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.
As a former Layout user, who has attended the Orcad PCB Editor class, I'm baffled why it's so hard to change a symbol within an existing design; for example, you decide that a 603 passive ought to be a 1206.I did update the symbol by deleting the part in Capture, netlisting, importing logic into Pcb Editor, puting back the same part with the different symbol into Capture, netlisting, and finally importing into Pcb Editor, but this seems like an overly complex thing to have to do.What is the preferred method?Thanks,Mike
HI Mike, you might want to try exporting the netlist w properties, in here it contains the $PACKAGES in here you can just sub out the footprint name for the new one, then save and do an import Logic (other) this saves time on the schematic, however I think its best practice to use the schematic. and I would in most cases advise that.Stephen Grant-Davies (QuantumCad)www.quantumcad.co.uk
>I did update the symbol by deleting the part in Capture, netlisting, importing logic into Pcb Editor, puting back the same part with the different symbol into Capture, netlisting, and finally importing into Pcb Editor, but this seems like an overly complex thing to have to do.That seems a bit more than needed- maybe try, in Capture, right click the part, edit properties, change PCB Footprint, build netlist, switch to PCB Editor, import logic, place part. It's pretty quick? If you need to change, for example, all the 0603's to 1206's, then it's easier to open the .upd file, edit>replace the footprint name in the text editor, then in capture tools>update properties, build netlist... -Phil
u can try following.
Use "Alternate Symbol" property in Capture. Give different package 0603,1206 for exapmple seperated by comma(or semicolon, just check it).
When placing a component in PCB editor use pop up menu and select "Alt Symbol" which will give u your defined alternatives.
Hit the Select Component Tool, then click on the component. Right click, select Properties, then Footprint. This brings up a dialog where you can graphicaly browse the footprints.Randy
Thank you for all of the replys. I believe that some of the problem was related to the location of my symbol directory. Placing these at the root (rather than C:\Profiles\My Documents and so on) made the search path work better when the padstack was matched up with the symbol. It then worked as I intended: loading a new footprint into an existing placed part without having to rip up that part.
"My Documents" folder is not a great idea: allegro does not like space in file names, despite they try to handle it in new release.And pecial caracters (such ç ô à) are not welcome in directory name.