.

• The image below shows how the Violations submenu details the measured condition against the value specified by the rule.

Right-click on a violation to examine what rule is being violated and the violation conditions.

The PCB Rules and Violations Panel

The second approach to understanding the error condition is to use the PCB Rules and Violations panel.

• Click the View | PCB | Rules and Violations button to display the panel.

• Click once on a Violation to jump to that violation; double-click on a violation to open the Violation Details dialog.

Resolving the Violation

As the designer, you have to work out the most appropriate way of resolving each design rule violation. There are two ways of resolving this clearance constraint:

• Decrease the size of the transistor footprint pads to increase the clearance between the pads, or
• Configure the rules to allow a smaller clearance between the transistor footprint pads.

Since the 0.25mm clearance is quite generous and the actual clearance is quite close to this value (0.22mm), a good choice in this situation would be to configure the rules to allow a smaller clearance. This can be done in the existing Clearance Constraint design rule, as shown below.

• The TH Pad - to - TH Pad value is changed to 0.22mm in the grid region of the rule constraint. To edit a cell first select it, then press F2.
• This solution is acceptable in this situation because the only other component with thruhole pads is the connector, which has pads spaced over 1mm apart.

Well done! You have completed the PCB layout and are ready to produce output documentation. Before doing that, let's explore the PCB editor's 3D capabilities.

Viewing Your Board in 3D

A powerful feature of CircuitStudio is the ability to view your board as a three-dimensional object. To switch to 3D, click the Switch to 3D button  (View | View group), or press the 3 shortcut. The board will display as a three-dimensional object; the tutorial board is shown below.

You can fluidly zoom the view, rotate it and even travel inside the board using the following controls:

• Zooming - Ctrl + Right-drag mouse, or Ctrl + Roll mouse-wheel, or the PgUp / PgDn keys.
• Panning - Right-drag mouse, or the standard Windows mouse-wheel controls.
• Rotation - Shift + Right-drag mouse. Note that when you press Shift, a directional sphere appears at the current cursor position as shown in the image below. Rotational movement of the model is made around the center of the sphere (position the cursor before pressing Shift to position the sphere) using the following controls. Move the mouse around to highlight and select each one:
  • Right-drag sphere when the Center Dot is highlighted - rotate in any direction.
  • Right-drag sphere when the Horizontal Arrow is highlighted - rotate the view about the Y-axis.
  • Right-drag sphere when the Vertical Arrow is highlighted - rotate the view about the X-axis.
  • Right-drag sphere when the Circle Segment is highlighted - rotate the view about the Z-plane.

Hold Shift to display the 3D view directional sphere, then click and drag the right-mouse button to rotate.

Tips for Working in 3D

• Press L to open the View Configurations dialog when the board is in 3D Layout Mode in which you can configure the 3D workspace display options. There are options to choose various surface and workspace colors, as well as vertical scaling, which is handy for examining the PCB internally. Some surfaces have an opacity setting - the greater the opacity, the less 'light' passes through the surface, which makes objects behind less visible. You can also choose to show 3D bodies or render 3D objects in their (2D) layer color.
• To display the components in 3D, each component needs to have a suitable 3D model.
• You can import a 3D STEP-format model into the component footprint in the Library editor; place a 3D Body Object then select the Generic STEP Model type to embed a STEP model inside that 3D Body Object.
• Check out 3D Content Central for STEP-format component models. 
• If there is no suitable STEP model available, create your own component shape by placing multiple 3D Body Objects in the footprint in the Library editor.

Output Documentation

Now that you've completed the design and layout of the PCB, you're ready to produce the output documentation needed to get the board reviewed, fabricated and assembled.

The ultimate objective is to fabricate and assemble the board.

Available Output Types

Because a variety of technologies and methods exist in PCB manufacture, CircuitStudio has the ability to produce numerous output types for different purposes:

Assembly Outputs

• Assembly Drawings - component positions and orientations for each side of the board.
• Pick and Place Files - used by robotic component placement machinery to place components onto the board.

Documentation Outputs

• Composite Drawings - the finished board assembly, including components and tracks.
• PCB 3D Prints - views of the board from a three-dimensional view perspective.
• Schematic Prints - schematic drawings used in the design.

