Stats

  • Locked Locked
  • Replies 9
  • Subscribers 125
  • Views 15601
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Simulating a logic library (without schematic views) in spectre

JohnB70

Hi,

I have received a logic library of about 50 cells.

Each cell one has a symbol view and layout view, but there is no spectre view and there is no prop.xx file.

There is also a big netlist file with a .subckt model for each of the cells.

I have asked for a schematic view for each cell, but these will not be provided. 

I want to simulate with ADE/Spectre a predominantly analog circuit with a few of these logic blocks as well.

Following the instructions in this link I was able to get an inverter to simulate.

http://community.cadence.com/cadence_blogs_8/b/rf/archive/2009/01/07/tip-of-the-week-how-to-simulate-a-subcircuit-netlist-with-spectre-in-ade

In a nutshell, I copied the symbol view to a spectre veiw and then Edit CDF to add terminal names for termOrder.

[I could add model= also, but that did not seem necessary as the model name and symbol name were identical.]

Do I have to do this for every cell in the library?

Is there any automated way to do it?

Why didn't the foundry deliver the kit with this already done (even if they did want to keep the scheamtics private)?

This is in Cadence IC 5.1.41

Thanks,

John

  • John,

    You could get away without the spectre view by ensuring that symbol is in your switch view list (probably at the end) and also in the stop view list, but it's better to create the spectre stop view - it's clearer.

    You could automate all of this with SKILL. I don't have anything to do this in my existing bag of tricks (although it wouldn't be too hard to write). I don't have the bandwidth in the next few weeks to write it, unfortunately.

    You'd have to ask the foundry why they don't provide this. It would seem a rather useful thing to provide to me!

    Regards,

    Andrew.

  • Hi Andrew, I got an updated library from the foundry that now has the prop.xx files. I also did what you suggest with the viewlists and it simulates now. Thanks.

  • Probably a good idea to create the spectre views too - it's a bit cleaner that way. This can actually be done in the library manager too. Go through these steps in the Library Manager:

    1. Edit->Copy Preferences and select "Do not add dependent property files to copy sets" and hit Apply
    2. With the library selected, Edit->Copy Wizard
    3. Click on the By View tab.
    4. In the Views to Copy field, enter "symbol". You should have the Library filled in, the Cell Filter blank (or can have "*")
    5. Click on the "Generate Copy List" button.
    6. Over an entry in the To View column, do Right Mouse->Select Column
    7. One of the entry boxes should have a white background with the text selected. In this box type "spectre" to replace the text "symbol"
    8. Having typed spectre, over the same box do Right Mouse->Apply Changes - all the other selected entries in the To View column should change to "spectre".
    9. OK the form.

    You'll then have spectre views for every cell in the library.

    Regards,

    Andrew.

  • That worked too, thanks.

    Now is there a way to generate the schematic views for every cell in the Library from the single netlist file (and the already existing symbols, if needed)?

    Thanks, John

  • You should be able to use File->Import->SPICE in the CIW. However, I'm not convinced it's worth it - the schematics typically aren't terribly pretty, and you often have to do a bit of work to set up the mapping to PDK devices, and sometimes need to call the CDF callbacks to make them behave properly.

    Regards,

    Andrew.

  • Apparently thats only available from IC 6.1 onwards.

    How different in Import/Netlist View... available in IC 5.1.41?

    The blocks are not too complicated so the schematics shouldn't be that ugly. But if there is a lot of setup I may stop here for now.

    My next step is to figure out how to do an AMS sim with this library... that may spawn a new thread!

    Thanks, John

  • John,

    The closest you have in IC5141 is File->Import->CDL.

    Regards,

    Andrew.

  • Hi Andrew,

    As you predicted following CDL import some parameters are wrong and I need to retrigger callbacks to fix.

    When I open the schematic a custom utility menu item from the foundry appears on the menu bar for "Callback Re-trigger".

    Is there a way I can run this on each cell in the library without opening each schematic individually?

    Thanks,John

  • John,

    I can't comment on the foundry-provided callback calling routine, but provides a similar function to do this on an entire library.

    Regards,

    Andrew.

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.