PSPICE mosfet sim

[technogeek]

Some quick questions.....

I'm using a voltage controlled switch to model a mosfet in pspice.

VCTRL 10 0 PULSE(0V 5V 0 100nS 100nS 1900nS 5000nS)
.MODEL SWP VSWITCH(VON=5V VOFF=0V RON=0.5 ROFF=1MEG)

I am averaging the (current * voltage) through the switch to calculate average power dissipation. Now I have a question about how they relate specifically to the mosfets and mosfet drivers....

The driver I have has a gate Trise of 50ns max, Tfall of 50ns max.

The mosfet has a rise/fall transition time of 20ns.

Should the rise/fall time of the voltage controlled switch be 20ns? 50ns? 70ns?

 

[Sceadwian]

Why are you using a voltage controlled switch to model a mosfet? It's not going to model the gate/source voltage or the non-linearity, or any of the mosfets other charactoristics properly.

 

[Optikon]

Why are you using a voltage controlled switch to model a mosfet? It's not going to model the gate/source voltage or the non-linearity, or any of the mosfets other charactoristics properly.

Sceadwian,

Because sometimes one doesnt need an elaborate model. A crude first order model for a hard switched power mosfet is simply a low valued resistor. Sometimes thats all you need!

However, now that the OP is asking about gate rise times and switching times, NOW he needs a more accurate model to account for these things.
My advice is to use a simulation model available from the vendor.

 

[technogeek]

My advice is to use a simulation model available from the vendor.

Hmmmmm....

Well that's a little over my head. How do you import and use the model?

Are there any "coding" examples on the net?

 

[Optikon]

Hmmmmm....

Well that's a little over my head. How do you import and use the model?

Are there any "coding" examples on the net?

First, you have to verify that the vendor even has one available for you to use. Go to their website and try to find the PSPICE model for the device. Some websites are easier than others at getting to this info, so I dont have any tips on how to get the model. If you can't find it, you may have to email someone for it.

Anyhow, once you have one, the way to incorporate the model depends somehwhat on the software being used. I dont know what simulator you are using so I cant say for sure. The end result for all types is the same though. The model must be present in the final netlist for simulation.

Sometimes this is as easy as pasting the model text right onto your schematic. The model name must match the name of the part in the circuit. Sometimes you can specify a link to the model text. The point is, when the simulator finds the part name in the netlist and it doesnt know what it is, it has to be told where it is or otherwise included somehow.

Use the help in your simulator - it will tell you how to add a model.
Try it and post back.

 

[technogeek]

I'm using Orcad PSPICE v9

Well here's what I found on the transistor I want to simulate:

* MODELLING FOR STB11NK50Z
.SUBCKT STB11NK50Z 1 2 3
LG 2 4  7.5n
LS 12 3 7.5n
LD 6 1  4.5n
RG 4 5  2.702
RS 9 12 0.219E-01
RD 7 6  0.304
RJ 8 7  0.232E-01
CGS 5 9   0.148E-08
CGD 7 10  0.225E-08
CK  11 7  0.408E-10
DGD 11 7 DGD
DBS 12 6 DBS
DBD  9 7 DBD
MOS  13 5 9 9 MOS L=1u W=1u
E1  10 5 101 0 1
E2  11 5 102 0 1
E3  8 13 POLY(2) 6 8 6 12 0 0 0 0  0.654E-01
G1  0 100 7 5 1u
D1  100 101  DID
D2  102 100  DID
R1  101 0  1MEG
R2  102 0  1MEG
.ENDS STB11NK50Z
 
.MODEL MOS NMOS
+ LEVEL = 3
+ VTO   = 4.763
+ PHI   = 0.847
+ IS    = 0.1E-12
+ JS    = 0
+ THETA = 0.304E-01
+ KP    = 11.208
 
.MODEL DGD D
+ IS    = 0.1E-12
+ CJO   = 0.137E-10
+ VJ    = 0.755
+ M     = 0.349
.MODEL DBD D
+ IS    = 0.1E-12
+ CJO   = 0.155E-10
+ VJ    = 0.761
+ M     = 0.332
.MODEL DBS D
+ IS    = 0.1E-12
+ BV    = 569
+ N     = 1
+ TT    = 0.388E-06
+ RS    = 0.636E-02
.MODEL DID D
+ IS    = 0.01E-12
+ RS    = 0
+ BV    = 679
* END OF MODELLING

I've been reading up on what a subcircuit is, and from what I understand, all those nodes are in their own little world, so they don't apply to the external circuit. Anyways, it has 3 pins, and it looks like gate is pin 2, source is 3, drain is 1.

Is that correct?

Now to put that "subcircuit" into my pspice model, I have to use the "X" function - like this:

Xmosfet 1 10 2 STB11NK50Z

where 1 10 and 2 are the "external" nodes for the drain/gate/source in that order. Correct?

Well obviously something's not correct, because I have nothing on the output now, it's a dead switch.

 

[Sceadwian]

Well you don't use a vswitch symbol, you use a mosfet symbol, usually you have to .include the subcircuit model and edit the mosfet symbols properties, to change the "prefix" to X and the 'value' to subcircuit entry for the mosfet you want to simulate. That's how I did the exact same thing in ltspice and I'm asuming orcad and ltspice are similar enough that you may know what I'm talking about.
In LTspice at least right clicking on a symbol brings up a context menu for the symbol type allowing selection from the library items installed. Control right clicking brings up the raw properties allowing you to change the normal symbol to map to the sub cirucit. Check Orcads help files or their support if you're lost after this post.