Fabrication Outputs

• Composite Drill Drawings - drill positions and sizes (using symbols) for the board in one drawing.
• Drill Drawing/Guides - drill positions and sizes (using symbols) for the board in separate drawings.
• Final Artwork Prints - combines various fabrication outputs together as a single printable output.
• Gerber Files - creates manufacturing information in Gerber format.
• NC Drill Files - creates manufacturing information for use by numerically controlled drilling machines.
• ODB++ - creates manufacturing information in ODB++ database format.
• Power-Plane Prints - creates internal and split plane drawings.
• Solder/Paste Mask Prints - creates solder mask and paste mask drawings.
• IPC-2581 Standard - creates an XML-based single file format that incorporates a rich range of board fabrication data – from layer stackup details to full pad/routing /component information and the Bill Of Materials (BOM).

Report Outputs

• Bill of Materials - creates a list of parts and quantities (BOM), in various formats that are required to manufacture the board.
• Report Single Pin Nets- creates a report listing any nets that only have one connection.
• Electrical Rules Check - formatted report of the results of running an Electrical Rules Check.

Individual Outputs or Managed Output Generation

CircuitStudio has two separate mechanisms for configuring and generating output:

1. Individually - the settings for each output type are stored in the Project file. You selectively generate that output when required using the options on the Outputs tab. These outputs are written to the folder specified in the Output Path setting on the Options tab of the Options for PCB Project dialog.
2. Managed Release - all output settings are stored in a special file in the project folder. You then generate all enabled outputs in a single action using the Generate Output Files dialog. Using this approach gives you confidence that all the correct outputs were generated from the same version of the source schematic and PCB files. The dialog is accessed either from the Project | Project Actions | Generate Outputs button or the Home | Project | Project » Generate outputs menu entry. These outputs are written to a folder named \Default Configuration. Once you have configured and enabled each required Outputer, click the Generate button in the dialog to generate the outputs in the \Default Configuration folder.

Preparing for a managed release:

1. The Generate Output Files dialog can be opened at any time with a schematic open, a PCB open, or no document open. Click the   button on the Project tab to open the dialog. Note that when you open the dialog, the special file that holds the output settings is automatically created in the project folder and therefore, the project file will now be marked as modified.
2. Note the list of Outputers that are included. For the tutorial, you will be using the Gerber Files outputer and the Bill of Materials outputer.
3. Click Configure... associated with Gerber Files to open the Gerber Setup dialog, which will be configured in the next set of steps.

Configuring the Gerber Files

• Gerber continues to be the most common form of data transfer between board design and board fabrication.
• Each Gerber file corresponds to one layer of the physical board - the component overlay, top signal layer, bottom signal layer, top solder mask layer, etc. It is advisable to consult with your board fabricator to confirm their requirements before supplying the output files required to fabricate your design.
• If the board has any holes, an NC Drill file must also be generated using the same units, resolution, and position on film settings.
• Gerber files are configured in the Gerber Setup dialog. If you intend to use the managed release approach, open the Gerber Setup dialog from the Generate Output Files dialog by clicking Configure associated with the Gerber Files entry.

Configuring Gerber generation:

1. In the Generate Output Files dialog, click Configure... associated with the Gerber Files output. The Gerber Setup dialog will open as shown in the image above. 
2. Since the board has been designed in Metric, set the Units to Millimeters on the General tab of the dialog.
3. The smallest unit used on the board is 0.25mm for the routing and clearance, but because most of the components have their reference point at their geometric center (and were placed on a 1mm grid), some of their pads will actually be on a 0.01 grid. Set the Format to 4:3 on the General tab. This ensures that the resolution of the output data is more than adequate to cover these grid locations. Note that the NC Drill file must always be configured to use the same Units and Format. 
4. On the Layers tab, click the Plot Layers button then select Used On. Note that mechanical layers may be enabled; these are not normally 'Gerbered' on their own. Instead they are often included if they hold detail that is required on other layers, for example, an alignment location marker that is required on every Gerber file. In this case, the Mechanical Layer(s) to Add to All Plots options on the right side of the dialog are used to include that detail with another layer. Disable any mechanical layers that were enabled in the Layers To Plot region.
5. On the Advanced tab of the dialog, confirm that the Position on Film option is set to Reference to relative origin. Note: the NC Drill file must always be configured to use the same Position on Film option. 
6. Click OK to accept the other default settings and close the Gerber Setup dialog.
7. The Gerber settings are configured. The next step is to configure other outputs. For this tutorial, you will also configure the BoM in the next set of steps.

Configuring the Bill of Materials

CircuitStudio includes a highly configurable BOM generation feature that can generate output in a variety of formats including: text, CSV, PDF, HTML, and Excel. Excel-format BOMs can also have a template applied using one of the pre-defined templates or one of your own.

