Thursday, January 08, 2009     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: Problem deleting layers in stackup
Posting to forums is available to community members only.
Login or Register
Rate this topic:
   
Author Messages
dgstan
Posts: 7
Online: User is Offline
3/23/2006 10:42 AM  
Hello,

   I've got a 4 layer board that is getting change to double-sided. I realize that you can't delete layers in the cross-section if there are elements residing on them. I have dilegently deleted everything on the two inner layers. When I try to delete the layers in the cross-section I get two different errors.

One one layer I get the error: "Can't delete this subclass, SYMBOL DEFS contain geometry on this subclass".

The other layer give a list of element Allegro thinks still reside on the layer.

(------------------------------------------------------------)
(                                                            )
(        Database Objects Preventing Layer From Being Deleted)
(                                                            )
(        Drawing          : 200-115447-0000P1.brd            )
(        Software Version : 15.2s080                         )
(        Date/Time        : Thu Mar 23 10:38:22 2006         )
(                                                            )
(------------------------------------------------------------)

Layer being deleted: ETCH/L3_PWR

    (2050.00 -1950.00) TEXT: Vcc Plane  Layer 3
    (2050.00 -1950.00) TEXT LINE: Vcc Plane  Layer 3
    (0.00 -300.00) TEXT: E/M,
    (0.00 -300.00) TEXT LINE: E/M,
    (550.00 -1300.00) TEXT: 3
    (550.00 -1300.00) TEXT LINE: 3
    (1250.00 -1300.00) TEXT: 11
    (1250.00 -1300.00) TEXT LINE: 11

Trust me, these features DO NOT exist on the layer. I've done everything possible to delete the text - it's not there!

I've also done the whole DBDOCTOR thing many times. Does anyone have any secret methods of getting rid of these layers or the "phantom features"?



Thanks,

Doug Stanley
cmusetti@silverstorm.com
Posts: 0
Online: User is Offline
3/23/2006 11:00 AM  
Doug,


    I have had this problem before we put our stackups in the board symbol and it created the same problem had to go back to the board symbol delte them then recreate the bsm and update that symbol in allegro. Your problem maybe this or some package symbol.

Carl
mcatramb91
Posts: 141
Online: User is Offline
3/23/2006 11:21 AM  

In addition to checking for symbols that may have a cross section defined I would also turn on the Route and Via Keepouts for two internal layers to insure that there isn't any shapes defined which would also prevent the layer from being deleted. 

Mike
dgstan
Posts: 7
Online: User is Offline
3/23/2006 1:46 PM  
Posted By cmusetti@silverstorm.com on 3/23/2006 11:00 AM
Doug,


    I have had this problem before we put our stackups in the board symbol and it created the same problem had to go back to the board symbol delte them then recreate the bsm and update that symbol in allegro. Your problem maybe this or some package symbol.

Carl


Yeah, we figured it out. There was an old .bsm in the board. Even though there was no features on the layers, simply having the layers defined in the .bsm was enough to cause the problem.

I discovered this by refreshing all the parts and then doing a library dump. I had to open each .psm/.bsm to see what each symbol was made of (luckily, I started with the suspect symbols and found the culprit after a few).

I find it odd that I'd get two different error messages for two different layers when there was really only one problem.

Thanks for your help.


Doug
Posting to forums is available to community members only.
Login or Register
Forums > Silicon-package-board > PCB Design > Problem deleting layers in stackup


ActiveForums 3.6
     
Copyright 2006 Cadence Design Systems, Inc.