Implementation of a LTSpice diode model in Cadence

In terms of model compatibility, I think treating it as a PSPICE model would be best. So put the model above in a file, and then reference it from Setup->Simulation Files->Pspice Files. Then instantiate a diode from analogLib and specify the model as D1N4148. That's it!

Hi, Andrew! 

I could not relate to the steps you mentioned. I haven't imported any third party model before in Cadence, so because of that, I am unaware of the process. I only could relate to specifying the model after instantiating the diode from analogLib as I can see an option to insert the model name. Here are my questions:

1. I have the diode model, right? You told me to put that model in a file. I can paste it in a text file but what should be the extension type of the file for Cadence to recognize? And does it have to be saved in a particular directory?

2. I do not have the "setup" tab and the subsequent tabs in the version that I am using as you mentioned for referring to the file. I am providing two screenshots here two show you what tabs I have. If you could tell me how to implement it in this version, even roughly, it would be helpful. The only setup tab that I can see is accessed from the "analog environment tab" (figure 03).

Figure 01: icfb terminal

figure 02: Virtuoso interface

Figure 03: Setup tab

Dear Muhaisi,

You really need to update your Cadence version!

Muhaisin said:

1. I have the diode model, right? You told me to put that model in a file. I can paste it in a text file but what should be the extension type of the file for Cadence to recognize

In order for Cadence to recognize it automatically as a spectre netlist, it should have the extension ".scs".

Muhaisin said:

And does it have to be saved in a particular directory?

You will provide the path to your file in the ADE-L GUI "Simulation Files..". You may choose one of the empty lines beneath, for example, the Simulation Files... "PSpice Files" if that is present in your version of ADE-L

Muhaisin said:

2. I do not have the "setup" tab and the subsequent tabs in the version that I am using as you mentioned for referring to the file. I am providing two screenshots here two show you what tabs I have. If you could tell me how to implement it in this version, even roughly, it would be helpful. The only setup tab that I can see is accessed from the "analog environment tab" (figure 03)

As mentioned, please refer to the GUI under  Setup->Simulation Files ->PSpice files

I hope this helps...

Shawn

A few mild corrections to Shawn's reply:

1. Since this isn't in Spectre syntax, you probably shouldn't use the ".scs" suffix. In general, spectre and ADE don't care about the suffix of the files passed to the simulator - the only special case is that if it has a ".scs" suffix then it's understood to be in the spectre language; any other suffix is treated as SPICE. That said, if it had been included via the "Pspice files" UI then it would have been treated as PSPICE syntax and compatibility anyway.
2. The version of Spectre you have however does not support PSPICE syntax/compatibility. That was added in MMSIM13.1 (and of course the later SPECTRE* versions), so in 2013 - 4 years after the version you're using. So the only option you would have is to use this is to treat it as vanilla SPICE. So you'd give the file any suffix other than ".scs" (or add the line "simulator lang=spice" in the file).
3. However, from a quick simulation, the results are a little different when it's been treated as PSPICE compared with standard SPICE. I believe LTSPICE is closer to PSPICE - whether this matters for a diode, I'm not sure, and if you're really stuck with 11 year old software, I guess you need to live with that.
4. In IC5141 that you're using, the UI is as I said, other than there's no "Pspice Files". That won't appear even if you use a new enough spectre, because the last hotfix version of IC5141 was in 2011, before the feature was added in SPECTRE.

So I'd reiterate Shawn's point - you're really hampering your options by using such old software.

Andrew.

Thank you to both of you. I have to make do with the version that is provided by the university, so upgrading is not an option now. So, for the version that I have, if I do the following, will it work?

1. Save the diode model in a text file with .txt extension, using the name of the diode model as the name of the .txt file.

2. Paste the file in the directory where Cadence looks for simulation files. I can know that folder by going to "simulation files" under "setup" tab in "analog environment".

3. Then when I instantiate the diode, in the "model name" option, I insert the file name.

Did I get anything wrong?

Not quite. All you need to do is store it in a file somewhere and then in Setup->Model Libraries navigate to the specific file. You could give a full path name, or just the file part of the name and ensure it's in a directory listed in the include path. From what you've done above, nothing will actually include the file - merely being in the include path doesn't cause it to be included.

When you instantiate the diode from analogLib, you'd give "D1N4148" since that is what the name of the model is in the .model statement. It's not the file name you give here.

Andrew

Dear Andrew,

A sincere thank you for "watching over my shoulder" and correcting my comment concerning the use of the ".scs" file extension for the PSPICE component netlist file. I, too, and continuing to learn (thanks to you!).

Shawn