Cadence® system design and verification solutions, integrated under our Verification 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.
More Support Log In
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 technology. 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.
Hi,it's the first i'm using allegro and i would like to know how can i convert the libraries i have from layout to allegro.Can i use them or must i design the footprints from the beginning in allegro?
Thanks for your time.
Providing that you have a sufficiently high version number, I think that at least 10.0 is required, you can use the Catalog tool. In the LSession (grey) window when Layout is started, Tools>Catalog>Create, point to the LLB file and create the catalog. This will create a MAX file, or files, of all of the library parts. (You may get multiple files since Layout has a drill limit of 40 drills per MAX file) You can then translate the MAX file with the OrCAD Layout import / conversion. Note that Layout has oversized pads for plane layers, PCB Editor won't use these so the inner layers in the conversion can be deleted, the translation will create the required "default internal" data from the regular pad for thru parts)
If you have a pre-Catalog tool version of Layout, you will need to add the footprints manually to a desgn and then convert the resulting MAX file.
1) Anything which you have on a global layer will not be translated since there is not global layer in PCB Editor.
2) Any height keepouts which are round or have a rounded section will not get translated.
In reply to KEN13:
How about Title Blocks that are parts, I can't get them into Allegro. I tried converting boards and the title block won't come in. I also converted my libraries and the parts all come in minus Title Blocks and out layer stack up that are saved as parts.
It shows a (#Refdes) where the title blocks would be but nothing more. Global visibility is on and nothing shows up.
I don't want to recreate every single title blockl and all the text associated with them.
Lonf time Pads user and worked with Orcad and now this company is finally switching over to Allegro from Orcad10.5
Any help is appreciated..
In reply to DonlAZ:
I suspect your title block is on a layer that the translator does not support. What layer in Layout are you using for Title Blocks ?
From memory mine are on the asy top layer and they translated into Allegro fine without issue.
BTW, Orcad 10.5 is very old, You might want to pull your designs and libs in to an orcad 16 x version of Layout first save them and then try export etc. I believe the last ver of Layout was 16.2
In reply to ScottCad:
Thanks Scott for your reply!!
Yes 10.5 is old but government contractors like stability and don't change much..
The Title block is on the Drill Drawling layer and we're just now upgrading to 16.3 and want to get out libraries and title block info into it.
I also sent it into suport a few days ago and they got back to me a few days later on Friday. They guy had the file first thing that day but haven't heard back yet so not sure what the fix will be. I wouldn't think it should be that hard to translate. Long time Pads user and just now learning Allegro at a new position. Well used Orcad for a few year here until it got slow and now back again and tney're finally upgrading.
Thanks again for your help..
Hi Don got to love the Gov Work : )
Since your Title Block is on the drill layer I would move that to the ASSY Top layer in layout as a first step. I had a bunch of designs done in the layout 16x package and they translated really well into Allegro. With the title block on the assy top layer in layout when you translate the design it will put it on the Board Geometry > Assembly detail layer in allegro which is a good fit.
If you have the opportunity try upgrade to Allegro 16.5 which is the latest. They made great ease of use strides with 16.5 but still no library manager yet.. Perhaps V 16.6 will get one : )
Actually thinking about allegro I still use layout to create footprints and import them into Allegro because well it is easier : )
Best of luck with the migration
Great tip on creating library parts thanks!! Oh and supposedly 16.5 is to be installed at some point.
Now onto other topics, can Allegro really not bring in a simple title block and notes conversion,,, WTF
I tried moving them to an Assy layer but nothing comes over in the translation. I can't beleive they couldn't open the file in a mid version between 10.5 and 16 and upconvert. I used Pads for 17 years so I was used to support being supportive ;-)
I can't imagine a large company telling its customers they have to breate a bunch of work because we can't figure out how to tranlate our own files.
I got this from cadence:
I could find out that the Manufacturing Notes and the lines of the Title Block are not getting translated during Orcad Layout to Allegro Translation. This is a known limitation and we have asked our R&D team in past to add this functionality. But the issue is not planned for implementation in near future with the releases under development.
Unfortunately I could not find any work around for translating the data. It will be required to add these title blocks as Format Symbol in Allegro PCB Editor.
As I am not in condition to provide any support regarding this known limitation, I am planning to close the Service Request.
Don, I was incorrect about having the TitleBlock on the assy layer in layout. It should be on the FAB layer. Moving between tools I guess I got my layers mixed up. Anyway I opened one of the .tch template files in layout which contained a title block. I saved out the file as a max file and then imported into allegro.
The import of the template worked good and came across OK as far as I can see. In Allegro it put the fab drawing on the Assembly_Detail layer.
I added some notes to the max file fab layer to see if they would import into allegro and they came across ok. Text size needs adjusting but other than that the template looks good.
Give that a go and see if it works. I was using layout 16.2 for the test.
I got it to work finally. I stipped out all the copper area's through the spreadsheet and got it to come in but the text sizes are all messed up and overlaping the successive lines. Now I've got to get the text size and import our Logo, it was the cause of the copper area's.
Thanks for your help in this Scott!!! I'm still amazed tech support couldn't figure this out over a week long user..