Tutorial - Capturing the Schematic in Altium Designer

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.
2. Other options on this tab can be left at their default states.

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 project 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.

To include a BomDoc in the tutorial:

1. Right-click on the project filename in the Projects panel then select Add New to Project » ActiveBOM. Note that a project can only include one BomDoc.
2. The ActiveBOM document will appear as a Source Document in the Projects panel. Right-click on the document entry 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. 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.
4. 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.
5. 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).
6. Because the components were saved 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.
7. 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.
8. 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.
9. The Status of four of the five BOM Items should change to green () indicating that these Items are clear (ready to order).
10. 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).

11. 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.
12. To add a Manufacturer Link, select the transistor in the grid, click the Add Solution button and select Create/Edit Manufacturer Links from the drop-down menu.

13. 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 in the same way as the Manufacturer Part Search panel. 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.
14. If the search only returns the same part you already have used, try broadening the search, for example, search for BC547C.
15. 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.

16. 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.
17. You will return to the Edit Manufacturer Links dialog. Click OK to close the dialog and return to the BomDoc.
18. 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).

19. All parts now include supply chain details. Save the BomDoc and the project locally.

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

20. Save the project 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.BomDoc files are checked in the Save to Server dialog that opens, enter a comment into the Comment field (e.g., BOM document added), then click the  OK button.