完結された設計のチュートリアル

1. Connect to your Workspace if not already.
2. Select File » New » Project from the main menus.

3. The Create Project dialog will open:

   1. Select the required Workspace in the list of Locations. In the image above, the Workspace is named Company Workspace.
   2. Confirm that the Project Type is PCB <Empty>.
   3. Enter a suitable name in the Project Name field, e.g. Multivibrator.
   4. Enter a suitable description in the Description field, e.g. Simple multivibrator design for the tutorial.
   5. Click the Advanced control. The Folder field defines the name of the folder in the Workspace where your project files are to be stored. The default is to have a Projects folder in the Workspace.
   6. 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.
4. Click Create to close the dialog and create the project. This will take a few moments, as the project is created in the Workspace and the working folder (as specified in the Local Storage field).
5. The new project will appear in the Projects panel. If this panel is not displayed, click the button at the bottom right of the design space, and select Project from the menu that appears.
6. The project will display a small blue cross next to its name. This indicates that it has been added to the Workspace's version control system (VCS) but is yet to be committed (saved). To commit the project, click the Save to Server control next to the project name in the Projects panel.

7. The Save to Server dialog will open. Confirm that the file Multivibrator.PrjPcb is checked. Add a meaningful comment describing the change into the Comment field (e.g., Initial saving of the new PCB project), then click the OK button. A status dialog will open 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 which means that the local working copy of the project file and its counterpart in the Workspace are fully synchronized.

   Document entries in the Projects panel are accompanied by icons that indicate their open/modified/version control status. This provides a quick visual summary of which documents are modified, saved, and their version control status. Some document icons that you might encounter when working on this tutorial project and their meanings are listed below.

   	Open	The document is open as a tabbed document in the design editor window.
   	Open and locally modified	The document is open and has been modified (yet to be saved locally).
   	No modification	The local copy of the file matches the file in the Workspace and is up to date.
   	Scheduled for Addition	A file has been added to version control but not yet committed to the Workspace's VCS repository.
   	Modified	The local copy of the file has been modified and saved to the working folder but not yet committed to the Workspace's VCS repository.

   To learn more about available document display icons, see the Document Display Icons section of the Projects panel page.

1. Right-click on the project filename in the Projects panel then select Add New to Project » Schematic, as shown in the image above.
2. The Select configuration item dialog will open. Select a schematic template from those that are stored in your Workspace (e.g. ANSI B Landscape) and click the OK button. A blank schematic sheet named Sheet1.SchDoc will open in the design space and an entry for this schematic will appear linked to the project in the Projects panel under the Source Documents folder icon.
3. To save the new schematic sheet locally, select File » Save As from the main menus (or use the Save As from the schematic's right-click menu in the Projects panel). 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, as it will be added automatically). 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.
4. 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 locally.
5. Save the new schematic and the modified project file to the Workspace. To do this, click the Save to Server control next to the project name in the Projects panel.
6. The Save to Server dialog will open. Confirm that the Multivibrator.PrjPcb and Multivibrator.SchDoc files are checked. Add a meaningful comment describing the change into the Comment field (e.g., A new blank schematic sheet added), then click the OK button. A status dialog will open while the files are written to the Workspace. 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 design space), 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 design space).

1. If the Properties panel is not visible, click the button at the bottom right of the application window and select Properties from the menu that opens.
2. The General tab of the Properties panel in its Document Options mode (when nothing is selected) 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 the Snap and Visible Grids, set the 100mil value.
4. To make the document fill the viewing area, select View » Fit Document (shortcut: V, D).
5. Save the schematic locally – right-click the schematic in the Projects panel and select Save.

• 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 the 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 enabled Filters list are detailed just below the search bar. Click the small x icon to remove any of the existing search criteria. Note that the contents of the Filters search box apply to these results too, so if it has not been cleared, you will only be able to remove the search criteria that was last entered into the search box. Clear the search box to resolve this.

  

• 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 for configuring column order and visibility.

  

• 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.

• The icon indicates that there are models available for this part. Click the button at the top right of the panel to display detailed part information, including the models.
• 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 are 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 Octopart website).
3. Country code for the Supplier location (ISO alpha 2).

4. Source of the part information (typically the Altium Parts Provider). Color indicates:

   • Light Gray = Default, updated less than one week ago
   • Orange = 1 week < last update < month ago
   • Red = last update > 1 month ago
5. Stock quantity: red if no stock available.
6. Unit price: red if no price available. Unit price is shown in currency configured in the panel settings ().
7. Packaging of supplied parts; hover for details.
8. Available price breaks with Minimum Order Quantities.

