Importing Microchip Spice Models(MOD)

[While(E)]

Hey guys, rather new to the MultiSim world and would like to import a .MOD Spice model from the Microchip website. http://www.microchip.com/wwwproducts/Devices.aspx?dDocName=en025917.

I have followed a few different tutorials, all using component wizard, and all have left me with "An error has been found in the Netlist, would you like to proceed anyway?" Most of these tutorials are extremely well written, and a few right from this site, but I still fail to achieve a usable model. So I'm sure I'm just mucking something up...

I apologize for the n00b question, but am I overlooking something here? It seems like if the manufacturer actually gives you the Spice model it should be relatively simple to import that directly into such a nice piece of soctware like MultiSim, but again I have very little experience with creating/importing new components in this software.

Thanks for any help!

I've attached a (CIR) file, because the original (MOD) wouldn't upload here. So I just went into Notepad++ and changed the extension. All info should be same.

[johnsold]

I do not have Multisim, but have used other SPICE simulators.

Converting models often takes some understanding of the differences between SPICE versions and the limitations of both the model and the simulator.

The model clearly indicates that it is intended for use with PSPICE or SPICE 2G6. I am not sure which SPICE version Multisim uses, but SPICE 3 is considerably different in some areas, such as controlled sources (G and E devices in the model).  My SPICE simulator will not accept POLY for example.

Another thing which is acceptable as a model but which may cause convergence problems is the use of voltage contrlolled switches with very large ratios between Roff and Ron.  I would be concerned about the model for SS59.

Lynn

[Tien_P]

Hi While,

There are a few problems with the model.

1.  There is an extra closing bracket at the end of the following lines, remove it:

G61 61   60   TABLE { V(61, 60) } (-20M,-1300)(-15.0M,-650)(-10.0M,-130)(0,0)(10,1N))

G62 60   62   TABLE { V(60, 62) } (-20.0M,-1300)(-15.0M,-650)(-10.0M,-130)(0,0)(10,1N))

2.  The following line is also causing a simulation problem and this one looks like a Multisim bug. 

R53  0 50 1 TC -4m 12u

TC is a temperature coefficient that changes the resistor value base on you temperature, and it doesn't look like Multisim accepts a negative number. 

R= Rnom·(1+TC1·(T-Tnom)+TC2·(T-Tnom)2)

-4m is TC1 and 12u is TC2, T is temperature you are simulating at and Tnom.

I don't think temperature coeffiecient makes a big different in simulation, you can use this:

R53  0 50 1