PADS POWERPCB TUTORIAL

Creating footprint

Let us try to create the footprint of the SMT resistor used in the design.

* The SMT resistor will have a footprint name of R0603_1. It will have two pins. The size of the pad will be 38 mils x 30 mils. The two pads are 62 mils apart. It will be enclosed by a rectangle of size 140 mils x 70 mils. The pads will be created such the the origin will be in the center of the two pads.

Use the following steps to create the footprint. * After opening the PADS, Click File -> Library. In the pop up menu, select the Library C:\padspwr\Lib\usr. We will be creating and saving the newly created library in C:\padspwr\Lib\usr . Slect Decals and Click New.

( Click the drafting button followed by the Termial button . The Terminal button will add a pad. bring your mouse near the center and click left. By default it adds a through hole pad. Click the Select button , take your mouse to the PAD, left click to select the pad and then right click and select "Pad Stacks" ( If your pad does not get selected, right click and click and "select anything") . It will prompt a window in which we can modify the padstack.

* Make the Drill size 0, since it is a SMT component. Change the mounted side pad to a rectangle of dimension 38 x 30 mils. For inner and opposite layers, set the circle sizes to 0.

* This will create a rectangular pad. Now we need to keep the pad at the right place. Select the pad, right click, select query modify. This will prompt for the coordinate. For X coordinate give -31. Leave Y to 0. This will place the PAD at (-31,0).

* We will create the second pads by step and repeat process. Select the PADS, right click and select step and repeat. Keep the distance at 62. Select OK.

* This will electrically complete the footprint. We will however, like to add a rectangle around it for the silkscreen. Click the 2D Line Button . Right Click and select "Rectangle". Add a rectangle by first left clicking at the place where you would like the left bottom corner and then keep holding the left booton drag to towards the upper right corner.

* The dimensions of the so created rectangle may not be very accurate in dimensions. So, using the select button , select the left edge of the rectangle, right click, select "query modify" and then modify the coordinates of the rectangle. Do the same for the right edge of the rectangle.

This will complete the process of creating the footprint. You may have slight difficulties at some point and you will have to do some experiments here and there to see what works. You may alse see the following flash which captures the above process.



You can similarly create the footprints of the HEADER2 and LED. Make sure that - if these names already exist in the PADS library then you either use them as it is or create them with a different name. If you create them with a different name, make corresponding changes in the Orcad design.

Next we will see, how to create a board outline, import netlist, and place them.

If you like this tutorial, you may like to get the book Signal Integrity for PCB Designers from amazon.