Tutorial - A Complete Design Walkthrough with Altium NEXUS

1. Select File » New » Project from the menus.
2. The Create Project dialog will open:
   • Select the required managed content server in the list of Locations. In the image above, the managed content server is named Nomad Engineering.
   • Confirm that the Project Type is PCB <Default>.
   • Enter a suitable name as the Project Name; include a description if required.
   • Confirm that the Repository field is set to Versioned Storage (more on this below).
   • The Folder field defines the name of the folder on the NEXUS Server where your project files are to be stored. The default is to have a Projects folder on the NEXUS Server. The files for each project will be stored in a project-named folder within it.
   • In the Local Storage field, select a suitable location to store the working copy of the project. A folder of the same name as the project will automatically be created in this location, and the working copy of the project file  will be saved in it.
3. Click Create to close the dialog and create the project. This will take a few moments, as the file is created on the managed content server, and a working copy checked out into the working folder (as specified in the Local Storage field).
4. The new project will appear in the Projects panel. If this panel is not displayed, click the button at the bottom right of the main design window, and select Project from the menu that appears.
5. The project will display a small blue cross next to its name. This indicates that it has been added to the VCS but is yet to be committed. To commit the project, right-click on the project name in the Projects panel and select Version Control » Commit Whole Project from the context menu (show me).
6. The Commit to Version Control dialog will open. Confirm that the file Multivibrator.PrjPcb is checked then click the Commit And Push button. A status dialog will appear while the file is written to the version control repository. When this is complete a small green check will appear next to the project filename in the Projects panel.

1. Right-click on the project filename in the Projects panel then select Add New to Project » Schematic, as shown in the image above. 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 (or use the right-click context menu). 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 and click Save (there is no need to type in the extension). 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, whereas 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 to save the project.

4. The last step is to commit the new schematic and the modified project file to the repository. To do this, right-click on the project name in the Projects panel and select Version Control » Commit Whole Project from the context menu.
5. The Commit to Version Control dialog will open. Confirm that the Multivibrator.PrjPcb and Multivibrator.SchDoc files are checked then click the Commit And Push button. A status dialog will open while the files are written to the version control repository. When this is complete, a small green check will appear next to the filenames in the Projects panel, as shown in the image above.

The properties of most objects, including the schematic sheet (or PCB workspace), are configured in the Interactive Properties panel. The panel automatically displays the properties of the selected object, or if no object is selected, it displays the properties of the schematic sheet (or PCB workspace).

1. If the Properties panel is not visible, click the  button at the bottom right of the application and select Properties from the menu that appears.
2. In Document Options mode (when nothing is selected), the panel is divided into the following sections: Selection Filter, General and Page Options. Each section can be opened/collapsed via the small triangle next to the section name. 
3. For this tutorial, the only change we need to make here is to set the sheet size to A4; this is done in the Page Options section.
4. Confirm that both the Snap and Visible Grids are set to 100mil.
5. To make the document fill the viewing area, select View » Fit Document (shortcut: V, D).
6. Save the schematic by selecting File » Save (shortcut: F, S).

• Categories are accessed using the drop-down, indicated by Number 1 in the image above.
• Click the button to toggle the Filters list on and off (Number 2 in the image). The contents of the Filters list changes to suit the category of component being searched.
• Some of the Filter fields include text boxes to enter numeric values. Press Enter on the keyboard to apply the value.
• If the results list does not update, click in the Search field and press Enter on the keyboard.
• The current search criteria defined by the chosen Category and enabled Filters list are detailed just below the search bar. Click the small x icon to remove any of the existing search criterion.
  
• Click on a column heading to sort the results by that column.
• Right-click on an existing column heading to access the Select Columns dialog ( show me).

• If the manufacturer provides an image of the part, it will be displayed. Next to the image is the Manufacturer Part Number (MPN), which is also link to detailed information about the part on the Octopart website (indicated by the number 1 in the image above).
• The vertical colored bar indicates the manufacturer's Lifecycle status; for example, Volume Production, EOL, etc. Hover the cursor over the bar for more information. Note that the manufacturer's Lifecycle status is not an indication of availability; that is displayed in the individual supplier tiles (as described below). For example, a manufacturer might have a part flagged as End of Life, but suppliers might still have large amounts of stock.
  ► Learn more about Interpreting the Manufacturer Lifecycle State.
• Click anywhere on a row to select that part. The row will highlight and a second link will appear indicating the number of suppliers who can deliver that part (number 2 in the image above). Click the link to display detailed supply chain information about the suppliers that carry that part, ordered by availability and price.
• Each Supplier's details about that part are presented on a tile with a colored banner. These tiles are also referred to as SPNs (Supplier Part Numbers). Details about the icons and information in each tile is given below.
• Click the panel's  button to configure: the currency used, if invalid SPNs should be excluded (display only suppliers that show suitable stock levels and up-to-date data), or configure the available suppliers.

1. Tile banner showing the Supplier name where the banner color indicates:
   • Green = Best choice
   • Orange = Acceptable
   • Red = Risky
2. Supplier part number (links to that part on the Supplier's website).
3. Last updated icon; the color indicates:
   • Light Gray = Default, updated less than one week ago
   • Orange = 1 week < last update < month ago
   • Red = last update > 1 month ago
4. Country code for the Supplier location (ISO alpha 2); colored red if unknown.
5. Part source.
6. Stock quantity; red if no stock available.
7. Unit price, red if no price available. Unit price includes currency icon; currency is determined by the location of the supplier.
8. Available price breaks, with Minimum Order Quantities.

