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: Package to package spacing
Posting to forums is available to community members only.
Login or Register
Rate this topic:
   
Author Messages
MURPHYS
Posts: 33
Online: User is Offline
11/28/2007 8:09 AM  
On my design that I converted from Orcad I have several package to package errors. Since we had our library shapes set up so that components could be placed line to line this is an issue. Is there some place I can change this? Thanks

Sandy
cadpro2k
Posts: 0
Online: User is Offline
11/28/2007 9:56 AM  
Sure can. Edit the symbols (ORcrap symbols that you converted to Allegro), and change the PLACE_BOUND_TOP to the "actual" size of the part. I'm guessing the translation expanded the boundry. Next, create a text file (like UPDATE_SYMS.lst), and add the symbol names you've changed. Next, in Allegro, do PLACE/UPDATE_SYMBOLS; check the symbol list (browse to your file); and update the symbols. If your constraints are set right, your errors should go away.

I know it sounds long, and drawn out, but it's fairly painless to do 10-15 parts. I do that on almost all my converted drawings (mostly coming from PADS). Also helps to have a 'generic' symbol library to pull from, so you don't have to continually mod common parts.

Good day.
Mitch
MURPHYS
Posts: 33
Online: User is Offline
11/28/2007 11:19 AM  
Ok, this makes sense and thats exactly what happened. How do I change the size of the place_bound_top box? I haven't ran across anyplace I can move these boundaries in. Does this make sense? Thanks

Sandy
Hpattie
Posts: 33
Online: User is Offline
11/28/2007 1:23 PM  
Placebound_top is a shape. In the symbol editor, you can either delete and redraw the placebound, or edit the shape.
Regards,
Harold
Harold Pattie C. I. D.+
MURPHYS
Posts: 33
Online: User is Offline
11/28/2007 1:29 PM  
OK, thanks to all of you I have that figured out. Now I need some advice on fiducials. In Orcad I had fiducials as part of the footprint and could move them to where I wanted them to be. Is there a way in Allegro to edit and move them locally or should I add them seperately? Also, how do I now get them off my translated PCB without the whole component being removed?

Sandy
cadpro2k
Posts: 0
Online: User is Offline
11/28/2007 5:00 PM  
Sure can.

Edit the symbol.
set the property: UNFIXED_PINS to TRUE.
You will now be able to move/delete the fiducials that are a part of the symbol.

BE VERY CAREFUL you don't move other pins in the part though :)

The 'local' package boundry can be mod'd too inside the layout. I do this all the time, when I need place things close together, and I know it's not a DFM issue.

Good day.
Mitch
cadpro2k
Posts: 0
Online: User is Offline
11/28/2007 5:04 PM  
Using SHAPES - tricks

Edit Shapes -
Move vertices around the shape (you can change from ALL LAYER grid to ETCH grid to increase accuracy.. good to know)
Delete vertices - simply select a vertex and RMB delete
Edit boundry allows you to REALLY modify the shape, good for quick changes
Next is important for keeping the selections going.

Good day.
Mitch
MURPHYS
Posts: 33
Online: User is Offline
11/29/2007 4:12 AM  
Thanks for all you help. I am sure I will be here asking other questions as I get used to Allegro.

Sandy
MURPHYS
Posts: 33
Online: User is Offline
11/29/2007 7:00 AM  
OK..one more question for now. Where is UNFIXED_PINS located? Is this done on the .brd file?
Trykon
Posts: 58
Online: User is Offline
11/29/2007 7:23 AM  
If you are in a board

Menu Select

Edit > Properties
Select the symbol
In the Edit Property GUI scroll down on the left to select the Unfixed_pins property to move it to the right
Select OK

The property will be added to the symbol instance. You will be able to move the pins

If you are in the symbol editor

Menu Select

Edit > Properties
In the Find filter "Find by Name" section set the pulldowns to "Drawing" and "Name"
Select "More..."
In the "Find by Name or Property" dialog move "Drawing Select" to the right hand side
Select "Apply"
In the Edit Property GUI scroll down on the left to select the Unfixed_pins property to move it to the right
Select OK

The unfixed_pins property will be added to the drawing and you can move or delete the pin(s)
Posting to forums is available to community members only.
Login or Register
Forums > Silicon-package-board > PCB Design > Package to package spacing


ActiveForums 3.6
     
Copyright 2006 Cadence Design Systems, Inc.