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.
Has anybody tried to do SI analysis from HDL XL directly. When i exported the net to SI the topology gets extracted to SIGxp but the Results and Measurement does not appear in SIgxp. With out this i cannot simulate the toplogy.
> Now i am saving the same topolgy and then simulating the same by opening the Sigxp separately.Cant we simulate the topology directly?
> I wanted to know about the properties about the transmission line which is passing to SigXp. Will it take only the constraints set in CM only? In that case we can create the topology independent of schematic in SigXP directly...
It's possible that you are running Concept from an non SI license, in this case, you will be able to get SigXP to open and extract "stuff" but you won't be able to simulate it without the "simulator" license. In Concept, use File>Change Product to select an SI license and see if that dows the trick.
In reply to oldmouldy:
Do you have Allegro PCB SI installed on the same pc as Concept HDL XL? If yes, then the problem could be that the tool is invoking that version of SigXP that does not include analyze/measurement capabilities. Try this: close all Cadence tools > double click on System icon in control panel > in system variables section add the SIGXP_TIER variable with it's value set to SELECT. Now see if you can get the tool to give you the option to select the version of SigXP that comes with Allegro PCB SI. If yes, select that version and click OK.
In reply to Khurana:
One more tit bit about topologies that are extracted from Concept CM. Since Concept has no understanding of the board real estate all the tlines comes out as 2800 mils in length. You may define min/max propagation rules, length matching rules in SigXP and then "backannotate" them by clicking on the Update Constraint Manager icon OR save the topology file by giving it a name then import the topology file as an Electrical Constraint Set (ECSet) in Constraint Manager by going to File > Import > Electrical Constraint Set. Lastly, you may also assign models to parts in Concept schematic. This is done by going to Tools > Assign Models (if I am not mistaken). You may select the .dml and attach it to the symbol in schematic so that when the topology is extracted the corresponding buffer (model) is what you get in SigXP. Try out the Concept/CM tutorials on this in Help - they are very good.
Thnx khurana it worked after assigning in the env variables..
Oldmouldy: With SI suite it doesnot allow us to work the concept hdl..The suite should be be hdl l r hdl xl...
Anyways thnx for the suggestions.