This Cadence walkthrough goes through the process of creating a PSoC® 4 BLE module schematic symbol and PCB footprint.
In Windows, open “Capture CIS”
Right-click on your custom library and choose “New Part” (see Figure 1). The New Part Properties window will appear (see Figure 2).
Figure 1: Creating a new part in your custom library |
Figure 2: New Part Properties window |
In the New Part Properties window (see Figure 2), name the part and click OK. The new part creation window will appear (see Figure 3).
Figure 3: New part creation window |
Figure 4: Place pin array tool |
Figure 5: Place Pin Array configuration window |
Pro Tip: Instead of configuring Place Pin Array as shown in Figure 5, repeat this step twice: Once for the first 20 pins, and a second time for the remaining 24 pins. This will eliminate the need to move pins from one side of the symbol to the other.
Place the pins on the symbol. You may need to adjust the size of the dotted rectangle in.
Click the “Place rectangle” button in the toolbar (See Figure 6) and add a rectangle box along the dotted lines inside the pins (see Figure 7).
Figure 6: Place rectangle tool |
Figure 7: Schematic symbol with pins and rectangle |
Figure 8: Pin Properties window |
Pin Name | Pin Type |
---|---|
All GPIO pins | Bidirectional |
VDDD, VDDA, VDDR, and all GNDs | Power |
XRES | Input |
VREF | Output |
Table 1: Pin types for the PSoC® 4 BLE module
Figure 9: Final custom schematic symbol for the PSoC® 4 BLE module
|
Figure 10: Saving the schematic symbol |
The custom PCB padstack definition includes mechanical dimensions for the copper pads and the hole to be drilled in the board for each pin in the custom PCB footprint that you will design in Step 4.
In Windows, open “Padstack Editor”
Choose File > New… The New Padstack window appears (see Figure 11).
Figure 11: New Padstack window |
In the “New Padstack” window (see Figure 11), click “Browse…” and select the location of your custom symbols folder (e.g., Desktop/Cadence/symbols)
In the “New Padstack” window (see Figure 11), enter a pad stack name of pad70cir40d_AB (where AB are your initials) and click OK.
On the “Start” tab, configure the parameters to match Figure 12 below.
Figure 12: Start tab configuration |
Figure 13: Drill tab configuration |
Figure 14: Drill Symbol tab configuration |
Figure 15: Design Layers tab configuration |
Figure 16: Mask Layers tab configuration |
Do not change any settings on the “Options” tab. Click on the “Summary” tab and confirm that your padstack matches this example.
Choose File > Save and close “Padstack Editor”
In Windows, open “PCB Editor”
Choose File > New… The “New Drawing” window appears (see Figure 17).
Figure 17: New Drawing window |
In the “New Drawing” window (see Figure 17), click “Browse…” and select the location of your custom symbols folder (e.g., Desktop/Cadence/symbols). Then, enter a drawing name of your choice. Do not use spaces in the drawing name. Choose a “Drawing Type” of “Package symbol” and click OK to return to the empty drawing window.
Next, you need to create the package geometry for the footprint. The package geometry is a visual representation of the physical dimensions of the part. Click the “Shape Add Rect” button in the toolbar (see Figure 18) and click on the Options tab on the right hand side of the screen. Configure the settings in the Options tab to match those shown in Figure 19. The dimensions of the rectangle and the rounded corners came from the PSoC® 4 BLE mechanical drawing (available on the Infineon website).
Figure 18: Shape Add Rect tool |
Figure 19: Options tab for the Shape Add Rect tool |
Figure 20: Package geometry and Command window |
Figure 18: Layout > Pins Options tab configured for the left header |
Figure 19: Left header placed using the command prompt |
Figure 20: Layout > Pins Options tab configured for the right header |
Figure 21: Right hand header placed using the command prompt |
Figure 22: Label Refdes tool |
Figure 23: Options tab for the Label Refdes tool |
Figure 24: Footprint with reference designator |
Open a schematic that uses the custom symbol in Capture CIS.
In your schematic, double-click on the placed custom symbol. The Property Editor window will open (see Figure 25).
Figure 25: Property Editor window for PSoC® 4 BLE module |
Type the filename for the footprint into the “PCB Footprint” field and close the Property Editor window.
To confirm that the footprint was properly linked to the custom schematic symbol, right-click on the part in the schematic and select “Show Footprint”. The “Footprint Viewer” window will open and show the footprint (see Figure 26).
Figure 26: Footprint successfully linked to the custom schematic symbol |
If the footprint does not show up, confirm that the name of the footprint in the Property Editor matches the filename of the footprint, and that the symbols folder is configured correctly in Cadence (standalone / cloud instructions).
The following video shows the process described in this tutorial from start to finish. Note that the Cadence interface has changed for padstack editing since the time the video was created.
Based on a video and tutorial created by Robert Goby