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 > Shared code - SKILL

Subject: Saving all operating point data for swept simulations
Posting to forums is available to community members only.
Login or Register
Rate this topic:
   
Author Messages
mballini
Posts: 6
Online: User is Offline
6/13/2008 1:37 PM  
I would like to make plots of gm over Id and I'd like to do that from a SKILL/OCEAN script. I am quite new to cadence and almost completely new to SKILL, so please forgive if some questions have obvious answers.

My problem is that I can only have access to the gm value for the bsim model for the DC operating point, not for all the values.

--------------------------------------------------------------------------------------
; Here's how I set up the analysis:
ocnWaveformTool('wavescan)
simulator('spectre)
design(library cell "schematic")
createNetlist(?recreateAll t ?display nil)
resultsDir(strcat("/local0/scratch/ballinim/xh035/" cell "/spectre/schematic" ))
modelFile(
    '("/usr/local/vlsi/cds/Design_Kits/XFAB_XH035_v3_1/spectre/xh035/mos/param.scs" "3s")
    '("/usr/local/vlsi/cds/Design_Kits/XFAB_XH035_v3_1/spectre/xh035/mos/bip.scs" "tm")
    '("/usr/local/vlsi/cds/Design_Kits/XFAB_XH035_v3_1/spectre/xh035/mos/bsim3v3.scs" "tm")
    '("/usr/local/vlsi/cds/Design_Kits/XFAB_XH035_v3_1/spectre/xh035/mos/cap.scs" "tm")
    '("/usr/local/vlsi/cds/Design_Kits/XFAB_XH035_v3_1/spectre/xh035/mos/dio.scs" "tm")
    '("/usr/local/vlsi/cds/Design_Kits/XFAB_XH035_v3_1/spectre/xh035/mos/ind.scs" "tm")
    '("/usr/local/vlsi/cds/Design_Kits/XFAB_XH035_v3_1/spectre/xh035/mos/res.scs" "tm")
)
saveOption( 'currents "all" )
save('i "/Mn/S" "/Mn/D" "/Mp/S" "/Mp/D")
analysis('dc ?saveOppoint t  ?param "vg"  ?start "0" ?stop "3.3" ?values 0.5
         ?write "spectre.dc"  ?oppoint "rawfile"  ?maxiters "150" ?maxsteps "10000" 
         ?annotate "status"  ?threshold "0.0"  ?detail "node" ?sort "name"  )
temp( 27 )
run()

; Here's how I get a single value for gm
gmoverid = pv("Mn.m1" "gmoverid" ?result "dcOpInfo-info")
printf("gmoverid = %g\n" gmoverid)

; For currents and voltages I get the values for the whole sweep range
id = i("Mn:1" ?result "dc-dc")
vg = v("/vgn" ?result "dc-dc")
---------------------------------------------------------------------------------------------

How can I get the value of gmoverid for the whole swept range?

I thought about these possibilities:

1) gmoverid = deriv(id)/id
 but I'm not even sure this is correct because I do not know the bsim model so well.

2) I read somewhere I can specify to spectre to save those things by adding a file with the following text to the model libraries: "save Mn:oppoint". Is there a way to invoke that spectre command directly from the script without writing a file?

3) Iterating the DC analysis with loop. How can I construct a loop for, say, linearly spaced values? In C I would use the for(vg=0;vg < 3.3; vg+=0.1){} construct, but I don't know how to do that in SKILL. I think I could use foreach, but I don't know how to (easily and compactly) creating the list of values. I also think this approach would be slower.

Can please give suggestion?

Thanks.
Marco Ballini
adbeckett
Posts: 248
Online: User is Offline
6/16/2008 10:53 AM  
If using a recent MMSIM version (e.g. MMSIM70, or MMSIM62 - I think you may need MMSIM62 Update 1), you can use wildcards in save statements.

So you can create an include file, and put:

save *:oppoint

or

save *:gmoverid

This eans it's the same include file for all circuits - no need to change it for different transistors.
mballini
Posts: 6
Online: User is Offline
6/16/2008 11:00 AM  
Thank you for your answer.
I actually don't know what MMSIM is.
However I need to do that from inside an OCEAN script.
How can I do it?
What is an include file and what is the syntax to include?
sorry but I am bit lost...
thanks again
mb
adbeckett
Posts: 248
Online: User is Offline
6/16/2008 1:17 PM  
Apologies - I had a problem with my computer earlier, and so didn't quite complete my post before sending.

Anyway, let's answer some questions:

1. MMSIM. Originally spectre was released as part of the "IC" release stream (e.g. IC5141). Some time ago, we (Cadence) made the decision to separate it from the IC stream, and release it in its own stream alongside Ultrasim. Simulators tend to advance more rapidly than the environment does (new models, analyses, etc), and so releasing it separately made sense. So whilst spectre is still in IC5141 (we couldn't take it away having released it in IC5141), it is not part of any later IC releases (ICOA5251, IC61), but instead you need to install an "MMSIM" release (e.g. MMSIM60, MMSIM61, MMSIM62 or MMSIM70). The last two of this list are the current releases.
2. Wildcards. Support for wildcards was added in MMSIM62 and MMSIM70. See "spectre -h save" for details on the syntax
3. Include files. Create a text file (give it a ".scs" suffix so spectre knows it is in spectre rather than SPICE syntax), containing one of the statements I mention in my previous post, save it, and then in ADE you can reference it as a file in the model libraries form.
4. For OCEAN, you could save the OCEAN script from ADE to see what that looks like, or just add another line in your modelFile() call:
"/path/to/your/saveFile.scs"
(don't give a section name, because it's just a straight file include).

I suggest you have a good look at the documentation - in IC5141 this is started with "cdsdoc"; in IC61 and MMSIM62/70 it's started with "cdnshelp".

Regards,

Andrew.
Posting to forums is available to community members only.
Login or Register
Forums > Custom IC > Shared code - SKILL > Saving all operating point data for swept simulations


ActiveForums 3.6
     
Copyright 2006 Cadence Design Systems, Inc.