Storing Unmanaged File-based Components

The following file-based component storage options can be used with Altium NEXUS:

Libraries Available for Placing Unmanaged Components

Dialog page: Available File Libraries

In Altium NEXUS, library-based components can only be placed from available libraries. The term available libraries includes:

• Libraries in the current project - if a library is part of the project, then the components in it are automatically available for placement within that project.
• Installed libraries - these are libraries that have been installed in Altium NEXUS, their components are available for use in any open project.
• Libraries on a defined search path - it is also possible to define a search path to a folder that holds multiple libraries. Because all files in the search path are searched every time a new component is chosen in a panel, this approach is only recommended for small libraries that hold simple model definitions, such as simulation models. Search paths are not recommended for complex models, such as footprints that include 3D models.

Installing a File Library

Libraries are installed in the Installed tab of the Available File Libraries dialog. To open the dialog, click the  button at the top of the Components panel and select File-based Libraries Preferences from the menu.

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

Advanced Searching in File-Libraries

To help find a component in both installed and not-installed libraries, Altium NEXUS includes a library searching feature.

Searching is performed in the File-based Libraries Search dialog, which is accessed by clicking the button on the Components panel, and selecting File-based Libraries Search from the menu. 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.

Search across installed libraries (Available libraries), or libraries on the hard drive (Libraries on path).

• The Scope of the search is libraries that are:
  • already installed (Available libraries), or
  • in libraries located in on the hard drive (Libraries on Path). The Path is set to point to the folder holding the file libraries, for example the supplied libraries are stored in C:\Users\Public\Documents\Altium\Altium NEXUS <Version>\Library.

• Click the Search button to begin the search. The results are displayed in the Components panel as the search takes place.
• You can only place components from file-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.

1. Select View » Fit Document (shortcut: V, D) to ensure your schematic sheet takes up the full editing window.
2. Using the search techniques just described, use the Manufacturer Part Search panel to search for: transistor BC547 .
3. Display the information section of the panel so that you can explore the properties and models of the selected component. You will be choosing a component that includes a symbol and footprint.
4. To explore the availability of a component, select it in the panel then click the SPN link that appears.

5. Click to select the required transistor in the results grid in the panel then click the Download drop-down (as shown below) and select Place. 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 Properties panel. The default behavior is to automatically highlight the most-used field in the panel, ready for editing; in this case it will be the Designator. Note that each section of the panel can be individually expanded or collapsed, which means your panel might look different.

Set the Designator to Q1, and the Comment to be visible.

7. In the Properties section of the panel, type in the Designator Q1.
8. Confirm that the visibility control for the Comment field is set to visible ( ).
9. Leave all other fields at their default values then click the Pause button ( ) to return to part placement.
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, which is displayed on the left of the Status bar at the bottom of the application. It defaults to 100mil; you can press the G shortcut to cycle through the available grid settings during object placement. It is strongly advised to keep the snap grid at 100mil or 50mil to keep the circuit neat and make it easy to attach wires to pins. For a simple design such as this, 100mil is a good choice.
11. Once you are happy with the transistor's location, left-mouse click or press Enter on the keyboard to place the transistor onto the schematic. The location can be changed later, if required.
12. Move the cursor and you will find that a copy of the transistor has been placed on the schematic sheet, and you are still in part placement mode with the transistor outline floating on the cursor. This feature allows you to place multiple parts of the same type.
13. You are ready to place the second transistor. This transistor is the same as the previous one so there is no need to edit its attributes before you place it. 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.
14. If you refer to the schematic diagram shown above, you will notice that Q2 is drawn as a mirror of Q1. To horizontally flip the orientation of the transistor floating on the cursor, press the X key on the keyboard. This flips the component along the X axis.
15. 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.
16. 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.
17. Since both of 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.

1. Return to the Manufacturer Part Search panel and search for: capacitor 22nF 16V 0603. The search will return a number of potential capacitors; the components that have models will be listed first.
2. Select a capacitor in the search result grid (that has models), right-click on it and select Place from the context menu.
3. While the capacitor is floating on the cursor, press the Tab key to open the Properties panel.
4. In the Properties section of the panel, type in the Designator C1.
5. Confirm that the visibility control for the Comment field is set to visible.
6. Expand the Footprint section of the Properties panel. Many of the resistors and capacitors have three footprint models: IPC Low Density (M), IPC Medium Density (N), and IPC High Density (L). If you compare the footprint names, they will be identical except for the letter indicating density. Select the M variety as shown in the image below.

7. Leave the other fields at their default values and click the Pause button ( ) to return to part placement; 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 (refer to the schematic diagram shown earlier) and 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.
12. The default parameters for the capacitor may be only the manufacturer name and part number, but any of the parameters shown in the Manufacturer Part Search panel can be added to the placed capacitors. To check the current parameters, double-click on one of the capacitors to open the Properties panel then click on the Parameters tab at the top of the panel.
13. If the list of Parameters does not include the capacitance and voltage, return to the Manufacturer Part Search panel, confirm that the same capacitor is still selected, then click the Show More link to show the complete list of available parameters. Using the Windows Ctrl+click selection technique, select the following parameters (if available): Capacitance, Case/Package, Tolerance, and Voltage Rating.
14. Right-click on any of the selected parameters and select Add Parameters to Part from the context menu.

