Monday, October 06, 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 > Signal Integrity and Modeling

Subject: Extracting Multiple Nets from PCB Editor into SigXplorer
Posting to forums is available to community members only.
Login or Register
Rate this topic:
   
Author Messages
nipri
Posts: 6
Online: User is Offline
1/24/2008 7:52 AM  
I hope that this question is appropriate for this forum

I am using the "L" version of PCB Performance and SigXplorer and am still somewhat new to them.

I am trying to use the Topology Extract feature to extract a net into SigXplorer. The net is actually divided into 2 individual nets with 2 net names. Net #1 is routed from the driving source to one side of a series terminating resistor. Net #2 connects the other side of the term. resistor to the receiver.

Using Topology Extract, I can only seem to extract one net or the other (including the resistor) into SigXplorer. How do I specify that I want to extract the entire net (from source to receiver)?

Thank You

Nick
darmoni
Posts: 8
Online: User is Offline
1/24/2008 8:19 AM  
Hi,
the SQuest & SigExp must recognize the net as xnet, for that you need to assign a SI model to the serie resistor.
Doron.
nipri
Posts: 6
Online: User is Offline
1/24/2008 8:38 AM  
Hi and thanks for the reply!

The resistor is part of a resistor pack to which I have created / assigned an IBIS device model. I assigned all of my IBIS models through the Setup Adviser.

How are Xnets created? Is this done through the Constraint Manager? My installation of 16.0 seems to have some problems with the help files!

Nick
darmoni
Posts: 8
Online: User is Offline
1/24/2008 9:22 AM  
if you created it right then it should work.
you either didn't creat a valid part or didn't assign it in the advisor,
make sure that the value field is a number only (10 not 10R or such).
also i think that it should be a spice model device not ibis model.
good luck.
Doron.
Kalevi2
Moderator
Posts: 69
Online: User is Offline
1/24/2008 9:40 AM  
You have to assign a dml model to the rpack and the rpack has to have the property of being a discrete for this to work correctly. SourceLink has a good example of an Rpack with common pins and the create e spice model will do standard rpacks automatically.
Kai Keskinen
nipri
Posts: 6
Online: User is Offline
1/24/2008 11:18 AM  
>>You have to assign a dml model to the rpack<<

Actually, I used the IBIS file generator in Model Integrity to make an Ibis model for the resistor pack which has 8 isolated resistors (not bussed, no common pin) I then converted the Ibis device model to DML and assigned it to each resistor pack in my design through the Adviser. The value field is set to the value of the resistor (47) with no other chars.

When I extract either net into SigXplorer, the resistor also ports in with the correct pins on the resistor pack that the nets are connected to and the correct R value (47) also ports in. It's only the other net and its driver or receiver that doesn't port in.

>>the rpack has to have the property of being a discrete<<
Where do I set this?

>>SourceLink has a good example of an Rpack with common pins<<
Im in the process of looking for this now.

Nick
Kalevi2
Moderator
Posts: 69
Online: User is Offline
1/25/2008 6:20 AM  
You can change a device type in Logic - Parts List but if you have correctly assigned an espice model to the rpack, this should not be a problem.
Kai Keskinen
Donald Telian
Posts: 42
Online: User is Offline
1/25/2008 10:53 AM  
Extracting through the resistor should work (eventually!). Make sure you have PinConnections.

When all else fails, you can extract the two nets separately and then use the File -> Append feature to glue them together. That feature is powerful yet simple, and works quite well.

Donald
Donald Telian
SI Consultant
telian@sti.net
559-760-5793
ejlersen
Posts: 40
Online: User is Offline
2/11/2008 10:34 PM  
Hi,

I've seen cases in the L version of the tools where you need to run Tools, Database check inside the PCB Editor in order for it to recognize the xnet after assigning espice models to resistors - so try that.

Best regards,
Ole
Best regards,
Ole Ejlersen
Technical Service Manager
Nordcad Systems A/S
Posting to forums is available to community members only.
Login or Register
Forums > Silicon-package-board > Signal Integrity and Modeling > Extracting Multiple Nets from PCB Editor into SigXplorer


ActiveForums 3.6
     
Copyright 2006 Cadence Design Systems, Inc.