Tutorial - Capturing the Schematic in Altium NEXUS

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.