1. Open the Manufacturer Part Search panel if not already – click the button at the bottom right of the application window and select Manufacturer Part Search from the menu.

2. Use panel's Search field to search for: transistor BC547.

   

3. Click the ON Semiconductor BC547CG transistor to select it in the results grid in the panel.

4. To explore the availability of a component, select it in the results grid in the panel then click the SPN link that appears.

   

5. Display the Component Details pane of the panel using the button (or using the button at the bottom of the panel if the panel is in its compact mode) 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.
6. When the required transistor is selected in the panel, click the Download drop-down in the top region of the Component Details pane and select Acquire.

7. In the Create new component dialog that opens, select the Transistors component type and click OK.

   

8. In the Use Component Data dialog that opens, disable the Only matching option at the top-right of the dialog and enable Parameters, Symbols, Footprints, and Datasheets options, then click OK.

   

9. The Single Component Editor will open, with the chosen data loaded. Leave the data values at their defaults and select the File » Save to Server command from the main menus.

   

10. In the Edit Revision for Item dialog that opens, type in a meaningful comment to the Component Item Revision release into the Release Notes field (e.g., Initial release of the transistor component, acquired from Manufacturer Part Search), then click OK. A status dialog will open while the component is saved to the Workspace. When this is complete, the Component Editor will close.

1. Return to the Manufacturer Part Search panel and use the panel's Search field to search for: capacitor 22nF 16V 0603.
2. Select the KEMET C0603C223J4RACTU capacitor in the search result grid, right-click on it then select Acquire from the context menu.
3. In the Create new component dialog that opens, select the Capacitors component type and click OK.
4. In the Use Component Data dialog that opens, disable the Only matching option at the top-right of the dialog and enable Parameters, Symbols, Footprints, and Datasheets options, then click OK.

5. The Single Component Editor will open, with the chosen data loaded. In the Name field in the Component region at the top-left of the editor, change the component name to Capacitor 22nF +/-5% 16V 0603.

   

6. Leave other data values at their defaults and select the File » Save to Server command from the main menus.
7. In the Edit Revision for Item dialog that opens, type in a meaningful comment to the Component Item Revision release into the Release Notes field (e.g., Initial release of the capacitor component, acquired from Manufacturer Part Search), then click OK. A status dialog will open while the component is saved to the Workspace. When this is complete, the Component Editor will close.

1. Return to the Manufacturer Part Search panel, search for: resistor 100K 5% 0805.
2. Select the Panasonic ERJ-6GEYJ104V resistors in the search result grid, right-click on it then select Acquire from the context menu.
3. In the Create new component dialog that opens, select the Resistors component type and click OK.
4. In the Use Component Data dialog that opens, disable the Only matching option at the top-right of the dialog and enable Parameters, Symbols, Footprints, and Datasheets options, then click OK.
5. The Single Component Editor will open, with the chosen data loaded. In the Name field in the Component region at the top-left of the editor, change the component name to Resistor 100K +/-5% 0805 125 mW.
6. Leave other data values at their defaults and select the File » Save to Server command from the main menus.
7. In the Edit Revision for Item dialog that opens, type in a meaningful comment to the Component Item Revision release into the Release Notes field (e.g., Initial release of the resistor component, acquired from Manufacturer Part Search), then click OK. A status dialog will open while the component is saved to the Workspace. When this is complete, the Component Editor will close.
8. Return to the Manufacturer Part Search panel, search for: resistor 1K 5% 0805.
9. Select the Panasonic ERJ-P06J102V resistor in the search result grid, right-click on it then select Acquire from the context menu.
10. In the Create new component dialog that opens, select the Resistors component type and click OK.
11. In the Use Component Data dialog that opens, disable the Only matching option at the top-right of the dialog and enable Parameters, Symbols, Footprints, and Datasheets options, then click OK.
12. The Single Component Editor will open, with the chosen data loaded. In the Name field in the Component region at the top-left of the editor, change the component name to Resistor 1K +/-5% 0805 500 mW.
13. Leave other data values at their defaults and select the File » Save to Server command from the main menus.
14. In the Edit Revision for Item dialog that opens, type in a meaningful comment to the Component Item Revision release into the Release Notes field (e.g., Initial release of the resistor component, acquired from Manufacturer Part Search), then click OK. A status dialog will open while the component is saved to the Workspace. When this is complete, the Component Editor will close.

