LTSpice questions

[Walter Harley]

Two LTSpice questions that maybe someone can help me with.

First: when I do a transient analysis, I get nice little "voltage probe" and
"current probe" tools that I can use to click on a component or a node and
add a trace. Easy, fast. When I simulate DC operating point, it gives me a
popup window with all the DC voltages and currents listed; when I close this
window, I can still poke around with the cursor and see voltages. BUT: I
can't see currents this way. So,

Q1: Is there any way to be able to conveniently view currents on my
schematic, after simulating DC operating point?

Second: I've added the Supertex MOSFET library into my LTSpice
"standard.mos" library. It seems to recognize them for the purposes of
simulation. However, in the "pick a MOSFET" dialog, I can't get any of the
parameters like Rds(on), Vgs, etc. to show up in the list. LTSpice's
built-in MOSFETs work, but the ones I added don't. So,

Q2: Does anyone know how to get third-party MOSFET models to show their
parameters in the "pick a MOSFET" list?

Thanks,
-walter

 

[Helmut Sennewald]

Two LTSpice questions that maybe someone can help me with.

First: when I do a transient analysis, I get nice little "voltage probe" and
"current probe" tools that I can use to click on a component or a node and
add a trace. Easy, fast. When I simulate DC operating point, it gives me a
popup window with all the DC voltages and currents listed; when I close this
window, I can still poke around with the cursor and see voltages. BUT: I
can't see currents this way. So,

Q1: Is there any way to be able to conveniently view currents on my
schematic, after simulating DC operating point?

Hello Walter,
you should see the current when you move the cursor over a resistor for
example. If you move the cursor exactly over the beginning of a transistor
pin, then you should get the current displayed flowing into that pin.

Second: I've added the Supertex MOSFET library into my LTSpice
"standard.mos" library. It seems to recognize them for the purposes of
simulation. However, in the "pick a MOSFET" dialog, I can't get any of the
parameters like Rds(on), Vgs, etc. to show up in the list. LTSpice's
built-in MOSFETs work, but the ones I added don't. So,

Q2: Does anyone know how to get third-party MOSFET models to show their
parameters in the "pick a MOSFET" list?

Here is an example which I tried for you.
There is no specification for Qg in the datasheet, so I set it to 0.
Everey time you see then 0 there it just means not given. You can also omit
the Qg=xx information in the file. LTSPICE shows then Qg=0 in the pick list.
The information mfg=Supertex Vds=60 Ron=3 Qg=0 must be read from the
datsheet. It is not derived from the SPICE paramter.


..MODEL 2N6660 NMOS (LEVEL=3 RS=0.36 NSUB=1.0E15
+DELTA=0.1 KAPPA=0.0506 TPG=1 CGDO=6.343E-10
+RD=0.43 VTO=1.600 VMAX=1.0E7 ETA=0.0223089
+NFS=6.6E10 TOX=1.0E-7 LD=1.698E-9 UO=862.425
+XJ=6.4666E-7 THETA=1.0E-5 CGSO=9.09E-9 L=2.5E-6
+W=5.0E-3 mfg=Supertex Vds=60 Ron=3 Qg=0)

Best Regards
Helmut

PS: I have tested with version 2.06u .

 

[Walter Harley]

you should see the current when you move the cursor over a resistor for
example. If you move the cursor exactly over the beginning of a transistor
pin, then you should get the current displayed flowing into that pin.

Thanks, Helmut! I don't know why I didn't see that before, but it works
fine.

Here is an example which I tried for you.
There is no specification for Qg in the datasheet, so I set it to 0.
Everey time you see then 0 there it just means not given. You can also omit
the Qg=xx information in the file. LTSPICE shows then Qg=0 in the pick list.
The information mfg=Supertex Vds=60 Ron=3 Qg=0 must be read from the
datsheet. It is not derived from the SPICE paramter.

.MODEL 2N6660 NMOS (LEVEL=3 RS=0.36 NSUB=1.0E15
+DELTA=0.1 KAPPA=0.0506 TPG=1 CGDO=6.343E-10
+RD=0.43 VTO=1.600 VMAX=1.0E7 ETA=0.0223089
+NFS=6.6E10 TOX=1.0E-7 LD=1.698E-9 UO=862.425
+XJ=6.4666E-7 THETA=1.0E-5 CGSO=9.09E-9 L=2.5E-6
+W=5.0E-3 mfg=Supertex Vds=60 Ron=3 Qg=0)

When I try that, it shows up properly in the list, which is great; thanks
again.

I do, however, get some (nonfatal) warning messages in the simulation:
Unrecognized parameter "mfg" - ignored
Unrecognized parameter "supertex" - ignored
Unrecognized parameter "vds" - ignored
Unrecognized parameter "ron" - ignored
Unrecognized parameter "qg" - ignored

Do you get that also? I'm using v2.06u, like you.

-walter

 

[Helmut Sennewald]

...

When I try that, it shows up properly in the list, which is great; thanks
again.

I do, however, get some (nonfatal) warning messages in the simulation:
Unrecognized parameter "mfg" - ignored
Unrecognized parameter "supertex" - ignored
Unrecognized parameter "vds" - ignored
Unrecognized parameter "ron" - ignored
Unrecognized parameter "qg" - ignored

Do you get that also? I'm using v2.06u, like you.

Hello Walter,
sorry, I have overlooked that. I have checked it now and I see the same
warnings.
It seems that these non-SPICE parameters are only allowed for VDMOS models,
but not for NMOS(PMOS?). I have forwarded this message to Mike Engelhardt
too.
Maybe he can correct it in one of the next releases.

Best Regards
Helmut