Pspice LM358P simulation

Can you explain what you are doing a little further? For example, both the libraries intended for PCB, <installation path>\tools\Capture\library, and the libraries intended for PSpice, <installation path>\tools\Capture\library\PSpice have LM358 parts but neither specifically has an LM358P. The part(s) from the PSpice libraries will have properties attached to support simulation with PSpice. Also there isn't a PSpice version 17.7, at least not so far, 17.2 and 17.4 are active.

Can you explain what you are doing a little further? For example, both the libraries intended for PCB, <installation path>\tools\Capture\library, and the libraries intended for PSpice, <installation path>\tools\Capture\library\PSpice have LM358 parts but neither specifically has an LM358P. The part(s) from the PSpice libraries will have properties attached to support simulation with PSpice. Also there isn't a PSpice version 17.7, at least not so far, 17.2 and 17.4 are active.

Yes oldmouldy. That was a typo . It was V17.2 not V17.7. I`m trying to simulate the dual opamp nature of the LM358P. Also the ones that cadence library has is just LM358 which is showing the single opamp behavior.I already have a .olb file of the LM358P opamp but I`m trying to see how should I be able to simulate it in the CIS Orcad capture 17.2 (pspice) version.Please let me know if this information was helpful.

Thank you

Devesh Kadambari

What are the details of the part in your OLB file? If you have a Heterogeneous split part, you won't be able to use that with PSpice. If you have a Homogeneous split part, two identical 5-pin sections, you can assign the Implementation, Implementation Type and PSpiceTemplate from the "single" part in the provided libraries (Check that the Pin Names in the Part(s) match the PSpiceTemplate values). If you a single, 8-pin, Part, you will need to build a "super model" for the 8Pins and then "call" two of the provided LM358 models from that - make a "default" part from that model text to get the required properties using Model Editor, and then copy / paste the properties to your "live" part.

Hello Oldmouldy,

I could understand in detail as to how to go about it? Is there a video link or tutorial page you can give ? That could be alot helpul. Also, this is just a homogeneous part not the heterogeneous part split. The idea is to check LM358P as a inverting amplifer since it is a dual opamp.  

The PSpice Users Guide covers topics like this. Here is an example "super model" for an 8-pin dual op-amp:

* LM358 Dual in 8-pin package
* Assumes LM358 model in configured libraries
.SUBCKT LM358Dual 1 2 3 4 5 6 7 8
X_U1 3 2 8 4 1 LM358
X_U2 5 6 8 4 7 LM358
.ENDS

Use the Model Editor to create a "default" symbol, that will get you the properties required to simulate, then you can add these to your library part. The PSpiceTemplate generated will need to be checked to ensure that the Pin Names are mapped correctly to the Pin Names on your schematic part. (The part PSpiceTemplate created from here will assume "pin numbers" are the pin names.)

Thanks, this helped me out a lot, as a beginner it's really hard to figure out from the help these simple things. Can you please point out a search key I can use in the help to locate the relevant section?
I have tried so far but I always get lost in the ocean of results