Importing PADS footprint into Allegro 17.2

Well its been awhile. But, these steps may work for this situation. However, no guarantees here thou! 1- All the parts that need translated must be first placed onto a design file in PADS first. 2- get an PADS 5.0 ASCII file of that design file. 3- import the ASCII into the Allegro or OrCAD's PCB.Editor. Hopefully, it will translate correctly and you should see the parts. 4-. Do an Export library within the PCB.Editor to create a library of the converted parts. 5- Set your library path to point to your newly created library to gain access of the parts you need.

Good luck 

Hello, the library  translator from pads to Allegro or OrCAD PCB Editor 17.2, work well and fine. Follow this steps:

1- In pads library manager select one lib for example LIBRARY01, then select ALL "Parts" and export all selected parts it in a file "LIBRARY01.P" file in a folder for example LIB01

2- Repeat the same procedure at point 1, but for ALL "Decal" of the same library off course, you can export a "LIBRARY01.D" file. Now in the folder LIB01, you have 2 files one for parts ".p" and one for decals ".d"

3- In PCB Editor Allegro or OrCAD, select the input translator lib, then  specify the path of library (for example LIB01), then browse to find the pads_lib_ini.ini, and select th output folder, LIB01 or another folder. REMEMBER to flag the "Show options dialog" for MAPPING the exact layer and others objects. If all are done well the translatation start, and you need only to wait the end of translation.

Maybe you need to adjust the options of translations for exact mapping layers and other elements, and repeat the translation.

Hope this help ! Let me know, Best Regards,

Gianni.

www.gpstudiopcb.it

Hi, is the translator able to translate the swappability of gates and pins that are inside the .p file from Pads? Is the program generate the correct device file? With the test that i have done, it seems that it is NOT able to support the definition of the Gates and pin swaps and it only translate (or better converts) all the gates on one unque gate with all the pins NOT swappable. If i am wrong please let me know what to do to obtain the correct translation from PADS components.

Hi (CIAO) Livio Valerio,

the translator extract PCB Symbols. Symbols in Allegro OrCAD PCB Editor are the same as called "decals" in pads. For swap pin and gate in PCB Editor, you need to define it on schematic editor, Capture for example. Then passing the netlist in PCB Editor you are able to swap pin or gates. For pin and gate swapping you must refer to Cadence documents, you can find it on Cadence Online Support. If you cannot find it let me know.

Hope this help, Best Regards to all, Gianni

www.gpstudiopcb.it

Is there a way to do this without PADS? Like say if I only have Allegro?