15. The cursor will change to a crosshair; left-click once on each capacitor in turn to add the selected parameters. If you find it difficult to position the cursor over the center of the capacitor symbol, hold the Ctrl key down to temporarily inhibit the snap grid.
16. Confirm that the parameters have been added to both C1 and C2.

1. In the Manufacturer Part Search panel, search for: resistor 100K 5% 0805. The search will return a number of potential resistors (including resistors with other values); the components that have models will be listed first.
2. Select a suitable 100K resistor in the search result grid (that has models), and display the footprint in the Models section of the panel.
3. Many of the resistors and capacitors have three footprint models: IPC Low Density (M), IPC Medium Density (N), and IPC High Density (L). If you compare the footprint names, they will be identical except for the letter indicating density. Select the M variety as shown in the image below. This selection can be done before the component is placed on the schematic during schematic placement or after schematic placement. 
4. Right-click on the resistor in the search results grid and select Place from the context menu, as shown below.

5. While the resistor is floating on the cursor, press the Tab key to open the Properties panel.
6. In the Properties section of the panel, type in the Designator R1.
7. Leave all other fields at their default values and click the Pause button ( ) to return to part placement; 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 previously) and 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 default parameters for the resistor may be only the manufacturer name and part number, but any of the parameters shown in the Manufacturer Part Search panel can be added to the placed resistors. To check the current parameters, double-click on one of the 100K resistors to open the Properties panel, then click on the Parameters tab at the top of the panel.
13. If the list of Parameters does not include the resistance, return to the Manufacturer Part Search panel. Confirm that the same resistor is still selected, then click the Show More link to show the complete list of available parameters. Using the Windows Ctrl+click selection technique, select the following parameters (if available): Case/Package, Resistance, and Tolerance.
14. Right-click on any of the selected parameters and select Add Parameters to Part from the context menu.
15. The cursor will change to a crosshair; left-click once on each resistor in turn to add the selected parameters.
16. Confirm that the parameters have been added to both R1 and R2. The visibility of the Resistance parameter will be changed shortly.
17. The remaining two resistors, R3 and R4, have a value of 1K; search for: resistor 1K 5% 0805 in the Manufacturer Part Search panel. The search will return a number of potential resistors (including resistors with other values). The components that have models will be listed first.
18. Select a suitable 1K resistor in the search result grid (that has models), and display the footprint in the Models section of the panel.
19. Many of the resistors and capacitors have three footprint models: IPC Low Density (M), IPC Medium Density (N), and IPC High Density (L). If you compare the footprint names, they will be identical except for the letter indicating density; select the M variety.
20. Right-click on the resistor in the search results grid and select Place from the context menu.
21. While the resistor is floating on the cursor, press the Tab key to open the Properties panel.
22. In the Properties section of the panel, type in the Designator R3.
23. Leave all other fields at their default values and click the Pause button ( ) to return to part placement; the resistor will be floating on the cursor.
24. Press the Spacebar to rotate the component in 90° increments until it has the correct orientation.
25. 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.
26. Right-click or press Esc to exit part placement mode.
27. Using the same process as described for R1 and R2; add the Case/Package, Resistance, and Tolerance parameters to R3 and R4.
28. The last step is to configure the visibility of the Parameters. This can be done for all four resistors at the same time. To select all of the resistors, drag the selection rectangle from right to left to select touching (demonstrated in the animation below).
29. On the General tab of the Properties panel, disable the visibility of the Comment parameter (demonstrated in the animation below).
30. On the Parameters tab of the Properties panel, enable the visibility of the Resistance parameter (demonstrated in the animation below).
31. Re-position the Resistance string to a suitable location. When a string is being moved, the snap grid can be temporarily disabled by holding down the Ctrl key. Alternatively, rotating any schematic component(s) (Ctrl+Spacebar) automatically sets all visible strings to their default locations (demonstrated in the animation below).

1. The last component to find is the 2-pin header. Return to the Manufacturer Part Search panel. This time you will use the panel's faceted searching capabilities.
2. In the Categories drop-down, select Headers and Wire Housings under Connectors.
3. Click the Filters button ( ) to display the Filters column.
4. The list of available filters is dynamically updated to suit the category being used, and can be quite long. To help manage it, only the most commonly-used filters are displayed. Scroll to the bottom of the list and click the  link to display all of the available filters.
5. An efficient way of working with the filters is to use the Search field at the top. Searching returns strings that match in either the Filter Name or in the Filter Settings. Using the following search terms, apply the filters and select the options listed below:

6. A small number of 2-pin vertical male headers should be returned, as shown below. Select a suitable 2-pin connector, such as the Samtec TSW-102-26-F-S or the Samtec TSW-102-26-G-S, from the search results; right-click on it and select Place from the menu.

