Thursday, December 04, 2008     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: Export IDF Format
Posting to forums is available to community members only.
Login or Register
Rate this topic:
   
Author Messages
rame
Posts: 11
Online: User is Offline
6/23/2008 10:05 PM  
Hi folks, Have anyone tried to export the board file to IDF Format and successful? I have problem while exporting,i had defined height max & min for the respective components in the dra file,updated the symbols in the board file, and while i try i export it,it asks for default height,height was specified,And it generates with the default value rather than the actual value defined in the dra file.. We need the IDF File for our solid works software,which can import the file for our board Feasibility study with various assemblies,like front panel,back panel etc,for our prototype purpose am i missing some step along ?. Request someone to help me out in this issue.. Thanks & Best Regards, Ramesh
Trykon
Posts: 58
Online: User is Offline
6/24/2008 6:47 AM  
Ramesh,

IDF will export the PACKAGE_HEIGHT_MAX of each unique component as defined in your library. By unique I mean that the entries in the file are unique per combination of the geometry name field and the part number field. If you have ten capacitors that are the same symbol and part number you will only get one library definition for that component in the idf file.
Randy R.
Posts: 52
Online: User is Offline
6/24/2008 9:01 AM  
The IDF export height assigned to a part is done in the following order:
First it looks for a HEIGHT property on the component.
Second, it looks for the PACKAGE_HEIGHT_MAX property on the symbol's placebound.
Third, it uses the idf export default height.
Note: You can check these heights in the board file and in the exported IDF file.
G'Day,
R²
rame
Posts: 11
Online: User is Offline
6/24/2008 9:09 PM  

Thanks Randy & Trykon for your replies,as i told you in my earlier mail,i had defined the min and max values in the Dra file itself and while exporting it to IDF,it asks for Default value,once the value set in the default option,it considers the default value and exports rather than one entered in the dra file min and max package height.

My question,is IDF file generated takes always the default value?if you see yes then whats the purpose of values entered in min and max in second step as told by Mr Randy? please explain ..

Thanks & Best Regards,

Ramesh
canind
Posts: 14
Online: User is Offline
6/25/2008 3:47 AM  
Ramesh,
There is a 3'rd party plug-in for Solid Works called "Circuit Works" which greatly enhances the IDF import of Solid Works, it's worth looking into.
Also, I have noticed bugs over the years with SDRC and Pro-E importing IDF files. Every so often I get a few holes that to not match the location data in the file so be aware. I'm not sure if Solid Words has that same bug though.
Regards
Ken
Kenneth J. Wood
Saturn PCB Design, Inc.
2737 Bishop Lane
Deltona, Fl 32725
Phone: 407-340-2668
Email: sales@saturnpcb.com
Internet: http://www.saturnpcb.com
Trykon
Posts: 58
Online: User is Offline
6/25/2008 5:00 AM  
Ramesh,

As Randy had posted IDF export output height data according to the following precedence:

1. From the component definition HEIGHT property. This can be ignored for all
using the environment variable IDF_IGNORE_COMP_HEIGHT.

2. From the symbol definition PACKAGE_HEIGHT_MAX property.

3. From the default value set as an option to idf_out.exe or in the Export IDF
UI.

You should ensure that the symbols have the correct heights in the board file using Edit >Properties and select component placebound shape.
Posting to forums is available to community members only.
Login or Register
Forums > Silicon-package-board > PCB Design > Export IDF Format


ActiveForums 3.6
     
Copyright 2006 Cadence Design Systems, Inc.