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 the All » Connectors category.
3. Click the Filters button () to display the Filters pane.
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 of the Filters pane. 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:

   Search for	Choose
   has model	Has Model: Yes
   contacts	Number of Contacts: 2
   pitch	Terminal Pitch: 2.54mm
   male	Contact Gender: Male
   straight	Mounting Style: STRAIGHT

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

   

7. In the Create new component dialog that opens, select the Connectors component type and click OK.
8. In the Use Component Data dialog that opens, disable the Only matching option at the top-right of the dialog and enable Parameters, Symbols, Footprints, and Datasheets options, then click OK.
9. The Single Component Editor will open, with the chosen data loaded. Leave the data values at their defaults and select the File » Save to Server command from the main menus.
10. In the Edit Revision for Item dialog that opens, type in a meaningful comment to the Component Item Revision release into the Release Notes field (e.g., Initial release of the connector component, acquired from Manufacturer Part Search), then click OK. A status dialog will open while the component is saved to the Workspace. When this is complete, the Component Editor will close.

1. Select View » Fit Document from the main menus (shortcut: V, D) to ensure your schematic sheet takes up the full editing window.
2. Open the Components panel if not already – click the button at the bottom right of the application window and select Components from the menu.
3. Click the button at the top of the Components panel and select Refresh from the menu to update the panel's content with the components acquired from Manufacturer Part Search.

4. Use panel's Search field to search for: transistor BC547.

   

5. Display the Component Details pane of the panel using the button (or using the button at the bottom of the panel when the panel is in its compact mode) so that you can explore the properties and models of the selected component.

6. Click to select the required transistor in the results grid in the panel then click the Place button (as shown below). The cursor will change to a crosshair and you will have a symbol 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!

   

7. 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.

8. In the Properties section of the panel, type in the Designator Q1.
9. Confirm that the visibility control for the Comment field is set to visible ().
10. Leave all other fields at their default values then click the Pause button ( ) to return to part placement.
11. 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 window. It is 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.
12. Once you are happy with the transistor's location, click the left mouse button or press Enter on the keyboard to place the transistor onto the schematic. The location can be changed later if required.
13. 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 symbol floating on the cursor. This feature allows you to place multiple parts of the same type.
14. 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.
15. 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.
16. 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.
17. Once you have positioned the part, click the click the left mouse button 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.
18. 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 Components panel and search for: capacitor 22nF 16V 0603.
2. Select the found capacitor in the search result grid, right-click on it then 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 General section of the panel, type in the Designator C1.

5. Expand the Parameters section of the Properties panel and open the Value drop-down of the Footprint entry. Many of the resistors and capacitors have several footprint models, for different density levels. Select the A variety as shown in the image below.

   

6. Using visibility controls in the Parameters section of the panel, enable the visibility of the Capacitance parameter and disable the visibility of other parameters. Value of the Capacitance parameter will be shown next to the component in the design space.

   Click the Show More link in the panel's Parameters region to show the full list of component parameters.
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 the part placement mode.

1. In the Components panel, search for: resistor 100K 5% 0805.
2. Select the found 100K resistor in the search result grid and display the footprint in the Models section of the panel.
3. Many of the resistors and capacitors have several footprint models, for different density levels. 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 General section of the panel, type in the Designator R1.
7. In the Parameters section of the panel, enable the visibility of the Resistance parameter and disable the visibility of other parameters.
8. 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.
9. Press the Spacebar to rotate the component in 90° increments until it has the correct orientation.
10. 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.
11. 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.
12. Exit part placement mode by clicking the right mouse button or pressing the Esc key. The cursor will revert back to a standard arrow.
13. The remaining two resistors, R3 and R4, have a value of 1K; search for: resistor 1K 5% 0805 fixed in the Components panel.
14. Select the found 1K resistor in the search result grid and display the footprint in the Models section of the panel.
15. Many of the resistors and capacitors have several footprint models, for different density levels. Select the M variety.
16. Right-click on the resistor in the search results grid and select Place from the context menu.
17. While the resistor is floating on the cursor, press the Tab key to open the Properties panel.
18. In the General section of the panel, type in the Designator R3.
19. In the Parameters section of the panel, enable the visibility of the Resistance parameter and disable the visibility of other parameters.
20. 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.
21. Press the Spacebar to rotate the component in 90° increments until it has the correct orientation.
22. 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.
23. Right-click or press Esc to exit part placement mode.

1. Return to the Components panel and search for: connector male straight.
2. Select the found connector in the search result grid, right-click on it then select Place from the context menu.
3. While the header is floating on the cursor, press Tab to open the Properties panel and set the Designator to P1.
4. Click the Pause button to return to part placement.
5. 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.
6. Right-click or press Esc to exit part placement mode.
7. Save your schematic locally.

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 crosshair.
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 crosshair 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. Select the Net Label command (choose the icon in the Active Bar, or select the Place » Net Label from the main menus). A net label will appear floating on the cursor.
2. To edit the net label before it is placed, press Tab to open the Properties panel.
3. Type 12V in the Net Name 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 uppermost 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 (the first image) and positioned over a wire (the second 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 locally – right-click each file in the Projects panel and select Save.

