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 have a design with some nodes using bus syntax, for example some nodes labelled BL<1:2>.
I create a stimulation file (.scs) containing:
_BL1 (BL<1> 0) vsource type=dc dc=0_BL2 (BL<2> 0) vsource type=dc dc=3.3
but when it parses it it gives the following error:
"/home/sim/Cadence/Sim/SynMem_Test/spectre/schematic/netlist/stimuli/2010_04_14SynMem_Test.scs" 1: Unexpected operator "<". Expected end of file or end of line.ERROR (SFE-874):
2: Unexpected operator "<". Expected end of file or end of line.
I assume I have to write something special for it to accept the bus syntax. Looking in the netlist it normally produces without the stimulation file, I see, for example:
InvBL\<1\> (nBL\<1\> BL\<1\> 0 vdd!) INV1InvBL\<2\> (nBL\<2\> BL\<2\> 0 vdd!) INV1
However when I try using the backslash in my stimulation file, like this:
_BL1 (BL\<1\> 0) vsource type=dc dc=0_BL2 (BL\<2\> 0) vsource type=dc dc=3.3
I get the same error.
Can anyone suggestion a solution?
If you're using the stimulus file field in ADE, it gets passed through a pre-processing option to allow you to use "schematic" names in the netlist, which can then have any mapping applied to them that happened during netlisting.
Because of this pre-processing, the \ you are entering is being stripped off (you'd have to use a double backslash). A better approach is to use the OSS mapping syntax. For example, if you do:
v1 ([#bus<0>] 0) vsource type=sine freq=1M ampl=1
v2 ([#bus<1>] 0) vsource type=sine freq=2M ampl=1.5
v3 ([#bus<2>] 0) vsource type=sine freq=3M ampl=2.0
v4 ([#bus<3>] [#/gnd!]) vsource type=sine freq=4M ampl=2.5
You should then end up in the netlist as:
v1 (bus\<0\> 0) vsource type=sine freq=1M ampl=1
v2 (bus\<1\> 0) vsource type=sine freq=2M ampl=1.5
v3 (bus\<2\> 0) vsource type=sine freq=3M ampl=2.0
v4 (bus\<3\> 0) vsource type=sine freq=4M ampl=2.5
or whatever those bus names got mapped to during netlist. Note that there's a problem in IC613/IC614 where this (by default) doesn't work properly with busses (the backslashes get missed out). It's OK in IC5141. The CCR is 752498 - and the workaround is to switch back to the mapping scheme used in IC5141 - enter envSetVal("asimenv" "mappingMode" 'string "oss")
We also have a CCR to get the above [#...] syntax documented more clearly (it is right now, but hidden away in the Open Simulation System manuals, rather than being in the ADE manuals).
In reply to Andrew Beckett:
Thanks very much for this. Mixed results though. It will now parse the file. However in the input.scs file that it generates for the design from the schematic, bus nodes that were previously listed as e.g. bus\<1\> are now listed as bus_1. Then, if I select one of those from the schematic for being saved and plotted, this appears in the save statement as bus\<1\>, with the effect that they are not recognised as nodes and not saved or plotted. Any ideas? (I'm not stuck though because I can use "nmp" mapping and double backslashes for now).
One more related question: in my design I had a bus called BLin<1:36>. When I simulated this, node BLin<35> and only that one caused problems - it seemed to recognise that node as already existing, although it's nowhere else in my design. when I changed the name of the bus to e.g. BLInputs<1:36> the problem went away. Have I hit on a reserved word or something like that?
In reply to simbamford:
I am trying to include a stimulus file using an OCEAN script with IC 6.15/MMSIM 12.1.
It connects a voltage source to a net bus<1>.
The OSS syntax [#...] doesn't seem to work (Unexpected '[' or unexpected '#' error). Bus<1> doesn't work either (unexpected '<').
In the input.scs the net seems to be output as bus\<1\>.
Using bus\<1\> and bus\\\<1\\\> work (i.e. no errors at read-in) but in all cases the net comes up as floating and is removed.
Using the suggested option by Andrew with bus_1 in the stimulus file still leads in the net being removed.
I am assuming I am missing some mapping happening at some point after the initial netlisting.
The net is not at the top level of the hierarchy but lower down.
Any ideas would be greatly appreciated.
In reply to kglaros:
This ought to work - are you using envSetVal("asimenv" "mappingMode" 'string "oss") ?
If you've changed it, you probably would need to re-start ADE and also force a Netlist->Recreate.
If it doesn't work, please contact customer support - we need to investigate why.
thanks for the reply.
Just for the record, simulating with ADE worked as expected in the end (even without the OSS mapping). It was a mistake on my side.
I didn't manage to get OCEAN to work consistently. I have given up on that approach a while ago.