Home > Uncategorized > How to create footprint in Allegro using Package Symbol wizard.

How to create footprint in Allegro using Package Symbol wizard.

July 25th, 2015

If the footprint that you wish to create in Allegro PCB design, has large number of pins that fit in regular size ( SOIC , TQFP etc), you can use the Package symbol wizard to quickly create the footprint. In this tutorial, we will show you, with example how to do that. We have used the Xilinx XC6SLX9-2TQG144C part as an example to walk through the steps required to use the package symbol wizard.

Step 1 : Collect the required footprint information. The document here lists the package. The page 71 of the document here lists the land pattern. These will used to create the symbols. The recommended land pattern is reproduced here.

landpattern

2. As seen in the above diagram we will first create a pad of size 1.60 mm x 0.35 mm. Since all dimensions are in mm, we will set the units to mm when creating pad. ( Caution - do not make it 0.35 mm x 1.60 mm in place of 1.60 mm x 0.35 mm - you will have to rotate all pins !)

3. Use File -> New Package Symbol Wizard to make make symbol ( footprint).

4. In package Type Select PLCC/QFP

5. In the next screen click on Load Template ( leave Default Cadence supplied template). Click Next.

6. Select Millimeter in the next screen against both fields.

7. In next screen - set Vertical Pin Count to 36 and Horizontal pin count to 36.
Location of Pin 1 - select Top Left corner
Select Lead pitch to be 0.50

8. In the next screen set e1 and e2 to 21.40.
Set E and D to 22.0

9. Click next and select the padstack you created in step 1.

If you are stuck, here is the youtube video for these steps

Uncategorized

  1. No comments yet.
  1. No trackbacks yet.