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.

• 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 validate the Multivibrator project, select Project » Validate PCB Project Multivibrator.PrjPcb from the main menus.
2. When the validation is complete, all warnings and errors are displayed in the Messages panel. The panel will only open 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 validate the project again:

1. Click on the Multivibrator.SchDoc tab at the top of the design space to make the schematic sheet the active document.
2. Click in the middle of the wire that connects P1 to the emitters wire of Q1 and Q2 (the wire of the GND net). Small, square editing handles will appear at each end of the wire and the selected 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. Validate the project again (Project » Validate 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, re-compile the project (Project » Validate PCB Project Multivibrator.PrjPcb); the Messages panel should show no errors.
4. Save the schematic and the project file to the Workspace – click the Save to Server control next to the project name in the Projects panel, confirm that the Multivibrator.PrjPcb and Multivibrator.SchDoc files are checked in the Save to Server dialog that opens, enter a comment into the Comment field (e.g., Schematic is created and validated), then click the OK button.

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 Projects panel 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 locally (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 design space, and the user-definable Relative Origin, which is used to determine the current design space 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 (the first image), then click to define the origin (the second 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. 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, you can check this on the Status Bar.

1. The default board shape is 6x4 inches; for this tutorial, you will change the board size to 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+Mouse Wheel 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 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 on the animation 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.
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.

   Use the current location information at the bottom left of the Status Bar to guide you as you reshape the board.

   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 design space 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 locally.

► 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 (that can be configured on the PCB Editor – True Type Fonts page of the Preferences dialog).
   • 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 save the changes and 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 to open the Engineering Change Order dialog.

   
   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 – Check column of the dialog. 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 Status – 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.

   You can create a report of the ECOs by clicking the Report Changes button.

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 Component Layer Pairs (except for Overlay layers), Mechanical 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 – select the Design » Layer Stack Manager command from the main menus. 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, make sure that the Stack Symmetry option is enabled 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. 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 the image above).
4. Using the image above as a guide, select 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.
5. Click on the Via Types tab at the bottom of the Layer Stack Manager and confirm that there is a Thru type via defined.
6. When you have finished exploring the layer stack options, save the stackup (File » Save to PCB), 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. Make sure that the Step X field has the value 1mm. 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 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 dialog if not already.
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 dropdown 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 dialog, 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. 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 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 Routing category in the tree of Design Rules then expand the Routing Via Style rule-type 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 save the changes and close the PCB Rules and Constraints Editor dialog.
4. Save the PCB file locally.

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 top-right of the application window 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 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.
4. Click OK to save changes and close the Preferences dialog.

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 use Click, Hold&Drag. The cursor will change to a crosshair 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 space to deselect 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. Reposition component designators if needed – click, hold and drag a designator, or use the Autoposition option in the Properties panel when designator(s) are selected in the design space.
14. Save the PCB file locally.

1. Open the PCB Editor – Interactive Routing page of the Preferences dialog.
2. Set the Routing Conflict Resolution Current Mode to Walkaround Obstacles. As you are routing, you can cycle through the enabled modes by pressing Shift+R.
3. 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.
4. Confirm that the Interactive Routing Width / Via Size Sources options are both set to Rule Preferred.
5. Click OK to save changes and close the Preferences dialog.
6. 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 design space. 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 design space 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 Objects for snapping feature pulling the cursor to the enabled hotspot of the nearest electrical object (configure the Snap Distance and the Objects for snapping in the Snap Options section of the Properties panel). Sometimes the Objects for snapping feature pulls the cursor when you don't want it to. In this situation, press the Ctrl key to temporarily inhibit snapping. Alternatively, use the Shift+E shortcut to cycle the Hotspot Snap mode through the three possible states – Hotspot Snap (All Layers) / Hotspot Snap (only snaps on the current layer) / Off (nothing displayed). The current mode is displayed on the Status Bar.

   ► Learn more about Working with the PCB Grids System, including object snapping.

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 R3, 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 R2. 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+Click to use the Auto-Complete function and instruct the software to attempt to 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+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.

    In the animation above, there is a route from the upper pad of R1 to the middle pin of Q1, that is placed on the bottom layer. Depending on the brand of surface mount resistor that you chose, it may be possible to place this route so that it passes between the pads of R3. For example, Panasonic resistors are slightly smaller, it will not be possible to route a track between the pads of their footprint. In this situation, you will need to route one connection on the bottom layer to complete the routing. To switch layers and place a via while routing, use the * key on the numeric keypad, or the Ctrl+Shift+Mouse Wheel shortcut combination. On the other hand, Yageo and Vishay Dale resistors are slightly larger and the pads of their footprint have sufficient space between them to route using the width and clearance configured in this design.
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 locally when you are finished routing.

