Placing and moving components in Cadence PCB Editor

While it is easy to place components using the mouse, most designs require precise placement of some components (e.g., to align parallel headers). This tutorial walks through how to place components at a specific X-Y coordinate, determine the X-Y coordinates of a component, measure the distance between two components, move an existing component to a specific X-Y coordinate, and move an existing component relative to its current location.

How do you place a component at a specific X-Y coordinate?

1. Choose Place > Manually... (see Figure 1). The Placement dialog box appears (see Figure 2).

Figure 1: Place > Manually... menu

Figure 2: Placement dialog box

2. Check the box next to the part that you want to place, but do not place it yet. Instead, go to the command line at the bottom of the screen and type the desired placement coordinates in the following format: x x-coordinate y-coordinate

Example:

Command > x 0 0 will place the component at the origin (0,0)

3. Press Enter to place the component at the desired coordinates (see Figure 3).

Figure 3: Component placed at origin (0,0)

How do you determine the current coordinates of a component?

1. Choose Display > Element (see Figure 4) and click on the component you would like to examine. The Show Element dialog box will appear and show the current coordinates of the component (see Figure 5).

Figure 4: Display > Element menu option

Figure 5: Coordinates of a placed component

How do you measure the distance between two components?

1. Choose Display > Measure (see Figure 6). The command line will ask you to "Make two picks for the distance calculator" (see Figure 7).

Figure 6: Display > Measure menu option

Figure 7: Command line message for Measure tool

2. Click parts of two components (e.g., a pin of a resistor and a pin of a capacitor). The Measure dialog box will appear and show the distance between the selected points (see Figure 8).

Figure 8: Measured distance between resistor and capacitor pins

How do you move an existing component to a specific  X-Y coordinate?

1. Right-click on the component and select "Move"

2. Use the command line to enter a specific coordinate in the x (x x-coordinate) or y (y y-coordinate) direction.

Examples:

A component is at (25,75).

Command > x 200 will move the component to (200,75) (see Figure 9)

Command > y 200 will move the component to (25, 200) (see Figure 10)

Figure 9: Moving a component to an absolute x coordinate

Figure 10: Moving a component to an absolute Y coordinate

How do you move a component relative to its current position?

1. Right-click on the component and select "Move"

2. Use the command line to enter a relative movement in one of the following formats:

ix x-units

iy y-units

ix x-units y-units

Examples:

A component is at (1000,2000).

Command > ix 200 will move the component to (1200, 2000)

Command > iy 200 will move the component to (1000, 2200)

Command > ix 200 -500 will move the component to (1200,1500) (see Figure 11)

Figure 11: Results of relative movement

Based on a tutorial by Seana O'Reilly

Printing a PCB Layout in Cadence PCB Editor

Note: This tutorial shows how to print a PCB design on paper. Please see the ASU PCB Fabrication Process for instructions on how to manufacture / "print" a PCB design in copper.

Why would you want to print a PCB design on paper?

Before sending a PCB to be manufactured, it is imperative to separate the layers and print it at 1:1 (100%) scale on paper to physically verify that your parts will fit through the holes and that pad spacing is correct.

Note: "Plot" in Cadence is synonymous with "Print" in other Windows programs

Note: You can also Print a PCB Layout in DFM Now.

How do you print a PCB design on paper?

1. In PCB Editor, open your design and choose File > Plot Setup... (see Figure 1). The "Plot Setup" dialog box will appear (see Figure 2).

Figure 1: Plot Setup menu option

2. In the "Plot Setup" dialog box, choose a "Scaling factor" of 1.00, "Auto center" checked and "Plot method" matching your printer's capabilities (color or black and white), and click OK (see Figure 2).

Figure 2: Plot Setup dialog box

3. On the right side of the screen, select the Options tab. Set the "Active Class and Subclass" to Etch and the Subclass to Bottom (See Figure 3). This will show the most important details in the printout.

Figure 3: Options tab

4. Choose File > Plot... (see Figure 4). The "Print" dialog box will appear (see Figure 5).

Figure 4: Plot menu option

5. In the "Print" dialog box, click "Setup..." (see Figure 5) and select the printer, paper size, and orientation in the "Print Setup" dialog box (see Figure 6).

Figure 5: Print dialog box

Figure 6: Print Setup dialog box

6. Click OK in the "Print Setup" dialog box, and OK in the Print dialog box to print the design (see Figure 7).

Figure 7: Print dialog box

Based on a tutorial by Seana O'Reilly

Pushing PCB changes back to a schematic in Cadence

Why would I need to back annotate a design?

If you make changes to your design while in PCB Editor (for example, swapping a footprint), you must back annotate (meaning, push changes) from the PCB design back into your original schematic. By doing this update, future changes to the schematic can be forward annotated (meaning, pushed forward) to your PCB design without having to start over from scratch.

How do I back annotate a design from PCB Editor to Design Entry CIS?

1. In PCB Editor, choose Setup > User Preferences... and click on the Logic folder. The User Preferences Editor window will appear (see Figure 1).

Figure 1: User Preferences Editor window with Logic folder selected

2. Under the Logic folder, set schematic_editor to capture (see Figure 1, above). Close the User Preferences Editor.

3. Choose File > Export > Logic.... The Export Logic dialog box will appear. (see Figure 2).

Figure 2: Export Logic dialog box

4. In the Export Logic dialog box, select the Cadence tab and choose the Design entry CIS option under "Logic type" (see Figure 2, above). If the path under "Export to directory" does not point back to the directory your design is stored in, click the "..." button and change it.