7. While the header is floating on the cursor, press Tab to edit the attributes and set the Designator to P1.
8. Before placing the header, press Spacebar to rotate it to the correct orientation. Click to place the connector on the schematic, as shown in the image above.
9. Right-click or press Esc to exit part placement mode.
10. Save your 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 on the Active Bar (Place » Wire, or Ctrl+W shortcut) 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 (red cross) will appear at the cursor location. This indicates that the cursor is over a valid electrical connection point on the component.
4. Left-click 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. If the wire is forming a corner in the wrong direction, press Spacebar to toggle the corner direction.
6. Click or press Enter to connect the wire to the base of Q1. The cursor will release from that wire.
7. 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.
8. Next, wire from the lower pin of R3 to the collector of Q1. Position the cursor over the lower pin of R3 and click or press Enter to start a new wire. Move the cursor vertically until 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.
9. Wire up the rest of your circuit, as shown in the animation above.
10. When you have finished placing all the wires, right-click or press Esc to exit placement mode. The cursor will revert to an arrow.

1. Click the  button (Place » 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 Properties panel.
3. Type 12V in the Net field, then click the Pause button ( ) to return to object placement.
4. Place the net label so that its hotspot (the bottom left corner) touches the upper most wire on the schematic, as shown in the images 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 in the Properties panel before placing it.
6. Type GND in the Net Name field and press Enter to return to object placement mode.
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 completed schematic image above). Right-click or press Esc to exit net label placement mode.
8. Save your circuit and the project, as well.

1. Select Project » Project Options to open the Options for PCB Project dialog.
2. Scroll through the list of error checks and note that they are clustered in groups; each group can be collapsed if required.
3. Click on the Report Mode setting for any error check and note the options available.

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 on the dialog face to display a menu that lets you toggle all settings simultaneously, including an option to restore them 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. Let's change the default settings so that the connection matrix detects unconnected passive pins. Look down the row labels to find the Passive Pin row. 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 later in the tutorial.

1. Clear the Component Classes checkbox as shown in the image above. This will automatically disable the creation of a placement room for that schematic sheet.
2. There are no buses in the design so there is no need to clear the Generate Net Classes for Buses checkbox located near the top of the dialog.
3. There are no user-defined Net Classes in the design (done through the placement of Net Class directives on the wires) so there is no need to clear the Generate Net Classes checkbox in the User-Defined Classes region of the dialog.

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

1. To compile the Multivibrator project, select Project » Compile PCB Project Multivibrator.PrjPcb from the main menus.
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  the  button at the bottom right and select Messages from the menu.
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.

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

1. Click on the Multivibrator.SchDoc tab at the top of the design window to make the schematic sheet the active document.
2. 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.
3. Recompile the project (Project » Compile PCB Project Multivibrator.PrjPcb) to check for errors. The Messages panel will display error messages indicating you have unconnected pins in your circuit.
4. 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.
5. 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 in error. 
6. When you hover the cursor over the object in error (not the wiggly line), a message describing the error condition will appear.

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

1. Make the schematic sheet the active document.
2. Undo the delete action (Ctrl+Z) to restore the deleted wire.
3. To check that there are no longer any errors, recompile the project (Project » Recompile PCB Project Multivibrator.PrjPcb); the Messages panel should show no errors.
4. Save the schematic and the project file, as well.

5. The final step is to commit the project file and the schematic to the Version Control repository (Project » Version Control » Commit Whole Project). The Commit to Version Control dialog will open. Confirm that the project file and the schematic are enabled. It is not necessary to commit the PrjPcbStructure file. Click the Commit and Push button in the dialog.

1. A new PCB can be added to the project via the Projects panel right-click menu. Select the Add New to Project » PCB command.

Add a new PCB to your project.

2. The PCB will appear as a Source Document in the Project as shown in the larger image above. Right-click on the PCB icon in the Projects panel to select the Save As command and name it Multivibrator. 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, so also save the project (right-click on the project filename in the Projects panel and select Save).

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 and press PgUp until both the Coarse and Fine grids are visible as shown in the images below.
2. To set the Relative Origin, select Edit » Origin » Set then position the cursor over the bottom left corner of the board shape, then left click to locate 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, as discussed in the table above. 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. For this tutorial, you will be using a Metric grid. A coarse 5mm grid will be suitable for component placement. Press Ctrl+Shift+G to open the Snap Grid dialog and enter 5mm, then click OK to close the dialog.
4. By entering the units as you entered a value, you have also instructed the software to switch to a Metric grid. Look at the Status bar to confirm that the Grid is now metric.

1. The default board shape is 6x4 inch; for the tutorial the board size is 30mm x 30mm. 
2. To zoom back out and show all of the board, select View » Fit Board from the main menus (Ctrl+PgDn).
3. The board will exactly fill the PCB editor. To manipulate the size you need to be able to see the edges of the board, use Ctrl+WheelRoll to zoom out a bit more or press PgDn.
4. The next step is to change the board shape. This is done in Board Planning view Mode. Select View » Board Planning Mode from the main menus to change it (shortcut: 1). The display will change; the board area will now be shown in green.
5. 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 Design » Edit Board Shape from the menus. Note that you must be in Board Planning Mode for this command to be available.

For this design, it is more efficient to edit the existing board shape. These commands are only available in Board Planning Mode.

6. Editing handles will appear at each corner and the center of each edge as shown below.

7. 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; these can be used as a guide. You can now either: slide the upper edge down and slide the right edge to the left to create the correct size; or move three of the corners in, leaving the one that is at the origin in its current location.
8. To slide the upper edge down, position the cursor over the edge (but not over a handle). 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, as shown in the animation below.
9. Repeat the process to move the right-hand edge in, positioning it when the X cursor location is 30mm on the Status bar.

