Friday, May 18, 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: Changing Testpoint Vias
Posting to forums is available to community members only.
Login or Register
Rate this topic:
   
Author Messages
EMAJeff
Posts: 0
Online: User is Offline
11/12/2004 7:08 PM  
Hello,

I have a BRD file that contains a large amount of testpoints.

I have supplied the test house a board file and they extracted test points of their choosing. Now my fixture might differ from their selected testpoints.

Does anyone know of a way to automatically read an ascii testpoint file and compare it to the Allegro testprep fixture one I have. I really need to lock down my fixture to match the test houses fixture for future ECNs.

Any help would be appreciated.
Padmin
Posts: 0
Online: User is Offline
11/15/2004 7:33 AM  
"One suggestion is to text edit the Allegro testprep report so it is in the same format as the report supplied by the board house and compare the two files.

If your file is too large to edit, you may want to create your own extract file and edit it so the format matches the one supplied by the test house. The extract (extracta) command file (from SourceLink solution 1816263) could look similar to:

FULL_GEOMETRY
CLASS= MANUFACTURING
SUBCLASS = PROBE_BOTTOM
NET_NAME
NET_NAME_SORT
VIA_X
VIA_Y
PIN_X
PIN_Y

END

To generate output similar to:

S!A0!A 00000000!4550.00!4535.00!!! <- via
S!E0!E 00000000!!!6350.00!4550.00! <- pin


You can download a free eval copy of a nice text editor at: http://www.textpad.com/ that would help you accomplish this.

Hope this helps!
splash
Posts: 2
Online: User is Offline
3/15/2006 6:37 PM  
Dear Experts
I have a similar problem to this thread.  I am trying to extract a list of
netname, device pins and x y coordinates and the layer they are on (top or bottom). 
I'm also looking to do the same with vias - netname, x y and layer (top or
bottom if they are blind vias.

I originally had this for the extract(a) file.  But couldn't find a parameter for 'layer'.

COMPOSITE_PAD
NET_NAME
REFDES
PIN_NUMBER
PIN_X
PIN_Y
END

Will the following work?
FULL_GEOMETRY
CLASS= MANUFACTURING
SUBCLASS = PROBE_BOTTOM
NET_NAME
REFDES
PIN_NUMBER
PIN_X
PIN_Y
END

Then I would create a second file for the top:

FULL_GEOMETRY
CLASS= MANUFACTURING
SUBCLASS = PROBE_TOP
NET_NAME
REFDES
PIN_NUMBER
PIN_X
PIN_Y
END

Is probe_top a way to get the components on the top of hte PCB?

Then for the vias I was going to do this:
FULL_GEOMETRY
CLASS= MANUFACTURING
SUBCLASS = PROBE_BOTTOM
NET_NAME
VIA_X
VIA_Y
END

FULL_GEOMETRY
CLASS= MANUFACTURING
SUBCLASS = PROBE_TOP
NET_NAME
VIA_X
VIA_Y
END 

So I can identify which vias are on which side and which components are on which side.

Any insight would be appreciated.

Regards,
Splash
drew3rdof3
Posts: 18
Online: User is Offline
3/15/2006 7:33 PM  
> Is probe_top a way to get the components
> on the top of the PCB?

Nope.  PROBE_[TOP/BOTTOM] are used for test points most commonly used for bed-of-nails testing.  In the footprint, one would use NO_PROBE_TOP to define a shape to keep those test points a certain distance away from the footprint.  The shape flips to the _BOTTOM when the footprint is on the secondary side and the PROBE_BOTTOM subclass is defined.  I cannot remember if this is done by default.

After saving a good copy of the BRD file, check out the menus under  'Route' > 'Testprep'.  When test-points are generated in Allegro it puts symbols on these layers to generate a location file for each nail.

There are a lot more things to consider but I will stop here since this has nothing to do with what you are currently trying to accomplish.

Cheers,
Drew
drew3rdof3
Posts: 18
Online: User is Offline
3/15/2006 7:42 PM  
Oh!

The pins of the footprint are located at;

CLASS: Stack-Up
SUBCLASS: pin/top

SUBCLASS: pin/bottom

The reference designators are located at;

CLASS: Components
SUBCLASS: ref_des/silkscreen_top

SUBCLASS: ref_des/silkscreen_bottom

Cheers!
Drew
Posting to forums is available to community members only.
Login or Register
Forums > Silicon-package-board > PCB Design > Changing Testpoint Vias


ActiveForums 3.6
     
Copyright 2006 Cadence Design Systems, Inc.