• BoM output is configured in the Bill of Materials For Project dialog. If you intend to use the managed release approach, you open the Bill of Materials For Project dialog from the Generate Output Files dialog.
• On the left side of the dialog there is a list of every component attribute for all components in the design. Enable the checkbox for each attribute you want to include in the BOM and clear the checkbox for any attributes you want to remove.
• The default settings for the BOM is to cluster by like components. Clustering is achieved by adding component attributes to the Grouped Columns region of the dialog. Click and drag these attributes out of the Grouped Columns and drop them into the All Columns region if you prefer every component to be on its own row in the BOM.
• The main grid region of the dialog is the content that is written into the BoM. In this region you can click and drag to reorder the columns, click on a column heading to sort by that column, ctrl+click to sub-sort by that column, define value-based filters for a column using the small drop-down in each column header, and right-click to force the columns to fit the current dialog width.
• The BOM generator sources its information from the schematic. Enable the Include Parameters From PCB option to access PCB information, such as location and side of board (note that this feature can also be used to configure and generate a configurable pick and place file, if required).

The default configuration for a new BoM is to group like components together.

This BoM has been reconfigured to present each component as a unique entry.

Mapping design data into the BoM:

Mapping Design Data into the BoM

Design data can be passed from CircuitStudio into an Excel Bill Of Materials by including special statements in the Excel template used to create the BOM.

When creating the Bill of Materials template in Excel, a combination of fields and columns can be used to specify the desired layout. Several example templates are provided with CircuitStudio in the \Templates folder of the installation user files. A list of available fields is detailed below.

Fields

Fields provide project-level information. These are not usually attached to each item listed in the BOM, but are often used in the header of the document. Fields are used in the format:

Field=FieldName

An example would be Field=Currency

The available fields include:

Currency	DataSourceFileName	DataSourceFullPath
GeneratorDescription	GeneratorName	OutputName
OutputType	ProductionQuantity	ProjectFileName
ProjectFullPath	ReportDate	ReportDateTime
ReportTime	TotalQuantity	Title (title of BoM)
VariantName

Document and Project Parameters

As well as the default Fields listed in the table above, schematic Document Parameters (both default and user-defined in the schematic Document Options dialog) and Project Parameters (Options for PCB Project dialog) can also be used as Fields.

These are entered as:

Field=ParameterName

If the same parameter exists as both a document parameter and a project parameter, the project parameter takes precedence. If the same document parameter exists in multiple documents, the document parameter that is higher up in the hierarchy takes precedence.

Below are the default document parameters, also referred to as the System parameters.

Address1	Address2	Address3
Address4	ApprovedBy	Author
CheckedBy	CompanyName	ConfigurationParameters
CurrentDate	CurrentTime	Date
DocumentFullPathAndName	DocumentName	DocumentNumber
DrawnBy	Engineer	ImagePath
Index	ModifiedDate	Organization
Revision	Rule	SheetNumber
SheetTotal	Time

Columns

Columns provide the information that is supplied on a per-component basis and would usually appear on each line in the BOM. Columns are defined by entering the column heading in the format:

Column=ColumnName

An example would be Column=Description or Column=LibRef

Column information can be taken from several sources including:

• Default component parameters (such as Designator or Description)
• User-defined parameters added to components
• PCB data
• Supplier data

These are discussed separately below.

Default Parameters

These ColumnNames are available for all components:

Comment	ComponentKind	Description
Designator	DesignItemId	Footprint
LibRef	LogicalDesignator	PartType
PhysicalPath	Quantity	UniqueIdName
UniqueIdPath

PCB Parameters

Pick and Place information can also be included from the PCB. In order to use these columns, the checkbox Include Parameters From PCB must be checked in the BOM Configuration dialog.

Center-X(Mil)	Center-X(mm)	Center-Y(Mil)
Center-Y(mm)	Layer	Pad-X(Mil)
Pad-X(mm)	Pad-Y(Mil)	Pad-Y(mm)
Ref-X(Mil)	Ref-X(mm)	Ref-Y(Mil)
Ref-Y(mm)	Rotation

Supplier Data

it is possible to retrieve online data from suppliers and feed that into the BOM. Note that these are updated live and are retrieved when the BOM is generated. Multiple suppliers can be set up for each component. In the table below, these have been described as Supplier Info x - replace x with the appropriate number.

Manufacturer x	Manufacturer Part Number x	Supplier x
Supplier Currency x	Supplier Order Qty x	Supplier Part Number x
Supplier Stock x	Supplier Subtotal x	Supplier Unit Price x

If you have just edited parameters in the schematic and want to see them in the BoM, save the edited documents and recompile the project before generating the BoM.