Continue to Site

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.

How to convert MOSIS HSpice to PSpice, for most accurate results?

Status
Not open for further replies.

Alsat

Newbie level 3
Newbie level 3
Joined
Mar 10, 2015
Messages
4
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Visit site
Activity points
31
I am doing some research about transconductors. I am using OrCAD 16.6 Lite version for my simulations. Model that I am using in my simulations is TSMC 0.35um V01C. That model is optimized for HSpice, but I need it for PSpice. I only changed LEVEL from 49 to 7, and it is working, I get results (results are in expected limits), but with warnings:
1) Using BSIM3 version 3.1 or lower
2) AD=0, AS=0, PD=0, PS=0A

After that, I set: AD=AS=W*L, and PD=PS=2*(W+L). I think I got better results with this setup (better accuracy). Still don't know which values to use for NRD,NRS,NRG,NRB, are these values for number of contacts necessary?

Other try was with LEVEL=8, it works without errors, but I think results are not good enough in AC analysis.

My questions is: How to properly convert HSpice to PSpice in order to get most accurate results in OrCAD PSpice? Or what You suggest to do for better accuracy?

I didn't find answer in similar posts.

Thanks beforehand.
 

Yes, I tried that tips already, they can be found on MOSIS website (FAQs section). I deleted XW and XL parameters and write new values for WINT and LINT. I am in doubt, what results will be more accurate with AD,AS,PD,PS as zero or non-zero value.

Can someone give opinion **broken link removed** for parameters?
 

I am in doubt, what results will be more accurate with AD,AS,PD,PS as zero or non-zero value.
You better use the right area and periphery values - if available from layout - otherwise use the estimations from given below. These are necessary to calculate good (i.e. as correct as possible) capacitance values by the simulator tool, which on their part affect the ac and transient analysis results.

Can someone give opinion **broken link removed** for parameters?

In absence of layout information, you can use 2Lmin to be junction length (i.e. 0.36µm in a 0.18µm technology) and set ad = as = 2WLmin and pd = ps = 2(W+2Lmin).

Analog circuits in most cases use L > Lmin; in any case use the real L instead of Lmin for the AD,AS,PD,PS values!

Some size extractors use pd = ps = W+4L instead of the equation given above, because one side of the source resp. drain width's capacitance is already considered by the gate capacitance in the transistor model, s. also this post and following ones.
 
  • Like
Reactions: Alsat

    Alsat

    Points: 2
    Helpful Answer Positive Rating
Problem is, that I don't know right areas. Because of that, I need as correct as possible values for AD,AS,PD,PS for my simulations. In my design, I don't have any length over 0.8um. I read the post, that You suggested, and I am really in doubt now, which values to use? What would You suggest?
 

In your case I'd suggest you keep the zero values for the 4 area & perimeter parameters: in such case, all the SPICE-flavour tools calculate "best known" values for these parameters from the given W & L values, and consider these values for the capacitances calculation.
 
  • Like
Reactions: Alsat

    Alsat

    Points: 2
    Helpful Answer Positive Rating
Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top