The resize cursor is shown, use the location information on the Status bar to help you as you drag the upper and right edges to resize the board to 30mm x 30mm.

10. Click anywhere in the workspace to drop out of board shape editing mode.
11. Press the 2 shortcut to switch back to 2D Layout Mode.
12. Now that the shape has been defined, you can set the grid to a value suitable for component placement, for example, 1mm. Grids are discussed in detail shortly.
13. Save the board.

► Learn more about Defining the Board Shape

1. To configure the default settings for the designator and comment strings, select Tools » Preferences to open the Preferences dialog, then open the PCB Editor - Defaults page.
2. Select Designator in the Primitive List; the default Properties will be displayed. Confirm that the:
   • Autoposition option is set to Left-Above for the Designator. This is the default location in which this string is held when the component is rotated. The string can be interactively relocated at any time during the design process.
   • Font Type is set to TrueType, and the Font is set to Arial. Stroke fonts are Gerber-friendly shapes that the software can generate. TrueType gives access to all fonts available on the PC, but the font must be embedded in the PCB file if the board is to be opened on a PC that does not have that font installed (PCB Editor - True Type Fonts Preferences page).
   • Text Height is set to 1.5mm for this tutorial.
3.  Select Comment in the Primitive List and confirm that the:
   • Autoposition option is set to Left-Below.
   • Font Type is set to TrueType and the Font is set to Arial.
   • Text Height is set to 1.5mm for this tutorial.
   • Comment visibility is set to hidden (  ). This is a common default; component Comment strings can be selectively displayed during the design process, if required.
4. Click OK to close the dialog.

1. Make the schematic document, Multivibrator.SchDoc, the active document.
2. Select Design » Update PCB Document Multivibrator.PcbDoc from the Schematic editor menus. 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. If all changes are validated, click on Execute Changes to send the changes to the PCB editor. As each change is performed, a check will appear in the Done column of the dialog.
5. When all changes have been completed, the PCB will open behind the Engineering Change Order dialog; click to Close the dialog.
6. The components will have been positioned outside of the board, ready for placing on the board. There are a few steps to complete before starting the component placement process, such as configuring the placement grid, the layers and the design rules.

1. Open the View Configuration panel.
2. In the Layers and Colors tab, confirm that the Top Layer and Bottom Layer signal layers are visible.
3. Note that this panel is where you control the display of the mask and silkscreen layers, as well as 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, Solder and Paste Mask Layers, and the Drill Guide and Drill Drawing layers.
5. Switch to the View Options tab.
6. Confirm that the Pad Nets and Pad Numbers options are enabled.

1. Open the Layer Stack Manager. For a new board, the default stack comprises: a dielectric core, two copper layers, and the top and bottom soldermask (coverlay) and overlay (silkscreen) layers, as shown in the image above.
2. To simplify the management of layers, enable the Stack Symmetry option in the Properties panel (as shown in the image above). With this option enabled, layers are added in matching pairs, centered around the mid-dielectric layer.
3. New layers are added (above or below the current layer) via the right-click menu or the Edit » Add Layer submenu. 
4. To explore the entire Material Library, select Tools » Material Library.
5. To use a material for a specific layer (or pair of layers if symmetry is enabled), click the  in the Material cell for the required layer to open the Select Material dialog (shown in image above).
6. Using the image above as a guide, select a suitable material for the: Solder Mask, Signal and Core layers. Note that the Core layer has been chosen to define a suitable thickness for the finished board. Values can also be typed directly into the Layer Stack Manager.
7. Click on the Via Types tab at the bottom of the Layer Stack Manager and confirm that there is a Thru type via defined.
8. When you have finished exploring the layer stack options, Save the Stackup, then right-click on the Layer Stack Manager tab and close the Stackup.

1. Press the Ctrl+G shortcut keys to open the Cartesian Grid Editor dialog.
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 and the Coarse grid to display as darker colored lines.
4. Click OK to close the dialog.

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 First Object Matches in the top section (also referred to as the rule's scope - what you want this rule to target) with 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 First Object Matches setting is set to All. An additional rule will be added to target the power nets.
5. Edit the Width settings to be: Min Width = 0.2mm, Preferred Width = 0.25mm, Max Width = 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.

The default Routing Width design rule has been configured.

1. The next step is to add another design rule to specify the routing width for the power nets. To add and configure this rule, 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 and select New Rule to add a new Width constraint rule, as shown in the animation below.
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_Power in the field.
5. Click in the drop-down in the Where The Object Matches section and select Custom Query from the list. The dialog will change to include an edit box where the custom query is entered.
6. Click the Query Builder button to open the Query Builder, then configure it to target objects: InNet('12V') or InNet('GND').
   • Click the Add first condition text, select Belongs to Net, then set the Condition Value to 12V.
   • Click the Add another condition text, select Belongs to Net, then set the Condition Value to GND.
   • The AND operator will have appeared between the two condition statements, click on it select OR from the dropdown.
   • Click the OK button to accept the query and return to the rules dialog.
7. 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 to allow power net routing widths in the range 0.25mm to 0.5mm, as shown below.

This Width rule targets the power nets.

8. Click Apply to save the rules and keep the dialog open.

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, this rule will be configured to define a single clearance between All objects.
3. In the Constraints region of the dialog, set the Minimum Clearance to 0.25mm, as shown in the image above.
4. Click Apply to save the rule and keep the dialog open.

