BSimv3 or supper simulator (free)

Hi there!
Can you suggest me, if any, an analog simulation environment or simulator for Windows (different than OrCAD), compatible with BSimv3 or upper, and free or with student or shareware version?

Is OrCAD (PSpice) compatible?

LTspice

https://www.linear.com/designtools/software/

Thank you!
However, i can't manage to add my libs... i placed the model in the MOS file...LTspice can find my models...however i can't customize W and L and multiplicity...

can I do it with LTSpice?

does it support LEVEL 7 models?

need some help...

Just click right button on mos symbol on your schematic. Another window pops up. you can change model name, W/L, M also.
And it supports BSIM3V3 (level 7)

uhm i can't... only Vds and Rds(on) come out, as for discrete components.
I tried my .lib with PSpice and W, L and other came out.
I don't know why they do not appear.
Maybe i've to write directly the netlist?

Added after 24 minutes:

ok no problem, i've found it! Just, i need to use the 4 terminals MOS.

ORCAD Pspice works well with BSIM3 (Level 7). In the case that you are using BSIM3 level 49 (HSPICE), then you will need to change certain parameters in your model file and convert it to level 7. You can refer to the following link for more details how to do the conversion.

https://www.mosis.com/Faqs/pspice.pdf

For PSPICE simulation using BSIM3(Level7), you can instantiate MOS devices from the 'Breakout.olb' library (MBreakP, MBreakP3 --> for PMOS and MBreakN, MBreakN3 --> for NMOS). You need to make a slight modification in the component properties so that your simulator can recognise the model file you are using.

To do this:
> Once you have instantiated the MOS Device, right-click on the component and go to 'edit properties'.
> Then edit the implementation to your model file component name.
For example: If in your model file the NMOS device is .NMOS, then in the edit properties, change the name to NMOS to match your model file.

Good Luck

One more tip,

If you want to use level49(Hspice model) for LTspice, you've better change these.

WINT=WINT (old one) - 0.5*XW
LINT=LINT (old one) -0.5 *XL

for example,

if your level49 model is like that,

....
....
+NCH = 8.8286E+16 LLN = 1 LWN = 1
+WLN = 1 WWN = 1 LINT = 6.3E-08
+LL = 0 LW = 0 LWL = 0
+WINT = 0 WL = 0 WW = 0
+WWL = 0 MOBMOD = 1 BINUNIT = 2
+XL =-3E-08 XW=1E-08 ACM = 12
....
....

Click to expand...

after changing,

....
....
+NCH = 8.8286E+16 LLN = 1 LWN = 1
+WLN = 1 WWN = 1 LINT = 7.8E-08
+LL = 0 LW = 0 LWL = 0
+WINT = 0.5E-0.8 WL = 0 WW = 0
+WWL = 0 MOBMOD = 1 BINUNIT = 2
+XL =-3E-08 XW=1E-08 ACM = 12
....
....

Click to expand...

k1gunner said:

One more tip,

If you want to use level49(Hspice model) for LTspice, you've better change these.

WINT=WINT (old one) - 0.5*XW
LINT=LINT (old one) -0.5 *XL

for example,

if your level49 model is like that,

....
....
+NCH = 8.8286E+16 LLN = 1 LWN = 1
+WLN = 1 WWN = 1 LINT = 6.3E-08
+LL = 0 LW = 0 LWL = 0
+WINT = 0 WL = 0 WW = 0
+WWL = 0 MOBMOD = 1 BINUNIT = 2
+XL =-3E-08 XW=1E-08 ACM = 12
....
....

Click to expand...

after changing,

....
....
+NCH = 8.8286E+16 LLN = 1 LWN = 1
+WLN = 1 WWN = 1 LINT = 7.8E-08
+LL = 0 LW = 0 LWL = 0
+WINT = 0.5E-0.8 WL = 0 WW = 0
+WWL = 0 MOBMOD = 1 BINUNIT = 2
+XL =-3E-08 XW=1E-08 ACM = 12
....
....

Click to expand...

Click to expand...

thank you!
i've read that if i use HSPICE models (level 49), it's okay for BSIM3v3.0.0 isn't it?