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 hope that this question is appropriate for this forumI am using the "L" version of PCB Performance and SigXplorer and am still somewhat new to them.I am trying to use the Topology Extract feature to extract a net into SigXplorer. The net is actually divided into 2 individual nets with 2 net names. Net #1 is routed from the driving source to one side of a series terminating resistor. Net #2 connects the other side of the term. resistor to the receiver.Using Topology Extract, I can only seem to extract one net or the other (including the resistor) into SigXplorer. How do I specify that I want to extract the entire net (from source to receiver)?Thank YouNick
Hi,the SQuest & SigExp must recognize the net as xnet, for that you need to assign a SI model to the serie resistor.Doron.
Hi and thanks for the reply!The resistor is part of a resistor pack to which I have created / assigned an IBIS device model. I assigned all of my IBIS models through the Setup Adviser.How are Xnets created? Is this done through the Constraint Manager? My installation of 16.0 seems to have some problems with the help files!Nick
if you created it right then it should work.you either didn't creat a valid part or didn't assign it in the advisor,make sure that the value field is a number only (10 not 10R or such).also i think that it should be a spice model device not ibis model.good luck.Doron.
You have to assign a dml model to the rpack and the rpack has to have the property of being a discrete for this to work correctly. SourceLink has a good example of an Rpack with common pins and the create e spice model will do standard rpacks automatically.
>>You have to assign a dml model to the rpack<<Actually, I used the IBIS file generator in Model Integrity to make an Ibis model for the resistor pack which has 8 isolated resistors (not bussed, no common pin) I then converted the Ibis device model to DML and assigned it to each resistor pack in my design through the Adviser. The value field is set to the value of the resistor (47) with no other chars.When I extract either net into SigXplorer, the resistor also ports in with the correct pins on the resistor pack that the nets are connected to and the correct R value (47) also ports in. It's only the other net and its driver or receiver that doesn't port in.>>the rpack has to have the property of being a discrete<<Where do I set this?>>SourceLink has a good example of an Rpack with common pins<<Im in the process of looking for this now.Nick
You can change a device type in Logic - Parts List but if you have correctly assigned an espice model to the rpack, this should not be a problem.
Extracting through the resistor should work (eventually!). Make sure you have PinConnections.When all else fails, you can extract the two nets separately and then use the File -> Append feature to glue them together. That feature is powerful yet simple, and works quite well.Donald
Hi,I've seen cases in the L version of the tools where you need to run Tools, Database check inside the PCB Editor in order for it to recognize the xnet after assigning espice models to resistors - so try that.Best regards,Ole