I have couple of PADS file and I need to perform SI analysis on it. Since I have been using PCB editor and PCB SI tools, I was wondering if I can import PADS file directly into PCB Editor and PCB SI tool without loosing any information.
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!
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=0SolderOversize=0[Line Map]0=BOARD GEOMETRY|ALL1=ETCH|TOP2=ETCH|INTERNAL13=ETCH|INTERNAL24=ETCH|INTERNAL35=ETCH|INTERNAL46=ETCH|BOTTOM7=UNUSED|-8=UNUSED|-