Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
System Development Suite Related Products A-Z
Cadence® digital design and signoff solutions provide a fast path to design closure and better predictability, helping you meet your power, performance, and area (PPA) targets.
Full-Flow Digital Solution Related Products A-Z
Cadence® custom, analog, and RF design solutions can help you save time by automating many routine tasks, from block-level and mixed-signal simulation to routing and library characterization.
Overview Related Products A-Z
Driving efficiency and accuracy in advanced packaging, system planning, and multi-fabric interoperability, Cadence® package implementation products deliver the automation and accuracy.
Cadence® PCB design solutions enable shorter, more predictable design cycles with greater integration of component design and system-level simulation for a constraint-driven flow.
An open IP platform for you to customize your app-driven SoC design.
Comprehensive solutions and methodologies.
Helping you meet your broader business goals.
A global customer support infrastructure with around-the-clock help.
24/7 Support - Cadence Online Support
Locate the latest software updates, service request, technical documentation, solutions and more in your personalized environment.
Cadence offers various software services for download. This page describes our offerings, including the Allegro FREE Physical Viewer.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
This course combines our Allegro PCB Editor Basic Techniques, followed by Allegro PCB Editor Intermediate Techniques.
Virtuoso Analog Design Environment Verifier 16.7
Learn learn to perform requirements-driven analog verification using the Virtuoso ADE Verifier tool.
Exchange ideas, news, technical information, and best practices.
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.
It's not all about the technlogy. Here we exchange ideas on the Cadence Academic Network and other subjects of general interest.
Cadence is a leading provider of system design tools, software, IP, and services.
I am using Calibre ( mentor Graphics). It creates the spectre Netlist and calibre view for PEX.
However, claibre view creation takes a lot of time unlike its spectre Netlist.
The spectre netlist it creates in a file like xyz.pex.netlist.
The format is as below:-
simulator lang=spectreinclude "SUBCKT_BLOCK.pex.netlist.pex"subckt SUBCKT_BLOCK ( DVDD DVSS A B C D E \ F )
............the sub ckt netlist body .............
include "SUBCKT_BLOCK.pex.netlist.DIV_BY_4_WITH_GRID.pxi"// ends SUBCKT_BLOCK// //
Is it possible to associate this netlist to the corresponding subckt symbol used in the bigger ckt block the schematic editor so that the created netlist will have the above sub-ckt netlist in the output netlist of the bigger ckt block ?
I followed this link :- http://www.cadence.com/Community/blogs/rf/archive/2009/01/07/tip-of-the-week-how-to-simulate-a-subcircuit-netlist-with-spectre-in-ade.aspx,
but it did not work.
The model name is being written 'subcircuit'
i.e in the netlist it shows something like I0 ( A B .......other terminals) subcircuit.\
Subsequently in the ADE run I am seeing the error " that the model subcircuit is NOt found".
Could anybody please tell where I am going wrong.
In reply to RFStuff:
Hard to be 100% sure without seeing the CDF, but my guess is that you've left the component name as "subcircuit" in the spectre simulation information in the CDF, or have left the value of the "model" parameter blank. You could also just replace "subckt" in the spectre simInfo with whatever the subckt is actually called.
In reply to Andrew Beckett:
Thanks a lot for your reply.
May be I was unable to interprete the steps written in that page. So I am thinking better to post the steps I have alrady done.
What I want :-
a) I want to associate the extracted netlist file named BLOCK.pex.netlist to the symbol BLOCK ( which is being used in a bigger schematic) only when I want to do PEX simualtion of the entire big schematic.
b) I should also revert back to normal symbol ( not PEXed netlist) view when I am not interested in PEX simulation
What I did is as follows:-
1) I went to BLOCK_LIB-> BLOCK and copied the symbol of BLOCK to spectre view. So a spectre view is created which is exactly like the symbol.
By the way BLOCK_LIB is the library containing the cell BLOCK. So what I did is:-
BLOCK_LIB-BLOCK-Symbol copied to BLOCK_LIB-BLOCK-Spectre
2) icfb->Tools->CDF->Edit ( CDF prompt came up)
3) CDF Section->Cell CDF Type-> Base
4) Browsed to the cell containing the symbol BLOCK.
5) Then went to the Component Prameter Section
clicked on Add button. Edit CDF Parameter Form came up
param Type - string
The remaining field I kept blank
Clicked on Apply
6) Then I went to Simulation Information Section
Clicked on Edit button
Edit Simulation Information Form came up
Choose Simulator:- spectre
kept blank as suggested in that page, I think, Andrew you are pointing to this ( bang on target) which is by default subcircuit. Am I right ?
termOrder- pins names filled in the proper order as in the .netlist file. i.e. "A" "B" "C" "D"
Rest kept blank
Clicked on Apply
Well That is it !!!
1) The model name is coming as subcrcuit
2) How I can revert back to the normal symbol view ?
With changing the " componentName- to the Name of The CELL" ( as suggested by Andrew), it is taking the netlist file.
But once the spectre view is created, the netlist always taking/ tries to take the model ( in my case the extracted big Netlist) even if you have both symbol view and spectre view of the cell. It doesn't distinguish between symbol view and spectre view as far as the netlist is concerned. If I disable the model ( the netlis), it still tries to take the netlist and gives error.
Could anybody please tell how I can revert back to the normal symbol view operation without deleting the already created Spectre view ?
Is there any simpler ways of inserting pin name into the cell view ? One can easily commit a mistake while inserting pin name in order especially when the number of pins of the CELL is large ?
I suspect you original problem was caused by adding a parameter "model" but not giving a value to the model parameter, and then it reverts to the default behaviour of using the componentName.
Anyway, if you want to switch between the schematic and your "spectre" view, you can do one of two things:
When the number of pins are really large, entering the pins manually is painful and error prone.
Is there a way other than manually, of entering the pins from the symbol.
You could open the symbol, and do:
and then you'd have to manipulate the order to match the external netlist.
You could always write some SKILL to parse the subckt header and then do some pattern matching to the terminal names in the symbol and do this yourself...
With QRC you can also specify the pin order that you want when doing the extraction; not sure if other extraction tools provide this (you'd have to ask the vendor) - that way you can generate the order in the CDF using the above SKILL function, and then give this order to your extraction tool.
Thanks a lot.