Sweeping Vth vs L

I tried in that version of spectre, and it also works.

There's no requirement that you have to run this from the command line - it should work fine from ADE too. I just did it from a netlist because it was quicker for me to throw together an example. Can you share the netlist that you are getting in ADE? Also show the results browser as a screenshot (use the Options tab to attach a picture).

Regards,

Andrew.

I have connected just one transistor with two vdc's. In the transistor edit object properties length i have given "length". In ADE L i copied the variables from the cell view. Clicked dc analysis and selected design variable under sweep. Selected the variable name "length". Gave start and stop values. Ran the simulation. I also selected the file mysave.scs in the model library which contains the command as given by you in previous post save *.all devtype=bsim4. 

After i am running the simulation there was no warning and error. I went to results browser and selected dc-dc. I couldnt see the vth of the transistor. I have attached the image with this post describing the things i have done. 

OK, but you didn't post the input.scs (the netlist) which is what I wanted to see...

Andrew.

You still didn't show the input.scs (Simulation->Netlist->Display in ADE will show this). Also, paste the contents rather than a screen grab please. You show your include file as "mysave" rather than "mysave.scs" - does it have a ".scs" suffix?

Andrew.

This is what i get from simulation-->netlist-->display. I dont know how to show include file as mysave rather than mysave.scs. Also uploaded the sceenshot

 // Generated for: spectre

// Generated on: Aug  6 19:09:59 2014

// Design library name: Vref

// Design cell name: test

// Design view name: schematic

simulator lang=spectre

global 0

include "/home/palaniapy13/mysave.scs"

include "models.scs"

parameters length=1

// Library name: Vref

// Cell name: test

// View name: schematic

M0 (net6 net3 0 0) nlvtlp w=0.135 l=length nfing=1 mult=1 srcefirst=1 \

        ngcon=1 mismatch=1 lpe=0 dnoise_mdev=0 dmu_mdev=0 dvt_mdev=0

V4 (net3 0) vsource dc=1 type=dc

V5 (net6 0) vsource dc=1 type=dc

simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \

    tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \

    digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \

    checklimitdest=psf 

dcOp dc write="spectre.dc" maxiters=150 maxsteps=10000 annotate=status

dcOpInfo info what=oppoint where=rawfile

dc dc param=length start=0.5 stop=10 lin=10 oppoint=rawfile maxiters=150 \

    maxsteps=10000 annotate=status

modelParameter info what=models where=rawfile

element info what=inst where=rawfile

outputParameter info what=output where=rawfile

designParamVals info what=parameters where=rawfile

primitives info what=primitives where=rawfile

subckts info what=subckts  where=rawfile

saveOptions options save=allpub subcktprobelvl=2

I just realised what you problem was after trying loads of different things. I noticed from your screen grab that you had "save *.all" rather than "save *:all" (i.e. dot rather than colon).

That would explain it.

Andrew.

Corrected that mistake and now i can plot Vth vs L . Thank you so much for patiently answering all my queries and helping me. Thanks again. 

Regards

Arjun 

Hi,

Is there any way to find the Mobility and Cox of the transistor in cadence ?. I am studying about Voltage References. I want to sweep Mobility and Cox with respect to temperature and length. By this way i can learn better about the transistor characteristics ? Please help me.