Designer’s Guide Community

Yutao Liu

Community Member

Offline

Posts: 76
Guangzhou, China

Re: How to simulate this circuit in Spectre???
Reply #15 - Apr 29^th, 2009, 1:10am

pancho_hideboo wrote on Apr 28^th, 2009, 9:09pm:

Yutao Liu wrote on Apr 28^th, 2009, 8:24pm:

attach is the netlists and the model of n18.

Both statements of parameter definition and statements of analysis don't exist. Angry

As I said to you repeatedly, no one except for you knows your specific situations.
What sizes on earth did you use as W and L for "n18" ? Angry

Show me complete netlists. e.g. "input.scs" if you use Cadence Spectre from ADE.

I am sorry for my mistake. :-[

input.rar is the input.scs file for my simulation.

And "op2 .scs" file listed inside is used to store the operating points while sweeping vds.
There is only one statement in "op2.scs", which is "save NM1:oppoint".

I hope information attached this time would be complete.

best regards

Back to top

input.rar

IP Logged

subgold

Community Member

Offline

Posts: 97

Re: How to simulate this circuit in Spectre???
Reply #16 - Apr 29^th, 2009, 1:30am

Yutao Liu wrote on Apr 29^th, 2009, 12:33am:

pancho_hideboo wrote on Apr 28^th, 2009, 9:09pm:

Yutao Liu wrote on Apr 28^th, 2009, 8:24pm:

attach is the netlists and the model of n18.

Both statements of parameter definition and statements of analysis don't exist. Angry

As I said to you repeatedly, no one except for you knows your specific situations.
What sizes on earth did you use as W and L for "n18" ? Angry

Show me complete netlists. e.g. "input.scs" if you use Cadence Spectre from ADE.

I am sorry for my mistake.

input.rar is the input.scs file for my simulation.

And "op2 .scs" file listed inside is used to store the operating points while sweeping vds.
There is only one statement in "op2.scs", which is "save NM1:oppoint".

I hope information attached this time would be complete.

best regards

first thing to try, do not define w and l as variable. specify them directly in the transistor property in the schematic.

Back to top

IP Logged

pancho_hideboo

Senior Fellow

Offline

Posts: 1424
Real Homeless

Re: How to simulate this circuit in Spectre???
Reply #17 - Apr 29^th, 2009, 1:38am

Yutao Liu wrote on Apr 29^th, 2009, 1:10am:

I hope information attached this time would be complete.

Still there are some unknown parameters like followings.
Are they all zero ?

Quote:

run Yutao_Liu.scs
.
Yutao_Liu.log

Cadence (R) Virtuoso (R) Spectre (R) Circuit Simulator
Version 6.2.0.493 -- 19 Sep 2007
Copyright (C) 1989-2007 Cadence Design Systems, Inc. All rights reserved
�worldwide. Cadence, Virtuoso and Spectre are registered trademarks of
�Cadence Design Systems, Inc. All others are the property of their
�respective holders.

Protected by U.S. Patents: 5,610,847; 5,790,436; 5,812,431; 5,859,785;
�5,949,992; 5,987,238; 6,088,523; 6,101,323; 6,151,698; 6,181,754;
�6,260,176; 6,278,964; 6,349,272; 6,374,390; 6,493,849; 6,504,885;
�6,618,837; 6,636,839; 6,778,025; 6,832,358; 6,851,097; 6,928,626;
�7,024,652; 7,035,782; 7,085,700; 7,143,021.

Includes RSA BSAFE(R) Cryptographic or Security Protocol Software from RSA
�Security, Inc.

Simulating `Yutao_Liu.scs' on lkenpc06 at 5:32:25 PM, Wed Apr 29, 2009.

Error found by spectre during hierarchy flattening.
� �ERROR (SFE-1999): "./n18.scs" 3: model `n18': parameter `tox': Unknown
�parameter name `dtox_n18' found in expression.
�
� �ERROR (SFE-1999): "./n18.scs" 3: model `n18': parameter `xl': Unknown
�parameter name `dxl_n18' found in expression.
�
� �ERROR (SFE-1999): "./n18.scs" 3: model `n18': parameter `xw': Unknown
�parameter name `dxw_n18' found in expression.
�
� �ERROR (SFE-1999): "./n18.scs" 3: model `n18': parameter `vth0': Unknown
�parameter name `dvth_n18' found in expression.
�
� �ERROR (SFE-1999): "./n18.scs" 3: model `n18': parameter `pvth0': Unknown
�parameter name `dpvth0_n18' found in expression.
�
spectre terminated prematurely due to fatal error.

