1. Blog>
  2. How to Create a SMD footprint using the Allegro PCB Editor?

How to Create a SMD footprint using the Allegro PCB Editor?

by: Aug 23,2023 2509 Views 0 Comments Posted in PCB Design Tutorial

Tutorial SMD footprint Cadence 17.2 Allegro PCB Editor

We learned about how to creat the pads of 0603 footprint in How to Create SMD pad in Cadence Allegro. In this tutorial, we will continue to demonstrate the process of creating footprint by taking the 0603 footprint as an example. The footprint specification is shown in the figure below:

Creating Process of SMD Footprint

Take GRM033Z71C104KE14D from Murata Electronics as an example.

Step 1: Open PCB Editor and select Allegro PCB Librarian XL.

Step 2: Click "File">"New" in the menu bar, as the figure below shows:

A new window will pop up. Fill in the footprint name (named C0603 here) in the Drawing Name text box, and select Package Symbol in the Drawing Type option box.

Click Browse to select the storage path. Click OK after finishing the setting.

Step 3: Choose "Setup">"Design Parameter" in the menu bar, as the figure below shows:

Set the User units to Millmeter under the Design menu bar in the Design Parameter Editor dialog box, and then click OK, as shown in the figure below.

Step 4: Select "Setup">"Grid" in the menu bar, as the figure below shows:

The default grid is 2.54mm, modify it to 0.1mm.

Step 5: Select "Setup">"User References" in the menu bar, as the figure below shows:

In the User References Editor window, click "Paths">"Library" in Categories on the left, and click the "..." corresponding to padpath on the right. 

Set the path as the path to save the pad, as shown in the figure below. After setting, click Apply, and then click OK to close the window.

Step 6: Select "Layout">"Pins" in the menu bar, as the figure below shows:

Add a pad in the Options sidebar, and the operation is shown in the following figure:

Note: If you cannot find the corresponding pad when adding pads, please check whether there is a pad file in the padpath.

Step 7: Place the pad. Directly enter the position ("x -0.725 0") in the command bar and press Enter to place the package. Right-click Done.

The picture above is to place pin 1, and the picture below is to place pin 2. Enter the coordinates ("x 0.725 0") and press Enter. Right-click Done.

The effect after placing is shown in the figure below.

Step 8: Add an silkscreen outline on the silkscreen layer. Click "Add">"Line" to set the layer and line width.

Select "Package Geometry">"Silkscreen_Top" in Options, and set the silkscreen line width to 0.15mm.

The completion effect of silkscreen drawing:

Note: It is recommended that the distance between the pad and the silkscreen is not less than 6mil.

Step 9: Referring to Step 8, add the same line on the Assembly_Top layer, and set the line width to 0mm.

Step 10: Place Place_Bound (used to set the area occupied by the package, you can use Place_Bound to check whether the devices overlap later).

Click "Add">"Rectangle",as the figure below shows:

Select "Package Geometry">"Place_Bound_Top" in Options.

The completion effect of Place_Bound_Top:

Step 11: Click "Layout">"Labels">"RefDes" to set the reference number.

Select "Ref Des">"Silkscreen_Top" in Options.

Put a position on the pad and input C*, as shown in the figure below.

Step 12: Referring to Step 10, add a refdes C* on the Ref Des/Assembly_Top layer.

Step 13: Click "Layout">"Labels">"Value" to set the device value.

Select "Component">"Silkscreen_Top" in Options.

Put a position on the Pad and input Value, as shown in the figure below.

Click Save, and the creating of a package is completed.

Join us
Wanna be a dedicated PCBWay writer? We definately look forward to having you with us.
  • Comments(0)
You can only upload 1 files in total. Each file cannot exceed 2MB. Supports JPG, JPEG, GIF, PNG, BMP
0 / 10000
    Back to top