Creating Padstack in Allegro PCB
Table : Allegro PCB Design Tutorial
Padstacks are the geometrical descriptions of individual pins of a component. The padstcks can be either through hole type or surface mount type. The padstacks are required when creating footprints.
Allegro has a number of through hole and surface mount padstacks in its library. We will create our own padstack by opening one of the existing padstacks and copying it to our location with a different name and then modifying it.
Create a directory, say, C:/learnallegro . We will have our design file in this directory. Let us create two subdirectories to hold the padstacks and the footprints. The subdirectory C:/learnallegro/padstacks will have all the padstacks. The subdirectory C:/learnallegro/symbols will have all the symbols or the footprints.
Let us try to create the padstack for the two pins of the 0603 size SMT resistor padstack. The size of the pad will be 38 mils x 30 mils.
Click on Start -> Allegro SBP 15.2 -> PCB Editor -> Select Allegro PCB Design 610 ( PCB Design Expert) -> Click OK.This will open up the Allegro software. Click on Tools -> Modify Library Padstack. Dont worry, we will not modify existing library padstack. We will copy it somewhere else before modifying it. There are a number of padstacks in the existing libraries. Some of them are through hole and some are surface mount. Let us select one of the surface mount pads, say SMD25_48. This is the padstack for a 25 x 48 mils size SMD pad. Before you move any further click on file -> save as -> go to C:/learnallegro/padstacks and save it as SMD30_38. Now we will make changes to this file so that it becomes a 30 x 38 pad.
In the Parameters window, confirm that the Type is Single and not Through. Mke sure that drill diameter is 0. Click on Layers. Click on the Top row that says BEGIN LAYER. In the Regular Pad change the dimension of width to 30 and dimension of the height to 38. Now click on the row that says SOLDERMASK_TOP. In the Regular pad make width 40 and height 48. Click File -> Save as -> go to C:/learnallegro/padstacks and save it as SMD30_38.
This completes the surface mount padstack.
Next we will create a through hole padstack. Click on Tools -> Modify Library Padstack. Select Pad30cir20d , which is a through hole padstach which has a drill dia of 20 mils and padstack of dia 30 mils. Click on File -> Save as -> go to C:/learnallegro/padstacks and save it as Pad50cir35d. We will be creating a padstack with 35 mil drill and 50 mil padstack. Click on Parameters -> In Type make sure it is Through. In the Drill/Slot hole – change the Drill diameter to 35. Now click Layers. Click on the 1st row that says BEGIN LAYER. In the Regular Pad, Change the Width and Height to 50. Change the Height and Width of Thermal Relief to 60.Change the Height and Width of Thermal Relief to 60. Do the same thing for Default Internal and End Layer. Click File -> Save as -> go to C:/learnallegro/padstacks and save it as Pad50cir35d.
This completes the process of creating padstacks. You will need to create more padstacks in a similar fashion as your design needs. You will also later on need to know the difference in the Thermal relief creation depending upon whether the Power plane is positive or negative. We will cover this topic separately.
Following are the links to some video Flashes that will help you understand Padstack creation.