PADS POWERPCB TUTORIAL


Creating 4 Layer Board

Till now we have been doing everything with 2 Layer board. Let us try to extend the board to a 4 layer board. We will be using the second layer for ground plane. The third layer will be used for power plane.

* Click Setup -> Layer Definition. It shows only two layers - Top and bottom

* To change increase the number of layers to 4 click on Modify under Electrical Layers. Enter 4 as the new number of layers. In the screen that follows, reassign the old layer 2 to layer 4.

* Now we have four layers. We will be reassigning layer 3 for ground plane. Click on the Inner Layer 2 and in the Plane Type - click Split/Mixed. Now click the Assign Nets. We want the GND_POWER net to be assigned to the ground plane. So click on the GND_POWER and click Add>>. Click OK.

* Click on the Inner Layer 3 and in the Plane Type - click Split/Mixed. Now click the Assign Nets. We want the VCC net to be assigned to the ground plane. So click on the VCC and click Add>>. Click OK.

Changing Net Colors

* It becomes easier if we assign some color to the Power and Ground Nets. We will assign Brown color to the ground net and pink to the power net.

* Click on view -> Nets. click GND_POWER in the Net List and then click ADD. In the View List now click GND_POWER and click on the Brown color.

This will color the GND_POWER net by brown.

We will now color the VCC net by pink. Click VCC in the Net List and then click ADD. In the View List now click VCC and click on the Pink color.

Click Apply and OK.

Changing Default Rules

The Design Rule checks are list of the checks including minimun trace width and trace separation. There is a default rule for all nets and there is a rule for individual nets.

To view or change the Design Rules - click setup -> Design Rules - Default. For now, we will just look at the most common trace width and separation. Click on Clearance. Change the Trace Width Minimum from 12 to 6, recommended from 12 to 6 and maximum from 12 to 100. Leave other things as it is. When you will be doing more fine pitch design you may have to reduce the minimum trace width and clearances to 4 mils.

Click OK.

We can also set the default width of nets wider. For example power nets will be normally wider. Click click setup -> Design Rules -> Nets. Select the net GND_POWER and then click Clearance. Change the Trace Width Minimum from 12 to 6, recommended from 12 to 20 and maximum from 12 to 100. Leave other things as it is.

Adding and changing Default Vias

We will have to use Vias when Changing the layers when routing. To View or change the available via click Setup padstacks. In Padstack Type select Via. You should see a Standard Via with 37 mil drill size and 55 mil pad size. This via is too big. Let us create an additional smaller via.

Click on Add Via.In the Vias name, write MINIVIA. Set the Drill Size to 15.Set the PAD sizes to 25 mils for all layers. Click OK.

Now we have two vias that we can use in our design when routing.

Our design is now ready for routing. You can see tha above in a Flash movie in the following link.



Next we will see, how to how to do simple routing.

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