Wednesday, February 08, 2012     Register | Login | Search | Contact Us
     
   
     
     

Many of you already received communications about the move of the Cadence user community into cadence.com. And many of you have already joined, with over 4000 registrations in the first two weeks.

The new Cadence Community enhances the ability of Cadence users to connect and collaborate. In addition to moving the community into cadence.com -- enabling single sign-on for community, Sourcelink and Cadence events -- the new site is organized around nine technology segments, giving you easy access to product information, training, forums and blogs. Some of the new features include:
  • Ability to respond to posts via e-mail
  • Technology-specific blogs
  • Latest Web 2.0 social networking capabilities
  • Public profile options
  • Private messaging
  • Friends lists
Visit the new Cadence Community today at www.cadence.com/community and join the discussions!

Registration note: Due to the scope of the enhancements and the new SSO registration system, we were not able to migrate existing cdnusers.org member accounts. So new registrations are required, but this enables a broader set of functionality we think you'll enjoy.

Forum note: Under the guidance of forum moderators, we have taken the 20+ cdnusers.org forums and consolidated them into 11 forums on the new site. Posts have been brought over so you can leverage that posting history. CDNusers forums will be set to read only starting 7/30, and cdnusers.org will be redirected to the new community on 8/4.

Best regards,
Mike and Tom

Michael A. Catrambone - Steering Committee Chairman
Distinguished Engineer
PCB/Mechanical
UTStarcom, Inc.

Tom Diederich
Cadence Community Manager
Home
Forums
Forums > Silicon-package-board > PCB Design

Subject: Translating orcad footprint to allegro footprint without Transolb.exe
Posting to forums is available to community members only.
Login or Register
Rate this topic:
   
Author Messages
nforniraj
Posts: 8
Online: User is Offline
11/15/2007 11:48 PM  
Hi ,
      I am new in the field of allegro PCB design , and currently facing some problems in creating land patterns(Footprints) in allegro.
      I have  a querry -> can I transalte an orcad footprint to allegro?
I tried one method and that is , place all the footprints(That need to be changed ) in a board file .MAX format and use the utility transolb.exe, but i was not succesful in doing so.

Do any of you guys have a separate method?

It would be of great help for me

Thanks and regards
Niraj
visiontek
Posts: 30
Online: User is Offline
11/17/2007 2:57 AM  
Hi Niraj,

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

Raghuram
rgauldin
Posts: 17
Online: User is Offline
11/27/2007 2:31 PM  

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.
nforniraj
Posts: 8
Online: User is Offline
11/28/2007 2:34 AM  

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
visiontek
Posts: 30
Online: User is Offline
11/28/2007 3:57 AM  
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
nforniraj
Posts: 8
Online: User is Offline
11/28/2007 4:09 AM  
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]
Posting to forums is available to community members only.
Login or Register
Forums > Silicon-package-board > PCB Design > Translating orcad footprint to allegro footprint without Transolb.exe


ActiveForums 3.6
     
Copyright 2006 Cadence Design Systems, Inc.