    Shortcut Icon	Action
    	Keyboard key combination, press Ctrl+W to start Interactive Routing.
    	Key + mouse combination, press Ctrl+Click to auto-complete the current connection. Only functions during Interactive Routing.
    	Click, Hold&Drag, use this to drag an existing route. It can be used when no other command is being run.

• Ignore Obstacles – 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, i.e. as soon as an obstacle is encountered, the track segment will be clipped to avoid a violation.
• Walkaround Obstacles – this mode will attempt to find a routing path around existing obstacles without attempting to move them.
• Hug & Push Obstacles – this mode is a combination of Walkaround and Push. It will hug as it performs a Walkaround of obstacles, however, it will also attempt to Push against fixed obstacles when there is insufficient clearance to continue using Walkaround.
• Push Obstacles – this mode will attempt to move objects (tracks and vias), which are capable of being repositioned without violation to accommodate the new routing.
• Autoroute on Current Layer – this mode brings basic autorouting functionality to interactive routing. It can automatically select between walkaround and push based on heuristics that consider push distance versus walk distance and route length. Like an autorouter, this mode can deliver better results on a complex, busy board than on a simple, unrouted board.
• Autoroute on Multiple Layers – this mode also brings basic autorouting functionality to interactive routing, it can also automatically select between walkaround and push based on heuristics that consider push distance versus walk distance and route length. This mode can also place a via and consider using other routing layers. Like an autorouter, this mode can deliver better results on a complex, busy board than on a simple, unrouted board.

• Current design space location and Snap Grid setting
• Object Hotspot Snapping: off / on for current layer / on for all layers
• Current track corner mode
• Current Interactive Routing Mode
• Source of routing Width
• Source of routing Via Style
• Name of Via Type that will be used
• Current Gloss strength
• Name of Net
• Overall route length
• Dimensions of routing segment being placed

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 design space after using a panel. This makes the design space 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 there is not sufficient space to place this route on the top layer that has been selected. As ActiveRoute is not an autorouter, and it cannot place vias, so a fanout for C1-1 should be created.

13. Enter the Interactive Routing mode (Ctrl+W), start routing from the C1-1 pad, position the cursor at the left of the pad, and switch layer (Ctrl+Shift+Mouse Wheel) to place a via. Click to commit the route and the via, then exit the Interactive Routing mode (right-click to drop routing of the current connection, then right-click again to exit the Interactive Routing mode).

    A fanout for the capacitor.

14. Click on the net NetC1_1 in the PCB panel, enable the Bottom Layer and disable the Top Layer in the PCB ActiveRoute 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 design space. There are two different methods available for displaying violations, each with its own strengths.
4. For the tutorial, right-click in the Choose DRC Violations Display Style 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. Click OK to save changes and close the Preferences dialog. 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 dialog to show the current Solder Mask Expansion rules; there should be one rule called SolderMaskExpansion.
4. Double-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 in the tree on the left 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 – select Footprint in the drop-down, then select ONSC-TO-92-3-29-11 (the name of the transistor footprint) in the second drop-down that appears
   • Expansion top / bottom – 0mm
   
7. Click Apply to accept the changes and keep the PCB Rules and Constraints Editor open.

1. Save the PCB file locally.
2. Open the Design Rule Checker dialog (Tools » Design Rule Check) and make sure that the Create Report File option is enabled on the Report Options page.
3. Click the Run Design Rule Check button.
4. A new report will be generated and open in a separate document tab. Make sure that it does not contain any rule violations.
5. If there are violations, back to the PCB document and resolve these violations, then generate the report again.

6. Remove the generated DRC report from the project (it will be generated during the design release process) – in the Projects panel, find the report file in the Generated\Documents sub-folder, right-click on it and select the Remove from Project command. In the Remove from project dialog that opens, choose the Delete file option.

   Remove the Design Rule Check report file from the project, with the permanent delete option.

7. Save the PCB and the project to the Workspace.
8. Close the PCB file.

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 Fabrication. 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 Files » [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. Same way, add the NC Drill output to the OutJob file – click the link in the Fabrication Outputs section of the OutJob and select NC Drill Files » [PCB Document].

8. Double-click on the added NC Drill Files output to access the NC Drill Setup dialog. Set the Units to Millimeters and the Format to 4:3. Make sure that the Coordinate Position option is set to Reference to relative origin, and click OK to accept the other default settings and close the dialog.

