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 > Custom IC > Custom IC Electrical Design

Subject: Addition of source with know statistical data
Posting to forums is available to community members only.
Login or Register
Rate this topic:
   
Author Messages
axp
Posts: 21
Online: User is Offline
6/18/2008 8:21 AM  
    Hi All,

I would like to run a monte carlo simulation on my analog design. I know the statistical distribution (gaussian shaped) of the input signal I have to provide to my system.

Does anyone know how to provide this information to a source like VDC in analogLib library?

Thanks for your support,
Best regards,

Axel
adbeckett
Posts: 248
Online: User is Offline
6/18/2008 2:39 PM  

Create a file with a ".scs" suffix, and set up the distribution you want (see "spectre -h montecarlo" for more details.

Then reference this file with Setup->Model Libraries in ADE. In the ADE variables, define variable MYDC, and give it a value (this will be your mean value). 

// statistics block for my
// design variables

statistics {

   process {
      vary MYDC dist=unif N=0.3
      }

   mismatch {
      vary MYDC dist=gauss std=0.05
   }

}

On an instance of the vsource, you can use the design variable "MYDC". If you want mismatch to be modelled, you'll need to ensure that the vsource is within a subckt - so create an additional level of hierarchy around the vsource in order to do this.

That's it.

Regards, Andrew.
axp
Posts: 21
Online: User is Offline
6/19/2008 1:03 AM  
Hi Andrew,

thanks for your fast reply... However that fails.


I have defined a variable in ADE named bgv = 1.2 V
I have defined a new cell including a vsource component whose DC value is the variable "bgv"

I have created a "bgvoltage.scs" file:

[quote]statistics{

mismatch{
vary bgv dist=gauss std=15e-3
}

}[/quote]

and have added this file to ADE.

However it tells me that the "bgvoltage.scs" file does not contain any library and it reports me an error.

Do you have any idea of what I have to do ?

Thanks in advance !!

Axel
adbeckett
Posts: 248
Online: User is Offline
6/19/2008 1:34 AM  
Two things:

1. When you reference the "bgvoltage.scs" on the model libraries form, do [u]not[/u] specify a [i]section name[/i]. If you do this, it will expect the statistics block to be within a [i]library[/i] statement, which you don't have.
2. If you want mismatch to work, the voltage source to be within a subckt, as I said before. Essentially mismatch in spectre works by having a parameterized component within a subckt - the mismatch parameters are then made different for each subckt.

The specific problem you're describing here is (almost certainly) down to the first of the two above; I just wanted to mention the second as I don't want you to solve the first only to find that there is no mismatch!

Regards,

Andrew.
axp
Posts: 21
Online: User is Offline
6/19/2008 2:40 AM  
Great,

indeed it was caused by the first problem you described !!
Thanks for you help !!

Best regards
Posting to forums is available to community members only.
Login or Register
Forums > Custom IC > Custom IC Electrical Design > Addition of source with know statistical data


ActiveForums 3.6
     
Copyright 2006 Cadence Design Systems, Inc.