How do I associate a PSpice Model to non PSpice Model resistor?

If you look in the analog.lib file with a text editor, you will see that this LIB file, unlike others, is just a "placeholder" to support the netlisting process. The "fundamental" SPICE models in Capture / PSpice just use the PSpice Template property value for modelling those components. Note that the PSpice Template property value contains Pin Names from the part graphics and these will need to match your schematic part for the mapping to work.

Ok thank you. I had a look at R from analog.lib and in the PSpiceTemplate it has the following code:

• R^@REFDES %1 %2 ?TOLERANCE|R^@REFDES| @VALUE TC=@TC1,@TC2 ?TOLERANCE|\n.model R^@REFDES RES R=1 DEV=@TOLERANCE% TC1=@TC1 TC2=@TC2|

To make it easier for me to do a single modification to a resistor I skipped out what I understand to be temperature coefficients, TC1 & TC2 and I am able to simulate using the part if I only use the following code:

• R^@REFDES %1 %2 ?TOLERANCE|R^@REFDES| @VALUE ?TOLERANCE|\n.model R^@REFDES RES R=1 DEV=@TOLERANCE%|

The part now get s a resistance value and a tolerance.

I can make due with selecting many components, adding a new property named PSpiceTemplate and then pasting that code to be able to make a simple simulation. This does not seem like a good way of doing it to me though since I would like to be able to simulate using temperature coefficients at some point in the future. It would therfore be better to refer to a simulation file instead since that's how I would be doing it for IC's and other components.

I understand that different resistors would have different coefficients, but then I could just refer to a different simulation file.

Is there a way for me to do write files like that? 

Take a look at the "breakout" library. You could copy / paste the Rbreak (and others that you might need from the analog library) to your own library and then associate the component(s) with those parts instead. For example:

.model Rdefault RES R=1 ; no temperature coeff

.model R10uCoeff RES R=1 TC1=10u ; 10ppm linear coeff

And so on. Then you should be able to Associate parts in the schematics with those libraries (I haven't checked that out) Just check that you then have the Implementation Type as PSpice Model, the Implementation as the Model name and the PSpiceTemplate properties set to couple the schematic part and the underlying model.

Great thank you very much!

Great thank you very much!