Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Cadence Spice level Problem

Status
Not open for further replies.

suhas_shiv

Full Member level 2
Joined
Nov 30, 2005
Messages
136
Helped
11
Reputation
22
Reaction score
4
Trophy points
1,298
Activity points
2,461
is model level 49 supported by cadence

I am using the TSMC 0.18um model files. When I run the simulator I get an error which says level=49 not supported. I think this is the spice level parameter mentioned in the model file.
Just to see if it works fine, I changed the level to 11 and it seems to work. Is this ok for simulating(are the results going to differ a lot from level 49)? If not, how can I make the tool work for level=49?

I am using version IC5141.

Appreciate any inputs on this. Thanks.
 

paulux

Advanced Member level 4
Joined
May 16, 2005
Messages
112
Helped
11
Reputation
22
Reaction score
2
Trophy points
1,298
Activity points
2,339
is model level 49 supported by cadence

If TSMC could guarantee the result of changing spice level, that's OK. In general, if your simulation does not require accurate results or it is just DC performance, I guess it is OK. Otherwise, the result may be different.
 

Chethan

Full Member level 3
Joined
Jul 11, 2005
Messages
173
Helped
20
Reputation
40
Reaction score
12
Trophy points
1,298
Location
Bangalore
Activity points
2,837
cadence hspices

suhas_shiv said:
I am using the TSMC 0.18um model files. When I run the simulator I get an error which says level=49 not supported. I think this is the spice level parameter mentioned in the model file.
Just to see if it works fine, I changed the level to 11 and it seems to work. Is this ok for simulating(are the results going to differ a lot from level 49)? If not, how can I make the tool work for level=49?

I am using version IC5141.

Appreciate any inputs on this. Thanks.

Hi
When u r running HSPICE then level=49 is supported.But when u r using spectre then change the level to level=11. Both HSPICE and spectre results are compatible.If u r using Simetrix then keep the level as Level = 49.If this has helped u , then press the helped me button, it doesnt cost u any points.
 

vss

Newbie level 1
Joined
Jan 7, 2006
Messages
1
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,294
cadence spectre change bsim level

Hey,
The results of the simulation may vary drastically depending on the type of design and simulation you are running. If you consider the BSIM levels 11 and 49 there would be a a lot of change. Many new parameters are added to emulate new effects. So, don't take the results to be granted if your design is complicated enough and that it needs high accuracy.

For model compatibility check for the presence of necessary model cards in the library.

VSS
 

Bilgin Metin

Newbie level 3
Joined
Jan 6, 2006
Messages
4
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,312
cadence 16 model level 49

By changing level 49 to level 8 you can use winspice instead of Pspice. Pspice works with level 1-3 only
 

Amuro

Full Member level 4
Joined
Mar 15, 2002
Messages
194
Helped
8
Reputation
16
Reaction score
5
Trophy points
1,298
Location
Thailand
Activity points
1,700
level 49 level 7 spice

Bilgin Metin said:
By changing level 49 to level 8 you can use winspice instead of Pspice. Pspice works with level 1-3 only

Level 7 in Pspice is equivalent to level 49 in Hspice and bsim3v3 in Spectre.
 

jcpu

Full Member level 4
Joined
Dec 17, 2005
Messages
215
Helped
18
Reputation
36
Reaction score
6
Trophy points
1,298
Activity points
2,968
spice level 1

Dear Suhas:

In case you are seriously working upon this project.
The best way is to ask a Spectre model of this process
formally from the foundry. So that model parameters shall
be gauranteed to their best knowledge.

"Changing model parameters is highly risky"
considering hundreds of thousands of maskset and wafer fee.
Unless the simulation is just an college homework.

Best Regards,
jcpu
 
  • Like
Reactions: santom

    santom

    Points: 2
    Helpful Answer Positive Rating

santom

Full Member level 2
Joined
Sep 8, 2007
Messages
143
Helped
2
Reputation
4
Reaction score
2
Trophy points
1,298
Activity points
2,262
Re: spice level 1

Dear Suhas:

In case you are seriously working upon this project.
The best way is to ask a Spectre model of this process
formally from the foundry. So that model parameters shall
be gauranteed to their best knowledge.

"Changing model parameters is highly risky"
considering hundreds of thousands of maskset and wafer fee.
Unless the simulation is just an college homework.

Best Regards,
jcpu


I completely agree with the user jcpu.His/Her comment is so right when it comes to check the transistor for new LEVEL. Its just not a matter of changing the LEVEL number in the SPICE file as there is a pure technology called Device Modeling behind this single word LEVEL. So try using the right level number once you are sure that you have that LEVEL inbuilt in your CAD environment.

Santom
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top