[moved] Error after importing PSPICE model of a transistor in ADS

Friends,

I'm trying to import PSPICE model of "EPC2012C" (which is available on https://epc-co.com/epc/Products/eGaNFETs/EPC2012C.aspx ) in ADS. ADS can import it without any error, but when I want to simulate a circuit including model of the transistor I face an error. It seems there is a function that has not been defined. Do you have any idea how to solve the problem?

The pulse source at left appears to have a red 'X' over it. Did the simulator mark it as an error?

- - - Updated - - -

It appears you have 2 signal/power sources connected directly. The simulator may call it an error. Try putting a low-ohm resistor between them.

BradtheRad said:

The pulse source at left appears to have a red 'X' over it. Did the simulator mark it as an error?

- - - Updated - - -

It appears you have 2 signal/power sources connected directly. The simulator may call it an error. Try putting a low-ohm resistor between them.

Click to expand...

One of them is deactivated. The error is because of the PSPICE model.

Did you review the model? It uses non-standard behavioral expressions, probably not supported by the ADS SPICE netlist translator.

FvM said:

Did you review the model? It uses non-standard behavioral expressions, probably not supported by the ADS SPICE netlist translator.

Click to expand...

Thank you!
Can I fix it myself? Doing some changes in the model I mean!

I believe that it's possible to translate the model to an ADS subcircuit, e.g. using controlled switches instead of the if () expressions, but not so easy.

Sometime Spice models/netlists include functions that are not natively supported by ADS. This appears to be the case in this model where the ADS_SPC_IF() function is referenced. There is a file provided with ADS to cover functions such as this. In on-line help it mentions:

Using Non-ADS Functions

If your file contains functions such as gauss() or pwr() or any other function that is not a built-in ADS function, the simulator will give an Unresolved reference error.

Look for the function in the supplied function file:

$HPEESOF_DIR/links/spice/spicefunction.net (for SPICE functions)

The function can be copied into the ADS netlist, placed in the schematic...

Click to expand...

The easiest way to make sure that this file is included is to add a NetlistInclude symbol in the schematic where you are trying to run this simulation.



For the IncludeFiles parameter browser to the spicefunctions.net file at the above location, the IncludePath parameter will be filled in automatically, and then run the simulation. The error should then no longer occur.