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

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.

Did you already try these tips?

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?

Alsat said:

I am in doubt, what results will be more accurate with AD,AS,PD,PS as zero or non-zero value.

Click to expand...

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.

Alsat said:

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

Click to expand...

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

Click to expand...

Analog circuits in most cases use L > L_min; in any case use the real L instead of L_min 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.

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.

Thank You for suggestion, I will go that way.