1. Expand the Design Rules tree and select the default RoutingVias design rule.
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, i.e. a Via Diameter = 1mm and a Via Hole Size = 0.6mm. Set all fields (Min, Max, Preferred) to the same size.
3. Click OK to close the PCB Rules and Constraints Editor.
4. Save the PCB file.

When you create a new board, it will include default design rules that might not be needed for your design. For example, Assembly and Fabrication Testpoint type design rules are included when you create a new board, which are not needed in this design.

1. If it is not open, open the PCB Rules and Constraints Editor.
2. Click on the Testpoint category, and disable the four Testpoint type rules (clear the checkboxes in the Enabled column). If this is not done, you will get testpoint violations later in the tutorial.

1. Click the  icon located at the upper right of the application to open the Preferences dialog.
2. Open the PCB Editor - General page of the Preferences dialog. In the Editing Options section, make sure the Snap To Center option is enabled. This insures 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.

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 then 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. Check the Status bar to confirm that the Snap Grid is set to 1mm; press Ctrl+Shift+G to change the grid if required.
3. The components in the tutorial can be placed as shown in the image above. To place connector P1, position the cursor over the middle of the outline of the connector and Click-and-Hold the left mouse button. The cursor will change to a cross hair and jump to the reference point for the part (or the center of the nearest pad if you have enabled the Smart Component Snap option). While continuing to hold down the mouse button, move the mouse to drag the component.
4. Press the Spacebar to rotate the component if required, and position the footprint towards the left-hand side of the board 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 and press the Spacebar to rotate it.
8. The PCB editor also includes interactive placement tools. These can be used 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. The Selection color is defined in the System Colors section of the View Configuration panel.
10. Right-click on any of the selected components and choose Align » Align to open the Align Objects dialog.
11. Select Space Equally in the Horizontal section and Bottom in the Vertical section, then click OK to apply these changes. The four resistors are now aligned (with the lowest component) and equally spaced.

 
Select then align and space the resistors.

12. Click elsewhere in the design window to de-select all the resistors. If required, you can also align the capacitors and transistors, although this might not be required since you have a coarse Snap grid at the moment.
13. Save the PCB file.

1. Set the Routing Conflict Resolution Current Mode to Stop at First Obstacle. As you are routing, you can cycle through the enabled modes by pressing Shift+R.
2. In the Interactive Routing Options section of the page, confirm that the Automatically Terminate Routing and the Automatically Remove Loops options are enabled. The first option releases the cursor from the current route when you click on the destination pad to finish that route. The second option allows you to change existing routing by routing an alternate path - 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. This feature will be explored later in the tutorial.
3. Confirm that the Interactive Routing Width / Via Size Sources options are both set to Rule Preferred.
4. Press Ctrl+Shift+G to open the Snap Grid dialog and set the Snap Grid to 0.25mm.

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 Configuration panel, 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, ready to route on.
3. It is often easier to route in single layer mode; press Shift+S to cycle through the enabled single layer modes.
4. Click   on the Active Bar (or the Ctrl+W shortcut), or select Interactive Routing from the Route menu, or right-click and 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 P1. 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 Hotspots feature pulling the cursor to the center of the nearest electrical object (configure the Snap Distance in the Snap Options section of the Properties panel). Sometimes the Snap To Object Hotspots feature pulls the cursor when you don't want it to. In this situation, press the Ctrl key to temporarily inhibit this feature. Alternatively, use the Shift+E shortcut to cycle through the three possible states (All Layers / Current Layer / Off). The current mode is displayed on the Status bar.
6. Left-Click or press Enter to anchor the first point of the track.
7. Move the cursor toward the bottom pad of the resistor R1, and 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, unless the next click will complete the route. In this situation, the Automatically Terminate Routing option kicks in and overrides the default look-ahead behavior. The look-ahead mode can be toggled on/off using the 1 shortcut during routing.

 
Solid segments are placed, hatched are proposed but not committed, hollow is the look-ahead segment. Press the 1 shortcut to toggle look-ahead on/off.

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 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 ways:
   • It takes the shortest path, which may not the best path as 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 as the routing path is mapped section by section, and complete mapping between source and target pads may not be possible.
   • You can also Auto-complete (Ctrl+Left Click) directly on a pad or connection line.
10. Continue to route all the connections on the board. The animation above shows the board being interactively routed.
11. There is no single solution to routing a board, so it is inevitable that you will want to change the routing. The PCB editor includes features and tools to help with this; they are discussed in the following sections and are also demonstrated in the animation shown above.
12. Save the design when you are finished routing.

Shortcut Icon	Action
	Keyboard key combination, press Ctrl+W to start Interactive Routing.
	Key + mouse combination, press Ctrl+LeftClick to auto-complete the current connection. Only functions during Interactive Routing.
	Mouse left click and drag, use this to drag an existing route. Can be used when no other command is being run.