   
   The NC Drill Setup dialog configured to generate proper NC Drill files for the tutorial.

9. Now that the Gerber and NC Drill 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 buttons for the Gerber and NC Drill Files in the Enabled column of the Outputs section to map these outputs to the selected container, as shown below.

   
   The OutJob configured to generate Gerber and NC Drill outputs as discrete files.

10. 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; make sure that they are set to Release Managed. Explore the other options. The lower part of the dialog will display how the names and folder structure change as you select different options.
11. Click OK to close the dialog.

1. To add a new Validation output, click the link in the Validation Outputs section of the OutJob and select Design Rules Check » [PCB Document].
2. Map the added report to the Folder Structure Output Container – select the Folder Structure container in the list on the right side of the OutJob, then click the radio button for the Design Rules Check output in the Enabled column of the Outputs section.
3. Save locally 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 be 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 (you may need to refresh the BomDoc with the Refresh button at the top-right of the document to show the Line # values in the grid).
5. Because the components were acquired 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 BOM 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 (accessed with the icon below the BOM Checks list).

10. Select the transistor Item; it may be flagged as Obsolete. 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.

    The Manufacturer Link feature allows you to connect a Workspace part, or a non-Workspace part with supply chain issues, to your preferred manufacturer part. Using this feature, you can bring the full power of the Altium Parts Provider to all of your design components directly in the BomDoc, complete with real-time supplier, price, and availability information. The Manufacturer Link is stored in the BomDoc.
11. To add a Manufacturer Link, select the transistor in the grid, click the Add Solution button and select Create/Edit PCL (Part Choice List) 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.

    The Search field in the Add Part Choices dialog is automatically populated with data from the component you selected in the BomDoc. The field that supplies the search data is determined by the Suggested Keywords setting in the Data Management – Part Providers page of the Preferences dialog. The default is to search using the Comment field; this can be changed if required.
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.

    Added part choices and rankings in the BomDoc are automatically saved back for the component in the Workspace.
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 to the Workspace.

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

1. Add a new OutJob file to the project and save it as Assembly in the same folder as the project file.
2. To add a new BOM output, click the link in the Report Outputs section of the OutJob and select Bill of Materials » [ActiveBOM Document].
3. Double-click on the added Bill of Materials output to open the Report Manager dialog.

4. In the Export Options of the Properties pane on the right side of the dialog, set Generic XLS (*.xls, *.xlsx, *.xlsm) for the File Format and BOM Template Single Supplier for the Template.

   Unlike the MS-Excel (*.xls, *.xlsx *.xlsm) file format, Generic XLS (*.xls, *.xlsx, *.xlsm) uses a built-in XLS-format file generator, so that this format can be generated without having Microsoft Excel installed.

   The Report Manager takes the configuration from the BomDoc if the project includes a BomDoc.

5. Click OK to save changes and close the dialog.
6. In the OutJob file, map the added BOM report to the PDF Output Container – select the PDF container in the list on the right side of the OutJob, then click the radio button for the Bill of Materials output in the Enabled column of the Outputs section.

7. Configure the PDF container – click the Change link in the container to open the PDF settings dialog. Click the Assembly.PDF entry, select the Separate file for each output using output name, and click Done. The output BOM will be assigned the name set to the output in the OutJob file (Bill of Materials.pdf), that can be seen in the Preview region of the dialog.

   Configure the BOM output naming in the PDF setting dialog.

8. Click OK to close the dialog.
9. Add the Pick & Place output to the OutJob file – click the link in the Assembly Outputs section of the OutJob and select Generates pick and place files » [PCB Document].
10. Double-click on the added Generates pick and place files output to access the Pick and Place Setup dialog. Set the Units to Metric in the Output Setting region on the bottom left part of the dialog and click OK to accept the other default settings and close the dialog.
11. Map the added Pick & Place output to the Folder Structure Output Container – select the Folder Structure container in the list on the right side of the OutJob, then click the radio button for the Generates pick and place files output in the Enabled column of the Outputs section.
12. Save the project to the Workspace.

1. Access the Release view – right-click the project file in the Project panel and select the Project Releaser command from the context menu.
2. The Release view will open as a separate document tab. On the first stage – 1. Configure Server Release (shown on the image above) – you specify the type(s) of data that you wish to generate. Click on Details controls at the far right of each data set header to access details of what exactly is going to be generated by a data set.

3. Click the Options button at the bottom-left of the view to access the Project Release Options dialog. On the dialog's Release Options tab, make sure that the Managed - <WorkspaceName> is selected as the Release Target; Fabrication is assigned to Fabrication Data set, and Assembly is assigned to the Assembly Data set. Click OK to close the dialog and get back to the Release view.

