How to get the values defined in BSIM3 directly from Hspice?

bsim3 abulk value

Dear all,

I have a question about the BSIM3v3 model and Hspice:

For some calculations, I need to know some parameters such as Esat, µeff, Abulk ... that are defined in BSIM3v3, however, it is really hard to calculate such parameter values by hand, coz all of the equations involve too many other parameters... and one leads to another, just too complicated...

I'm wondering that whether or not I can use Hspice to do such a job, but I still can not figure out how to output such parameters...

Can anyone here help me out?

Thank you!

L2F

Re: How to get the values defined in BSIM3 directly from Hsp

Hi, You want to make a transformation between your model BSIM3v3 HSPICE to BSIMv3 ADS?

regards.

Re: How to get the values defined in BSIM3 directly from Hsp

Frank_H said:

Hi, You want to make a transformation between your model BSIM3v3 HSPICE to BSIMv3 @DS?

regards.

Click to expand...

No, not really. As a matter of fact, I have the ADS model provided by the foundry. I just need those parameters for some calculations.

BTW, Do you know how to get those parameters in ADS?

Thanks,

L2F

Re: How to get the values defined in BSIM3 directly from Hsp

You can simulate a single transistor in Hspice and get almost every model parameters. command .OP and DC sweep will do this job. For example, wanna get Ueff(effective mobility) of M1, just use: .probe dc ubeff(M1). Also gmo(m1) means transconductance of m1, vdsat(m1) is ..., I think you should know this : )
Sometimes maybe you don't know how to name the paramters of MOSFET in hspice, just find help from SPICE manual. Best regards.
By the way, ADS or other simulators can also do this job.

Re: How to get the values defined in BSIM3 directly from Hsp

flamingo said:

You can simulate a single transistor in Hspice and get almost every model parameters. command .OP and DC sweep will do this job. For example, wanna get Ueff(effective mobility) of M1, just use: .probe dc ubeff(M1). Also gmo(m1) means transconductance of m1, vdsat(m1) is ..., I think you should know this : )
Sometimes maybe you don't know how to name the paramters of MOSFET in hspice, just find help from SPICE manual. Best regards.
By the way, @DS or other simulators can also do this job.

Click to expand...

Hi, Flamingo,

Thank you very much for your reply, it is true that Hspice and ADS both can indicate almost all the model parameters, but they are actually not the ones I'm expecting (please check the equations I attached). The parameters you mentioned probably are listed in the .lis file, e.g.,

element 0:m1
model 0:cmosn
region Saturati
id 19.7815u
ibs 0.
ibd 0.
vgs 700.0000m
vds 1.0000
vbs 0.
vth 508.9218m
vdsat 158.4333m
beta 917.7711u
gam eff 422.1155m
gm 178.8971u
gds 6.1316u
gmb 36.0394u
cdtot 706.1121a
cgtot 2.9680f
cstot 1.4815f
cbtot 387.5707a
cgs 2.1692f
cgd 697.0264a

Actually I need something defined in BSIM3v3, like ueff, esat(ecrit) ... which are calculated with equations! not in the .model sentense or in the summary of .lis file!

I wish to get more info. from you, thanks,

L2F

Re: How to get the values defined in BSIM3 directly from Hsp

OK, maybe I am not get the point.
you want to get Esat, µeff, Abulk from simulator, right?
These parameters belong to the semifinished products during shifting the device model to mosfet paramters, so maybe some of them are invisible in simulator's output.
I have checked the spice manual, unfortunely only ueff can be directly gotten from simulator. Just as what I have mentioned above: do dc analysis, and then .probe dc ueff(M*).
The other two paramters Esat and Abulk can't be read dirtectly from simulator. Maybe the only way is to do hand calculations. By the way these paramters are changeable with different sizes, different work conditions of transistor, so it is not recommanded to calc other parameters using one of fixed value of Esat, µeff, Abulk.