Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
Verification 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.
The Cadence Academic Network helps build strong relationships between academia and industry, and promotes the proliferation of leading-edge technologies and methodologies at universities renowned for their engineering and design excellence.
Participate in CDNLive
A huge knowledge exchange platform for academia to network with industry. We are looking for academic speakers to talk about their research to the industry attendees at the Academic Track at CDNLive EMEA and Silicon Valley.
Come & Meet Us @ Events
A huge knowledge exchange platform for academia. We are looking for academic speakers to talk about their research to industry attendees.
Americas University Software Program
Join the 250+ qualified Americas member universities who have already incorporated Cadence EDA software into their classrooms and academic research projects.
EMEA University Software Program
In EMEA, Cadence works with EUROPRACTICE to ensure cost-effective availability of our extensive electronic design automation (EDA) tools for non-commercial activities.
Apply Now For Jobs
If you are a recent college graduate or a student looking for internship. Visit our exclusive job search page for interns and recent college graduate jobs.
Cadence is a Great Place to do great work
Learn more about our internship program and visit our careers page to do meaningful work and make a great impact.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
Overview All Courses Asia Pacific EMEANorth America
Instructor-led training [ILT] are live classes that are offered in our state-of-the-art classrooms at our worldwide training centers, at your site, or as a Virtual classroom.
Online Training is delivered over the web to let you proceed at your own pace, anytime and anywhere.
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 find the one big footprint library very cumbersome. Has anyone broken theirs down into sub categories, ie; resistors, capacitors, ic's, etc..... If so are there any special constraints for the directory structure?
Do the padstacks need to be resident in the footprint library directory, or can I have a padstacks directory seperate from the footprints?
I would think I'd have to do something with the paths in order to make Editor locate the new sub directories, right?
Yes you can have sub directories but they all need to be listed in the psmpath setting, You can also have a padstacks folder that can be different - hence the padpath setting. The only thing you need to do is keep the dra and *.sm file together (a recommendation).
When the tools look for a symbol they start at the top of the psmpath list and work down the list until it finds the relevant symbol name. This means that you have to make sure you don't have duplicates in the folder that you use because it will use the first one it finds...
Tom you can have different folders for your symbols and padstacks but you would have to edit the PSMPATH & PADPATH to tell the system where to look. In Allegro go to Setup User Preferences then go to Paths, Libary.
When you create a package symbol for a footprint there will be 3 files created. .DRA, .PSM, .TXT. You will also have the padstacks used for that particular symbol. What I do is keep the pads,dra,psm, .txt files for each symbol in the same folder. This has helped me cut down on packaging problems when creating a board from the schematic.
By way of an example here is directory structure.
PSMPATH is configured to point to the following "Click expand in that dialog box first" and remove any paths you do not need before making your edits.
PADPATH is configured the same but I also include a folder for vias, again "Click expand in that dialog box first" and remove any paths you do not need before making your edits.
When you create your symbols dont use spaces in the name as it will lead to packaging problems. For example SOT_23.dra,SOT23.dra are all ok to use.Be aware also that it is possible for Allegro 16.5 to blow away your custom PSMPATH and custom PADPATH and replace them with system defaults. I kid you not. This one seems to be a bug. My work-around for this is to make the env file read-only after all edits have been made. Depending on your setup you may or may not come across this hidden treasure, hope you dont : )
In reply to ScottCad:
Exactly what I had in mind to do. Thanksfor the help. Looks like I'll be spending tomorrow converting old libs and setting up new directories / paths and the like.
I just received a PO for a job I quoted a while back and it requires using 16.5 so I am diving into the deep end........ and hoping to surface............
In reply to TH Designs:
I keep the .dra organized as you suggested in their own folders. But at the top of the library path I keep *all* of the .psm files. What is the advantage to this? The pathing is simple and Allegro will package correctly since it only cares about .psm files.
The only disadvantage is preview in OrCAD for footprints which I don't use.
ScottCadBe aware also that it is possible for Allegro 16.5 to blow away your custom PSMPATH and custom PADPATH and replace them with system defaults. I kid you not. This one seems to be a bug. My work-around for this is to make the env file read-only after all edits have been made. Depending on your setup you may or may not come across this hidden treasure, hope you dont : )Thanks Scott
Be aware also that it is possible for Allegro 16.5 to blow away your custom PSMPATH and custom PADPATH and replace them with system defaults. I kid you not. This one seems to be a bug. My work-around for this is to make the env file read-only after all edits have been made. Depending on your setup you may or may not come across this hidden treasure, hope you dont : )
Guess what just happened................................... Paths are gone.
Opened service ticket with EMA. We'll see what they say.
Response from EMA:
When you set your psm and pad that did you add it to the favorites in the Setup
User Preferences? If you did that would explain it. There is a bug and adding
the psm and pad path to the favorites causes them to reset.
And Yes you have to add every folder. You cannot add the
highest level. The tool will not recursively search the sub folders.
I have the paths set as favorites............ figures.
PS: I think I recall reading this in another post, sorry if I'm duplicating subjects.
Tom, that is a bug in the SW for sure. What you might consider doing is Make a copy of your env file and save it off to another folder just in case Allegro tries to nuke some of it's settings. I did that and then made the working env file Read only as a precaution.
Got to love the hidden Treasures : )
I found this really helpful.
Thanks Scott. And unfortunately I kind of hit the hidden treasure. But your readonly trick save me another day. :)