   Configure options for the online release in the Project Release Options dialog.

4. Make sure that both fabrication and assembly Data Items are included in the release – Include Fabrication Data and Include Assembly Data for No Variant options are enabled (source data are always included in the project release) – then click the button to proceed.
5. The Item Creation dialog will open, with the list of target release items to be created in the Workspace. Select the Create items option to confirm creation of the items.

6. If there are changes in the open documents that have not been saved locally, the Project Modified dialog will open. In this case, select the Save and Commit changes option to save the changes locally and proceed with saving the changes to the Workspace.

   If there are changes to the project and/or its files that have not been saved to the Workspace yet, the Pending Commits dialog will open, alerting about this fact. Select the Commit option to proceed with saving the changes to the Workspace.
7. In the Commit to Version Control dialog that opens, make sure that modified project's source files, and those that are not in version control, are enabled, enter a meaningful Comment (e.g., The project is ready to be released), and click the Commit And Push button.

8. The next stage of the release process – 2. Validate Project – is run automatically when one or more Validation-type reports are detected in assigned OutJob file(s). As the Fabrication OutJob file includes generation of the Desing Rules Check report, this validation output generator is run.

   If any validation checks are not passed successfully, the release will fail. For the project release in this tutorial, this will mean that the PCB document includes at least one DRC violation. In this case, stop the release process with the Cancel button at the bottom-right of the view, open the PCB document, resolve the DRC violations, then start the release process again.
9. If validation is successful, the next stage of the release process – 3. Generate Data – is run automatically. This is where all other outputs – defined in the OutJob file(s) assigned to the included Data Items – are run, to generate the data to be released into the relevant target items in the Workspace.

10. With all validation checks passed, and output data generated, the next stage of the release process – 4. Review Data – allows you to review the generated data. Click a View link to open the associated data file, or file set, either within the relevant editor within Altium NEXUS (e.g. the CAM editor) or within the relevant external application (e.g. a PDF viewing tool). If the generated data all looks good, proceed with the release by clicking the Release button at the bottom-right of the view.

    Review of the generated data, ready to be released to the Workspace.

11. The Confirm Release dialog will open, summarizing the configurations of the project that will be released to the Workspace. Enter a Release Note (e.g., Initial Release), and click OK.
12. After confirming the release in the previous stage, the next stage – 5. Upload Data – is automatically entered. It simply presents the progress of data upload into the revisions of the relevant data Items in the Workspace.
13. The final stage of the process – 6. Execution Report – provides a summary of the release. Close the Release view using the Close button at the bottom-right of the view.

1. To access the History view for the project from within Altium NEXUS, right-click on its entry in the Projects panel and choose the History & Version Control » Show Project History command from the context menu. The History view presents as a distinct tabbed document (Multivibrator History).
2. Explore events relating to the project: project creation (the tile at the very bottom of the timeline), project commits (saving it to the Workspace), project release (the tile at the very top of the timeline, that straddles the timeline as a 'major' event).

3. Click the control at the top-right of the view to access a search field and perform a search of events related to the R1 resistor. Enter R1 to the search field – one tile should be filtered, with the search string highlighted in the event details.

   Using the Search feature in the History view.

4. Clear the search field to clear the current filtering and return to the full timeline – click on the Clear Filter control in the box summarizing how many events are being shown (at the top of the view) or click the control at the far right of the search field.
5. Close the History view – right-click on its document tab and select the Close Multivibrator History command from the context menu.

1. To access the Web Viewer interface from within Altium NEXUS, right-click on the project entry in the Projects panel and choose the Show in Web Browser command from the context menu. The detailed management page for the project will open in your default web browser, with the Design view of the project presented.

2. The SCH data view that presents the source schematic sheet will open by default. Using view buttons at the top of the main viewing area, switch between other data views available: PCB (the board in 2D), 3D (the board in 3D), and BOM (Bill of Materials).

   
   Buttons for switching the current data view.

3. On the SCH data view, use Mouse Wheel to zoom in/out; Click, Hold&Drag (or Right-Click, Hold&Drag) to pan the document.
4. Hover the cursor over a component and click to select it and display its details in the right-hand pane.
5. Hover the cursor over a wire and click to select the net and display its details in the right-hand pane.

6. Buttons at the top of the right-hand pane allow cross-probing to the selected object on other data views. When a component or a net is selected, use these buttons to switch to another data view, with the same object selected, centered, and zoomed there. Select the 12V net on the schematic view and click the PCB button in the details pane to switch to the board data view with the net selected, centered, and zoomed.

   
   Cross-probing controls (for a selected net).