Back to top

Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!!
http://www7.plala.or.jp/ungeromeppa/flash/kita.html
http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related

IP Logged

Yutao Liu

Community Member

Offline

Posts: 76
Guangzhou, China

Re: How to simulate this circuit in Spectre???
Reply #18 - Apr 29^th, 2009, 1:53am

subgold wrote on Apr 29^th, 2009, 1:30am:

Yutao Liu wrote on Apr 29^th, 2009, 12:33am:

pancho_hideboo wrote on Apr 28^th, 2009, 9:09pm:

Yutao Liu wrote on Apr 28^th, 2009, 8:24pm:

attach is the netlists and the model of n18.

Both statements of parameter definition and statements of analysis don't exist. Angry

As I said to you repeatedly, no one except for you knows your specific situations.
What sizes on earth did you use as W and L for "n18" ? Angry

Show me complete netlists. e.g. "input.scs" if you use Cadence Spectre from ADE.

I am sorry for my mistake.

input.rar is the input.scs file for my simulation.

And "op2 .scs" file listed inside is used to store the operating points while sweeping vds.
There is only one statement in "op2.scs", which is "save NM1:oppoint".

I hope information attached this time would be complete.

best regards

first thing to try, do not define w and l as variable. specify them directly in the transistor property in the schematic.

Thanks for subgold's suggestion.
I did this change before I change the w and l as variable. But the result did not change.
And when I run the simulation, the simulator warned me that "Vgs has exceeded the oxide breakdown voltage"
Dose this warning matter? If so, how should I change my simulation?

Back to top

IP Logged

Yutao Liu

Community Member

Offline

Posts: 76
Guangzhou, China

Re: How to simulate this circuit in Spectre???
Reply #19 - Apr 29^th, 2009, 2:07am

pancho_hideboo wrote on Apr 29^th, 2009, 1:38am:

Yutao Liu wrote on Apr 29^th, 2009, 1:10am:

I hope information attached this time would be complete.

Still there are some unknown parameters like followings.
Are they all zero ?

Quote:

run Yutao_Liu.scs
.
Yutao_Liu.log

Cadence (R) Virtuoso (R) Spectre (R) Circuit Simulator
Version 6.2.0.493 -- 19 Sep 2007
Copyright (C) 1989-2007 Cadence Design Systems, Inc. All rights reserved
�worldwide. Cadence, Virtuoso and Spectre are registered trademarks of
�Cadence Design Systems, Inc. All others are the property of their
�respective holders.

Protected by U.S. Patents: 5,610,847; 5,790,436; 5,812,431; 5,859,785;
�5,949,992; 5,987,238; 6,088,523; 6,101,323; 6,151,698; 6,181,754;
�6,260,176; 6,278,964; 6,349,272; 6,374,390; 6,493,849; 6,504,885;
�6,618,837; 6,636,839; 6,778,025; 6,832,358; 6,851,097; 6,928,626;
�7,024,652; 7,035,782; 7,085,700; 7,143,021.

Includes RSA BSAFE(R) Cryptographic or Security Protocol Software from RSA
�Security, Inc.

Simulating `Yutao_Liu.scs' on lkenpc06 at 5:32:25 PM, Wed Apr 29, 2009.

Error found by spectre during hierarchy flattening.
� �ERROR (SFE-1999): "./n18.scs" 3: model `n18': parameter `tox': Unknown
�parameter name `dtox_n18' found in expression.
�
� �ERROR (SFE-1999): "./n18.scs" 3: model `n18': parameter `xl': Unknown
�parameter name `dxl_n18' found in expression.
�
� �ERROR (SFE-1999): "./n18.scs" 3: model `n18': parameter `xw': Unknown
�parameter name `dxw_n18' found in expression.
�
� �ERROR (SFE-1999): "./n18.scs" 3: model `n18': parameter `vth0': Unknown
�parameter name `dvth_n18' found in expression.
�
� �ERROR (SFE-1999): "./n18.scs" 3: model `n18': parameter `pvth0': Unknown
�parameter name `dpvth0_n18' found in expression.
�
spectre terminated prematurely due to fatal error.

Oh, god! i forget to show you those datum again! Please forgive me!
Yes, those datum are all zero.
Please try this model file (attached) where all those datum have been set zero.

Thanks a lot.

Back to top

n18.rar

IP Logged

pancho_hideboo

Senior Fellow

Offline

Posts: 1424
Real Homeless

Re: How to simulate this circuit in Spectre???
Reply #20 - Apr 29^th, 2009, 4:31am

Attached is a method I suggested in http://www.designers-guide.org/Forum/YaBB.pl?num=1240322183/4#4
Your NMOS FET is connected to nodes, "d", "g", "s" and "GND".