1. Open the PCB ActiveRoute panel ( » PCB ActiveRoute).
2. Open the PCB panel.
3. Select Nets mode in the drop-down at the top of the panel, and enable the Select checkbox.
4. Unroute the board (Route » Unroute » All).
5. In the list of nets in the panel, click on the 12V net name.
6. In the PCB ActiveRoute panel, enable the Top Layer.
7. Click the ActiveRoute button at the top of the panel; the 12V net will be routed.
8. Click on the GND net in the PCB panel, then click the ActiveRoute button. If you would like to use the Shift+A shortcut to ActiveRoute, you must click once on the workspace after using a panel. This makes the workspace the active element in the software, otherwise the software will attempt to interpret the shortcut as a panel instruction.
9. Click on the net NetC1_2 in the panel, and click the ActiveRoute button.
10. Click on the net NetC2_1 in the panel, and click the ActiveRoute button.
11. Click on the net NetC2_2 in the panel, and click the ActiveRoute button.
12. Click on the net NetC1_1 in the panel, and click the ActiveRoute button. One of the connections in the net will route, the other will not. It does not route because the default pattern of connection lines is not correct for the possible routing solution, i.e. the connection line is between Q1-2 and C1-1, but the potential route path is between Q1-2 and R1-2. While it is possible to rearrange the connection lines by defining manual From-Tos, a simpler approach is to encourage ActiveRoute to attempt a different pattern by routing a stub from both Q1-2 and R1-2, so that the shortest distance between the unrouted points on this net is between these two stubs (show me).
13. Click on the net NetC1_1 in the panel, and click the ActiveRoute button; this connection should now route.

The ActiveRoute results

1. Select  » View Configuration (shortcut: L) and confirm that the DRC Error visibility option (System Colors section) is enabled so that DRC error markers are 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, and 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 and select Show Violation Details - Used, then right-click again and select Show Violation Overlay - Used, as shown in the dialog image above.
5. You are now ready to check the design for errors.

To resolve this violation you can:

1. Increase the solder mask opening to completely remove the mask between the transistor pads, or
2. Decrease the minimum acceptable sliver width, or
3. Decrease the mask opening to widen the sliver to an acceptable width.

This is a design decision that would be made in light of your knowledge of the component and the fabrication and assembly technology that is going to be used. Opening the mask to completely remove the sliver of mask between the transistor pads means that there is more chance of creating solder bridges between those pads, whereas decreasing the mask opening will still leave a sliver, which may or may not be acceptable, and will also introduce the possibility of mask-to-pad registration problems.

For this tutorial, you will do a combination of the second and third options, decreasing the minimum sliver width to a value suitable for the settings being used on this board, and also decreasing the mask expansion, but only for the transistor pads.

1. The first step is to reduce the allowable sliver width. To do this, open the PCB Rules and Constraints Editor, then in the Manufacturing section locate and select the existing Minimum Solder Mask Sliver rule, called MinimumSolderMaskSliver.
2. A value equal to the pad separation of 0.22mm ( ≈ 8.7mil) will be acceptable for a design such as this; edit the Minimum Solder Mask Sliver value to be 0.22mm in the Constraints region of the rule.

3. The next step is to add a mask expansion rule for just the transistors that reduces the mask expansion to zero. Doing this will mean that the opening in the solder mask is the same size as the pad, making the width of solder mask sliver between the pads equal to the separation distance between the pads (0.22mm). Click on Mask in the tree on the left of the PCB Rules and Constraints Editor panel to show the current Solder Mask Expansion rules; there should be one rule called SolderMaskExpansion.
4. Click on it to select the rule and display its settings; it will specify an expansion value of 0.102mm (4mil). Since it is only the transistor pads that are in violation, you will not edit this value; instead you will create a new rule.
5. To add a new Solder Mask Expansion rule, right-click on the existing rule and select New Rule from the context menu. A new rule called SolderMaskExpansion_1 will be created; click on it to display its settings.
6. Edit the rule settings to be as shown below:

• Name - SolderMaskExpansion_Transistor
• Where the Object Matches - Footprint ONSC-TO-92-3-29-11 (the name of the transistor footprint)
• Expansion top / bottom - 0mm

7. Click Apply to accept the changes and keep the PCB Rules and Constraints Editor open.

The function of this rule is to ensure there is sufficient separation between the silkscreen objects and the copper. This requirement can fail if there is a silkscreen object close to an opening in the solder mask, for example, at a pad. The rule supports checking against the opening in the mask, or checking against the copper exposed by that opening in the mask.

1. For this violation, the actual measurement is close to the current rule setting, 0.175mm versus 0.25mm, as can be seen in the Messages or the PCB Rules and Violations panel. The value 0.175mm is still an acceptable separation; edit the constraint value, as shown in the image below.

Edit the clearance to be 0.175mm.

2. Click OK to accept the changes and close the PCB Rules and Constraints Editor.

The OutputJob file, or OutJob, maps each output (in the list on the left) to an output container (in the column on the right). The output setting defines what you want to output (double-click to configure); the container defines where the output is to be written to (double-click the icon, or click the Change link). Any number of outputs can be added in the OutJob, and outputs can be mapped to individual or shared output containers.

1. In the Projects panel, right click on the project name and select Add New to Project » Output Job File. A new OutJob will be opened and added to the project.
2. Save the OutJob and name it Multivibrator. It will automatically be saved in the same folder as the project file.
3. To add a new Gerber output, click the  link in the Fabrication Outputs section of the OutJob and select Gerber » [PCB Document] as shown in the image below. If you select the [PCB Document] option, the project PCB is automatically chosen. Choosing this also means the OutJob can easily be copied between projects, as this setting will not have to be updated. If there are multiple PCBs in the project, you will need to select the specific board.
4. The Gerber output has been added; you will configure it shortly.

