PADS POWERPCB TUTORIAL

Creating Board Outline

After creating the foot print, the next process is to create a board outline.

* Start the PADS and click File -> New -> System Default Start-up File

* Select Drafting button followed by "board outline and cut out" button

* Place the cursor at the origin and click left button. Now take the button to approximately to the upper right corner of the size of the board and then left click again.

* The dimensions of the board outline are not exact. Let us do it right. Right click and select "board outline". Now click on the right edge of the board outline and select "query modify". Enter the correct dimensions. Do the same for the upper edge.

* Save the file as say experiment_01.pcb

Importing the Netlist

* The Next process is to import the net list. Let us assume that we have a netlist generated from Orcad. The name of the netlist file is experiment.asc and has the following content. 

*PADS2000*
*PART*
D1 LED
J1 HEADER2
R1 R0603_1

*NET*
*SIGNAL* GND_POWER
J1.1 D1.2
*SIGNAL* VCC
R1.1 J1.2
*SIGNAL* N000031
D1.1 R1.2
*END*


* Click File Import and then point to the ASC file. After importing you should be able to see all components concentarted at the origin.

Spreading and placing the component

* Click on Tools -> Disperse Components and it will disperse the components. You can now see the three components with rats connections.

* The next step is to place the components.

* Click on the design button , followed by the move button . Let us say we want to move the header J2. Take the cursor to the Header and then left click on it. The header will be "lifted". Now move the cursor to the place you want to move it and then left click again. If you want to rotate the component you can do so by Control + R ( This can be done while moving or separateley after sellecting the component). If you want to place the component at the bottom, use Control+F.

* It is possible that the components are not placed "exactly" at the desired location. To correct this problem, select the component using select tool , right click it and select "Query Modify" and the enter the coordinates of the component.

Do the same thing for all three components. Let us place the resistor at the bottom.

Save the design as say, experiment_02.pcb

This completes the process of the component placement. You can view the Flash of this here for a better undestanding.



Next we will see, how to create a power planes, how to assign default rules, how to create a via, how to do simple routing.

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