5. In the Export Logic dialog box, click the "Export Cadence" button (see Figure 3). You are now finished exporting the design from PCB Editor, but still need to import the design changes into Design Entry CIS.

Figure 3: Export Cadence button in the Export Logic dialog box

6. Open your project in Design Entry CIS.

7. In Design Entry CIS, go to the "Project Manager" window and select the project icon. Choose Tools > Back Annotate... (see Figure 4). The Backannotate dialog box will open (see Figure 5). If you want to make any changes to what is imported, click the "Setup..." button and edit the allegro.cfg file (not recommended for most users) (see Figure 5).

Figure 4: Project Manager and Back Annotate...

Figure 5: Backannotate dialog box and setting up the path8. Click "OK" to complete the back annotation.

Based on a tutorial written by Seana O'Reilly and updated by Griffin Puggie

Changing a Hole Diameter in Cadence PCB Editor

Why would you need to change the hole diameter?

The default diameter of holes in Cadence is 0.3 mm. This is too small for most components to fit through, as well as too small for proper through-plating of vias.
According to the Peralta PCB Mill specifications, hole diameters should be at least 0.5 mm (19.7 mil). Therefore, the following settings are recommended:

• Drill diameter > 20 mil
• Pad diameter = drill diameter + (at least) 30 mil
• Soldermask diameter = pad diameter + 20 mil

Example: If the drill diameter = 31.5 mil, the pad diameter = 61.5 mil and the solder mask = 81.5 mil.

How do you change the hole diameter in PCB Editor?

1. In PCB Editor, open your design and right-click on a via or hole and choose "Replace padstack". If you want to only change the selected via or hole, choose "Selected instance(s)". If you want to change all vias or holes on your board, choose "All instances" (see Figure 1). The "Select a padstack" dialog box appears (see Figure 2).

Figure 1: Replace pad stack contextual menu

2. In the "Select a padstack" dialog box, select Pad62cir32d (which has a 62 mil pad and a 32 mil hole) or another pad with a hole size of at least 20 mil and click OK (see Figure 2). While the hole size is reasonable for many components, the pad size is still too small.

Figure 2: Select a padstack dialog box

3. Or you can modify the existing Padstack in your design. Right-click again on a via or hole and choose "Modify design padstack". If you want to only change the selected via or hole, choose "Selected instance(s)". If you want to change all vias or holes on your board, choose "All instances" (see Figure 3). The "Padstack Editor" dialog box appears (see Figure 4).

Figure 3: Modify design pad stack contextual menu

4. In the "Padstack Editor" dialog box, increase the "Regular Pad" diameters to 60.0 or greater on the TOP and BOTTOM layers (see Figure 4), and change the Mask Layers diameters to 80.0 (see Figure 5).

Figure 4: Padstack Editor dialog box

Figure 5: Padstack Editor dialog box - Mask Layers tab

5. In the "Padstack Designer" dialog box, choose File > Update to Design and Exit. You have successfully increased the pad size of the via or hole.

Based on a tutorial by Seana O'Reilly and updated by Qinchen Zha

Configuring the UART on PSoC®

What is a UART (Universal Asynchronous Receiver/Transmitter)?

UART is one serial protocol used for communicating data between two digital devices (e.g., between the Pioneer Kit and the computer).

When is a UART useful?

Some sensors (e.g., GPS and RFID units) have a UART interface. Additionally, it is very helpful for debugging programs by using it to send messages back to the computer indicating the current status of the program.

How does a UART work?

More information on UARTs is available in the Microcontroller UART Tutorial from Society of Robots.

How many PSoC® chips does the PSoC® 4 Pioneer Kit have?

See the PSoC® Hardware Development Kits page. This is important to understand the answer to the next question.

How do I connect and configure the PSoC® 4 Pioneer Kit to send information to the computer over the UART?

1. On the Pioneer Kit, connect a jumper wire from UART RX (P0[4]) of the PSoC® 4 to J8_10 (P12[7]) of the PSoC® 5LP

2. On the Pioneer Kit, connect a second jumper wire from UART TX (P0[5]) of the PSoC® 4 to J8_9 (P12[6]) of the PSoC® 5LP

3. Connect the Pioneer Kit to your computer with a USB cable.

Next, you will need to determine which COM port the Pioneer Kit is connected to, install a terminal program, and configure it to read data from the serial port on your computer. This will allow you to see the output from your program.

4. Determine which COM port the Pioneer Kit is connected to by opening the Bridge Control Panel application in the Cypress folder in the Start menu, and looking for the COM port listed with the highest number (see Figure 2, below). Write down this port name and close the Bridge Control Panel.

Figure 2: Bride Control Panel

5. Download, install, and open the terminal program PuTTY

6. Click on the Terminal tab and configure it with the settings shown in Figure 3 (below)

Figure 3: PuTTY terminal configuration tab

7. Click on the Session tab and configure it with the settings shown in Figure 4. Use the COM port for your computer determined earlier in this tutorial. Save the session as PSoC and click "Open".

Figure 4: PuTTY Session configuration tab

8. Finished! Now, you can see text sent between your computer and PSoC® 4 Pioneer Kit via the UART.