1. In the OutJob, double-click on the Gerber Files output added in the previous set of steps. 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: the NC drill file must always be configured to use the same Units and Format. 
4. Switch to the Layers tab then click the Plot Layers button and 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 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 section of the dialog.
5. Click 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 Units, Format and Position on Film settings as the Gerber files otherwise the drill locations will not match the pad locations!
6. Click OK to accept the other default settings and close the Gerber Setup dialog.
7. Now that the Gerber settings are configured, the next step is to configure their naming and output location. This is done by mapping them to an Output Container on the right side of the OutJob. For discrete files with their own file format, use a Folder Structure container. Select Folder Structure in the list of Output Containers then click the radio button for the Gerber Files in the Enabled column of the Outputs to map this output to the selected container, as shown below.

The OutJob configured to generate Gerber, NC Drill and Pick and Place output as discrete files.

8. The last step is to configure the container. To do this, click the Change link in the container to open the Folder Structure Settings dialog. Across the top are a set of controls that are used to configure if the outputs are Release Managed or Manually Managed; set them to Manually Managed. Explore the other options. The lower part of the dialog will display how the names and folder structure changes as you select different options.  
9. Click the Advanced button at the bottom of the Folder Structure settings dialog and enable the Gerber Output in the list of CAMtastic Auto-Load Options. Click OK to close the dialog.
10. To generate the Gerber files, click the Generate Content link in the Container region of the OutJob.
11. The files will be generated and opened in the integrated CAM editor, which can be used for final checking of CAM files before you release them to manufacture. Close the CAM file without saving it.
12. Save and close the OutputJob file.

To include a BomDoc in the tutorial:

1. Select File » New » ActiveBOM Document from the main menus. Note that a PCB project can only include one BomDoc.
2. The BomDoc will be created, and the components used in the tutorial listed as BOM Items. The BomDoc is configured in the Properties panel, where the production quantity and currency, supply chain, and visible BOM Item parameters are defined, along with other settings. Take some time to familiarize yourself with the features available in the Properties panel's two tabs. Note that the panel includes a search field at the top, which is handy for quickly locating a control or a parameter.
3. Explore the Columns tab of the panel. Note that the available data to included in the BOM can be sourced from various locations, controlled by the Sources buttons.
4. The components are detailed in the main grid area of the BomDoc. By default, there is a column titled Line #. Click the Set Line Numbers button ( ) to populate this column.
5. Because the components were placed from the Manufacturer Part Search panel, each part already includes supply chain information. When you click on a part in the BOM Items grid, its supply chain information is displayed in the lower region of the BomDoc as shown in the image above. Each row displayed in this lower region of the BomDoc is referred to as a Solution, with the manufacturer part + part number (referred to as an MPN) shown on the left, and available suppliers + supplier part numbers (referred to as SPNs) are shown in each tile on the right.
6. Note that the BOM Items grid includes a Status column on the right. Hover the mouse cursor over a status icon for information about any issues detected.
7. The Status icons should indicate that all of the Items include the error no MPN ranked. This means that the designer (you) has not yet checked through the selected parts (MPNs) and indicated that they are happy with each of them. An MPN is accepted by assigning it a rank (as shown in the image above). Do this for each of the Items that show no other error type. It is possible that the transistor may have other errors; this will be resolved shortly.
8. The Status of four of the five BOM Items should change to green (  ) indicating that these Items are clear (ready to order).
9. The status of each item is checked against the current configuration of BOM Checks configured in the Properties panel. The BOM Checks list in the panel details all BOM checks that are currently being violated. The available BOM checks and their current settings are configured in the Bom Checks dialog. click the  icon below the BOM Checks list to open the dialog.
10. Select the transistor Item; it may be flagged as Not Recommended For New Designs (NRFND). For an Item that does not have an MPN assigned, or has an MPN but that part has no suppliers, you can also create a Manufacturer Link.

11. To add a Manufacturer Link, select the transistor in the grid, click the Add Solution button and select Create/Edit Manufacturer Links from the menu that appears.
12. The Edit Manufacturer Links dialog will open. Click the Add button to add a new Manufacturer Link; the Add Part Choices dialog will open. This dialog is used to search for a suitable manufacturer part. As well as identifying a suitable part, you can also check the suppliers, price and availability.

13. If the search only returns the same part you already have used, try broadening the search, for example, search for BC547C.
14. Keep an eye on the vertical colored bar at the edge of the Manufacturer Part column. This indicates the Lifecycle state of that part. Ideally you will select a part with a green Lifecycle state (Volume Production). Note that you do not need the part to have models since you already have a symbol on the schematic and a footprint on the PCB.
15. Choose a part that has a Lifecycle state of Volume Production (hover the cursor over the vertical colored bar to view the lifecycle state) and stock available, then click OK to accept this part.
16. You will return to the Edit Manufacturer Links dialog. Click OK to close the dialog and return to the BomDoc.
17. The Solutions region of the BomDoc will show two solutions: the original part used in the design, and the Solution you just added. The Solutions are listed in the order they will be used in the BOM. Use the Ranking feature to promote the part you selected to be the primary Solution by hovering over the stars then clicking the desired rank (as shown below).
18. All parts now include supply chain details. Save the BomDoc and save the project. You are now ready to generate a BOM.

Create a Manufacturer Link to select a part directly in the BomDoc when the schematic part does not include suitable supply chain details.