Translating orcad footprint to allegro footprint without Transolb.exe

Hi Niraj,

U Can find A layer2alegro (L2A) converter in tools\pcb\bin or in Cadence utillities Using this u can do it.

Raghuram

OrCAD® Layout to Allegro® Allegro PCB Editor Translator

PCB designs created in any version of OrCAD® Layout may be converted to Allegro® PCB Editor designs using the File - Import - OrCAD Layout (orcad_in command). The translator converts designs (.max files) created in Layout to design databases (.brd files) that can be read by Allegro PCB Editor. The Layout.max file contains all footprint information.

Do the following to translate designs from Layout to Allegro PCB Editor:

1.                  Create a catalog of the library using the Layout Catalog tool and generate .max files. Layout libraries contain TOP, BOTTOM, PLANE, and INNER layers. The rest of the layers are documentation layers.

2.                  Convert the .max files into Allegro PCB Editor (.brd) files using the Allegro Allegro PCB Editor File - Import - OrCAD Layout (orcad_in command). The .max file the Catalog tool creates also contains these four layers and the rest of the layers are documentation layers.

3.                  Delete PLANE and IS2 layers using Setup - Cross-section.

4.                  Create the flash and shape symbols if you wish to update the same for the padstacks of your design. Otherwise, run DBDoctor.

5.                  Update padstacks with Tools - Padstack - Modify Design Padstack.

6.                  Run the DB Doctor program on the design.

7.                  Export all the symbols from your .brd file using File - Export - Libraries.

Hi raghuram,

                     It is very nice of you to have answered my querry, but the problem with L2A tool is that, it takes .MAX file as an input, and I am comfortable with .brd file(allegro), i have not created a .Max file till date. I don't know how to place all footprint(orcad) into the max file. Can I create a max file without a schematic, and place all the required footprint, and then use L2A? If that is possible , then L2A may be helpful for me.

Thanks and Best Regards

Niraj

Hi Niraj,

u can do it by placing all u r library components on a ORCAD board file ( *.MAX) and save it then u can go for conversion

Regards,

N Raghuram

Hi Raghuram,
Thank you very much, I can do it now :) . The thing was, I was little apprehensive about the placement of conponents(or footprints) in the layout file, bcoz in allegro, you are suppose to export your schematic, and then place ur components(footprints), and then proceed.

On the same tracks, I didn't found the procedure to create a Max file, and then import all the footprints , so that was the cause of my problem.

But now its OK, and all credit goes to you and Mr Rgauldin.

Thanks once again Buddy

Regards
Niraj
[b] [/b][b] [/b][b] [/b]