H2 implement mosfet spice model level 3 into multisim or h2 convert level 3 to 1

[mluhn]

I am curently try to define dual gate mosfet BF998 or BF 994.

But I have only spice models level 3, which seems to be not supported by multisim.
Consequently I am looking for procedures to implement level 3 mosfet model into Multisim

or

how to translate mosfet level 3 into level 1 model

or

does somebody know mosfet level 1 defined models for BF998, BF 996 or BF994.

[lacy]

II have a BF998 in my Master Database. I will post a schematic with the part on it and you can save it to your user database. I have included the model file just in case you have a different version of Multisim.

.SUBCKT BF998 1 2 3 4
L10          1 10   0.12N
L20          2 20   0.12N
L30          3 30   0.12N
L40          4 40   0.12N
L11         10 11   1.20N
L21         20 21   1.20N
L31         30 31   1.20N
L41         40 41   1.20N
C13         10 30   0.085P
C14         10 40   0.085P
C21         10 20   0.017P
C23         20 30   0.085P
C24         20 40   0.005P
D11         42 11   ZENER
D12         42 41   ZENER
D21         32 11   ZENER
D22         32 31   ZENER
RS          10 12   100
MOS1        61 41 11 12 GATE1 L=1.1E-6 W=1150E-6
MOS2        21 31 61 12 GATE2 L=2.0E-6 W=1150E-6

.MODEL  ZENER  D ( BV=10 CJO=1.2E-12  RS=10)

.MODEL  GATE1
+  NMOS ( LEVEL=3 UO=600  VTO=-0.250 NFS=300E9 TOX=42E-9
+  NSUB=3E15 VMAX=140E3 RS=2.0 RD=2.0 XJ=200E-9 THETA=0.11
+  ETA=0.06 KAPPA=2 LD=0.1E-6
+  CGSO=0.3E-9 CGDO=0.3E-9 CBD=0.5E-12 CBS=0.5E-12)

.MODEL  GATE2
+  NMOS ( LEVEL=3 UO=600  VTO=-0.250 NFS=300E9 TOX=42E-9
+  NSUB=3E15  VMAX=100E3 RS=2.0 RD=2.0 XJ=200E-9 THETA=0.11
+  ETA=0.06  KAPPA=2 LD=0.1E-6
+  CGSO=0.3E-9 CGDO=0.3E-9 CBD=0.5E-12 CBS=0.5E-12)

.ENDS BF998

Based on the model above I would say that Multisim does support Level 3 Models. If you have other models that you wish to put into Multisim then maybe you can use this model file in order to get the syntax right to where Multisim will accept it.

I hope this help you.

Message Edited by lacy on 10-31-2007 07:40 PM

[mluhn]

Lacy,

I regret to tell you, that it does not work. I am using multisim 2001, be so
kind and resend your BF998.ms10 file in version *.msm (2001).
Attached I share with you my spice model code based on your input, maybe
you can see what is wrong.

Thanks for your support.

[lacy]

O.K. Sorry about that. I do Have both 2001 amd Version 10. I did have this component also in my 2001 Database. It is the same model as is in Version 10 That I posted in the above post. You can take that model and create a component with it. Unfortunately, I don't see a way of putting in a schematic so you can save it to your database since I  don't believe 2001 has that feature (or at least I can't find it).

The problem with the model you posted is this: 2001 is very contrary on it's model files. The first thing it must see is the .SUBCKT statement otherwise it will not work. In your model for your component there were comments before the .SUBCKT statement. These must be deleted up to the .SUBCKT Statement in order for Multisim to recongize the model file. This has always been the case when I put model into it including one's that I created with Multisim 2001. For some reason these pre-subckt comments cause problems even though they are supposed to be ignored.

You can just take my model file and copy it and paste it into your component as is and it should work.

[Peiyun]

Hi, I have the similar question too. How should i import the spice model of this Infineon IGBT into Multisim library?

Because what i realized is Infineon Spice model is using Level 3 whereas Multisim is using Level 1.

[orugo]

Hi could you please tell is there any model for organic thin film transistor