From practical point of view, a method subgold suggested is more good because input signals of OPAmp is very small in my method.

Indeed I don't use any of the followings.
� - Testbench which sheldon showed
� - my suggestion
� - subgold suggestion

I use Agilent ADSsim(RFDE) for device characterizations.
Here I invoke optimizer with parametric sweep.

[Parametric Sweep of vds]
� � [Optimization of vgs for target Ids under vds]
[Final Analysis such as DCOP, SP, AC, Noise under seached bias conditions, vgs, vds, Ids]

The followings are non parametric sweep case.
http://www.designers-guide.org/Forum/YaBB.pl?num=1212376329/3#3
http://www.designers-guide.org/Forum/YaBB.pl?num=1203057659/7#7

As you said to us, testbench which sheldon showed don't seem to work correctly.
Later I will investigate causes.

Back to top

Yutao_Liu_FB.jpg

« Last Edit: Apr 29^th, 2009, 7:11am by pancho_hideboo »

Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!!
http://www7.plala.or.jp/ungeromeppa/flash/kita.html
http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related

IP Logged

subgold

Community Member

Offline

Posts: 97

Re: How to simulate this circuit in Spectre???
Reply #21 - Apr 29^th, 2009, 6:36am

Yutao Liu wrote on Apr 29^th, 2009, 1:53am:

subgold wrote on Apr 29^th, 2009, 1:30am:

Yutao Liu wrote on Apr 29^th, 2009, 12:33am:

pancho_hideboo wrote on Apr 28^th, 2009, 9:09pm:

Yutao Liu wrote on Apr 28^th, 2009, 8:24pm:

attach is the netlists and the model of n18.

Both statements of parameter definition and statements of analysis don't exist. Angry

As I said to you repeatedly, no one except for you knows your specific situations.
What sizes on earth did you use as W and L for "n18" ? Angry

Show me complete netlists. e.g. "input.scs" if you use Cadence Spectre from ADE.

I am sorry for my mistake.

input.rar is the input.scs file for my simulation.

And "op2 .scs" file listed inside is used to store the operating points while sweeping vds.
There is only one statement in "op2.scs", which is "save NM1:oppoint".

I hope information attached this time would be complete.

best regards

first thing to try, do not define w and l as variable. specify them directly in the transistor property in the schematic.

Thanks for subgold's suggestion.
I did this change before I change the w and l as variable. But the result did not change.
And when I run the simulation, the simulator warned me that �"Vgs has exceeded the oxide breakdown voltage"
Dose this warning matter? If so, how should I change my simulation?

i think the warning is exactly the problem. since your netlist looks fine, i think it is purely a simulator related problem, because everyting is ideal here, the cccs is also modeled as an ideal current source, which has very high impedance (seems to be 10^12ohm). therefore, with the current of the ideal current source, your gate voltage goes crazy and the correct dc operation points are never obtained.

try to clamp a diode there, with anode connected to the gate, and cathode connected to the max. allowed voltage (vdd), and see if it works.

Back to top

IP Logged

pancho_hideboo Senior Fellow Offline Posts: 1424 Real Homeless	Re: How to simulate this circuit in Spectre??? Reply #22 - Apr 29^th, 2009, 9:19pm This is a method which subgold suggested. Here I used Cadence Spectre.
Back to top	test_Yutao_Liu_2.JPG Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!! http://www7.plala.or.jp/ungeromeppa/flash/kita.html http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related IP Logged

pancho_hideboo Senior Fellow Offline Posts: 1424 Real Homeless	Re: How to simulate this circuit in Spectre??? Reply #23 - Apr 29^th, 2009, 10:07pm This is a result of Agilent ADSsim.
Back to top	test_Yutao_Liu_2_ADSsim.jpg Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!! http://www7.plala.or.jp/ungeromeppa/flash/kita.html http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related IP Logged

Yutao Liu

Community Member

Offline

Posts: 76
Guangzhou, China

Re: How to simulate this circuit in Spectre???
Reply #24 - Apr 30^th, 2009, 1:46am

pancho_hideboo wrote on Apr 29^th, 2009, 9:19pm:

This is a method which subgold suggested. Here I used Cadence Spectre.

Thanks for pancho_hideboo's reply.
The simulation results exactly meet what i want.

But I don't quite understand why the opamp in ahdlLib is able to achieve the result while the vcvs in analogLib fails, since both of them are used to make the drain voltage keep tracked with "Vds" while sweeping, and to stabilize the gate voltage?
What 's the difference between them?

Best regards!