7. In the PCB data view, use Mouse Wheel to zoom in/out Click, Hold&Drag (or Right-Click, Hold&Drag) to pan the document.
8. Use the Layers pane accessed by clicking on the control at the top-left of the view (e.g. ) to control layer visibility. Use the Top View and Bottom View controls at the top of the pane to quickly toggle between viewing the board from the top or bottom respectively.
9. Switch to the 3D view. Use Mouse Wheel to zoom in/out; Click, Hold&Drag to rotate the board; Right-Click, Hold&Drag to pan the board.

10. Click the control in the top-right control cluster to access the Search facility, allowing you to search for components and/or nets. Type C1 in the search field to display the list of matching components and nets. Click NetC1_1 to select this net on the current data view.

    
    Searching for a net within the active 3D view.

11. Switch to the BOM data view. Use links in the Designator column to cross-probe to the component on the last active data view prior to accessing the BOM data view.

1. When the project is opened in the Web Viewer interface, switch to the SCH data view.
2. Click the control in the top-right control cluster to display the Comments pane where project comments are shown.
3. Click the button at the top of the Comments pane – the cursor will change to a cross-hair and you will enter comment placement mode.

4. Left-click on the C1 capacitor. A commenting window will be presented – enter a comment in the field provided and click Post. A comment marker will be presented in the main viewing area.

   
   Placing a comment in the Web Viewer interface.

5. Open the schematic sheet in Altium NEXUS. Note that the comment marker () next to the C1 capacitor. Click on it to display the commenting dialog. Double-click on it to open the Comments panel (the panel can also be opened from the button menu).

6. In the Reply field of the commenting window, enter a reply to the initial comment and click Reply.

   
   Replying to a comment.

7. Click the button at the top-right of the dialog to mark the comment as resolved (i.e. close it as complete).
8. In Altium NEXUS, open the PCB document in its 2D layout mode (shortcut: 2).
9. Click the  button at the top-right of the application window or the button in the Comments panel to enter comment placement mode.
10. Click and hold the left mouse button away from an object and drag the cursor to create a rectangular highlighted area around resistors, and then release the mouse button to confirm its final shape.

11. In the commenting dialog, click the control or enter the @ character and select a user from the dropdown list that appears. Enter a comment in the comment field, leave the Assign to option enabled and click Post. The user will be mentioned in the comment, and the comment will be assigned to this user.

    
    Comment for an area in the PCB document. A user is mentioned in the comment, and the comment is assigned to this user.

12. In the Web Viewer interface, switch to the PCB data view of the project and make sure that the comment added to the PCB in Altium NEXUS presents in the main viewing area and in the Comments pane.
13. Click the comment marker to open the commenting window and click the control at the top-right to mark the comment as resolved.

1. In Altium NEXUS, click the button at the top-right of the application window to open the Share dialog.

2. Click the Share with control to see who currently has access to the projects.

   Access the Share dialog in Altium NEXUS and check with whom the project is currently shared.

3. By default, the project is available to all members of the Workspace for viewing and commenting only – note the Everyone in the team entry and the Can View at the right. Click the Can View and select Can Edit from the drop-down – Workspace members will have editing permissions to the project.

   Change access to the project permissions from the Share dialog.

4. Click the Save button to save the changes. You can click the Who has access control to get back to the list of entities who has access to the project and make sure that the change has been applied.

   Project sharing setting can also be configured through the Workspace's browser interface. For more information, see the Server Projects – Sharing a Managed Project page.
5. Besides sharing an actual work-in-progress design within the Workspace team, you can also create and share design snapshots, i.e. design at that specific point in time of the project's development, for wider collaboration with others through the Web. To share in this manner, click to select the Snapshot on the Web entry, on the left side of the Share dialog.

6. By default, the dialog is set to Share By Link, meaning that you can generate a link and anyone who is given the link will have access to view the design snapshot through their Web browser for a time-limited period of 48 hours. Click the button to generate the link to the design snapshot.

   Generate a link to the provide a simple access to the project snapsoht on the Web.

7. Once the link is ready, click the button to copy it.

8. Open the link in your web browser – you will be taken to an instance of the Altium 365 Viewer – on the main altium.com site – with the design processed and loaded.

   Using the shared link, a recipient can browse the design snapshot using Altium 365 Viewer, loaded on the main altium.com site.

   The Share dialog also provides an ability to share a design snapshot with one or more specific people, by email invitation. Clicking the Share with specific people control on the Snapshot on the Web tab of the dialog will switch the sharing mode to allow you to do this. Recipients will have access to view, share or download the design snapshot through the Web-based Altium 365 Platform Interface. Such a design snapshot is available permanently through the platform and commenting on the design is possible with this level of sharing.