Pads File to Board File

Hi Gaurav,

I  often run sims of PADs designs in Allegro PCB SI. The basic flow is as follows;

1/ Save the PADs design out as an ASCII file - you may have to revert to an older PADs version, such as v5.0 (see header below)

!PADS-POWERPCB-V5.0-BASIC-250L! DESIGN DATABASE ASCII FILE 1.
*PCB*        GENERAL PARAMETERS OF THE PCB DESIGN

2/ Run import PADs utility from Allegro PCB editor (not PCB SI)

3/ Set up the mapping file to map the layers in the PADs design to the layers in the Allegro design.

4/ Import PADs

5/ Check pads_in.log file:

Closing database.
Translation complete.
Finished reading input file with no errors.

Typical problems that can create a lot of work are that values are missing, so if you have lots of different R and C values it can take a long time to set up the ESPICE models.

Good luck, come back if you have any problems!

Chris

Hi Gaurav,

Expanding on the above, you can run the pads_in tool from within PCB editor OR PCB SI.

Also, the mapping I referred to is done by an .ini file. The default one is in the tools/pcb/bin directoryand is set up for mapping a 6-layer board. Edit this file to set the layers you require...

[Options]
CreateSolderLayers=0
SolderOversize=0
[Line Map]
0=BOARD GEOMETRY|ALL
1=ETCH|TOP
2=ETCH|INTERNAL1
3=ETCH|INTERNAL2
4=ETCH|INTERNAL3
5=ETCH|INTERNAL4
6=ETCH|BOTTOM
7=UNUSED|-
8=UNUSED|-