Back to top

IP Logged

sheldon

Community Fellow

Offline

Posts: 751

Re: How to simulate this circuit in Spectre???
Reply #25 - Apr 30^th, 2009, 5:31am

Yutao,

If you want measure gm, why don't you limit the sweep range
to bias conditions where the device is in saturation? You are forcing
the Vds to be perfectly 0, vds=0, at the same time you are forcing
the transistor to conduct a finite current, ibias=40u. This condition
is not physical so the model and the testbench react non-physically.
If you sweep the Vds from 3.2V to 0V, you will see that the Vgs
becomes large as the Vds approaches 0 and that the curve starts
to break up at about Vd,sat. The op-amp model clamps at the supply
voltage so that the results look better. Also you will need to use
a different testbench to measure rds when Vds < Vds,sat.

Best Regards,

Sheldon

Back to top

Picture1.jpg

IP Logged

pancho_hideboo

Senior Fellow

Offline

Posts: 1424
Real Homeless

Re: How to simulate this circuit in Spectre???
Reply #26 - May 1^st, 2009, 4:51am

A method which subgold suggested is unreasonable for low Vds region.
A method which my suggested is more reasonable for low Vds region.

Indeed I don't use any of the followings.
- Testbench which sheldon showed
- my suggestion
- subgold suggestion

I use Agilent ADSsim(RFDE) for device characterizations.
Here I invoke optimizer with parametric sweep.

Attached figure is an example I'm using for device characterization, here I use SP-Analysis as FinalAnalysis of Optimizer.

[Parametric Sweep of Idrain ; Sweep2]
� [Parametric Sweep of Vds ; Sweep1]
� � � �[Optimization of Vgs for target Idrain under Vds ; Optim1 with DC1]
[SP Analysis as Final Analysis under seached bias conditions, Vgs, Vds, Idrain ; SP1]

This result is also reasonable for low Vds region.

Back to top

ADSsim_Optimizer_001.jpg

Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!!
http://www7.plala.or.jp/ungeromeppa/flash/kita.html
http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related

IP Logged

sheldon

Community Fellow

Offline

Posts: 751

Re: How to simulate this circuit in Spectre???
Reply #27 - May 1^st, 2009, 6:12am

Yutao,

� I am curious about your original testbench. I was looking at the
EE240 website lecture on MOS transistors and found the references
on these pages. Was this your original testbench the circuit described
on page 14?

https://www.eecs.berkeley.edu/~boser/courses/240_2004_sp/index.html

� � � � � � � � � � � � � � � � � � � � � � � � � � � � � � � � �Best Regards,

� � � � � � � � � � � � � � � � � � � � � � � � � � � � � � � � � � Sheldon

Back to top

IP Logged

Yutao Liu

Community Member

Offline

Posts: 76
Guangzhou, China

Re: How to simulate this circuit in Spectre???
Reply #28 - May 1^st, 2009, 6:47am

sheldon wrote on May 1^st, 2009, 6:12am:

Yutao,

� I am curious about your original testbench. I was looking at the
EE240 website lecture on MOS transistors and found the references
on these pages. Was this your original testbench the circuit described
on page 14?

https://www.eecs.berkeley.edu/~boser/courses/240_2004_sp/index.html

� � � � � � � � � � � � � � � � � � � � � � � � � � � � � � � � �Best Regards,

� � � � � � � � � � � � � � � � � � � � � � � � � � � � � � � � � � Sheldon

Sheldon,
Not on page 14, but on page 33 instead. And my reference is http://bwrc.eecs.berkeley.edu/classes/icdesign/ee240_s09/lectures/Lecture04_MOS_... on page 10.

I used the vcvs as the feedback opamp in spectre, and I failed.
I think the testbench that pancho_hideboo provided is feasible and the result looks the same as that on the notes.
But I still don't understand what difference between opamp in ahdlLib and vcvs in analogLib makes the simulation result different, even if I read your reply. Could you explain more clearly, please?
� � Best regards,
� �Yutao

Back to top

IP Logged

Yutao Liu

Community Member

Offline

Posts: 76
Guangzhou, China

Re: How to simulate this circuit in Spectre???
Reply #29 - May 1^st, 2009, 7:05am

pancho_hideboo wrote on Apr 29^th, 2009, 9:19pm:

This is a method which subgold suggested. Here I used Cadence Spectre.

Pancho_hideboo,
thanks for your work. I think your testbench is feasible and the result looks reliable.
I have tried your testbench in spectre, the result looks the same as yours basically, but discontinuity exist when vds is in low region, as shown below. My schematic and the setting of the opamp is totally the same as you described above. Do you have any idea what makes the discontinuity?
Thanks.

Best regards

yutao

Back to top

scheme_005.PNG

IP Logged