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.
I have a PDF called A basic intrduction to Cadence Orcad (Allegro) 16.2 PCB Designer.
I have been following that to help me learn this program, so far it has worked but when I make the artwork (gerber files) Fig.25 says the Board Outline is not included in the films. Why is that? the PDF doesn't give me a reason why.
Doesn't the PCB Manufacture need the outline to make the board?
The PCB software I use now is Orcad Layout 9.0 and I can make outlines for the Artwork (gerber files).
Any help is appreaciated...
It's related to your board outline being zero (0) in width or thickness. Under the aerwork settings there is a undefined line width. Specify a value here (I suggest 10 mils or 0.254mm). Remember to do this for each artwork. You will then see a thickness in your gerber data. Some people generate an artwork that just contains the board outline.
In reply to steve:
Thanks for the info, I'll give it a try and let you know...
Actually it's not needed. It's comfort food for them. There have been 1 or 2 specfic vendors I've used in the last 100 or so boards that asked for it as a cross-check. Outputting it on its own film is best. Just create a film, set up just the outline to display, match the film to the display and then set the line width for plotting for this layer. Voila!
In reply to redwire:
I tried putting 10 mils in the undefined line width box for each artwork and I left everything else the way it was and it still didn't work.
In reply to Dennis H:
Dennis. Can you please confirm that the board geometry / oultine class/subclass is included in the artwork film you are viiewing ?
Sorry to be a pain, The board outline/outline/subclass looks like it is included. Is there a box to check or as long as the outline say Board Geometry/ outline...
Dennis. It should look like below. Make sure when you have the outline.art selected that the undefined line width is shown. (You have to repeat this for each artwork. (It's not a one off setting).
Thanks it worked, the PDF you sent helped out. After I opened it I knew what I was doing wrong....
It's late and I'm totally busted - but my 16.2 also seems to ignore the "undefined line width setting" for the outline... Showing the films looks fine (BoardGeometry/Outline layer is included in films)!
So I thought I could just change the outline in the BoardGeometry/Outline layer. NOT: "E- (SPMHGE-544): Rectangle line width cannot be changed.". Ended up (embarrassing!) drawing a line on top of the outline rectangle. That worked - but was only plausible because it was a simple outline!
Reminder to self: Find out best practice (or just a rational one) for including outline in artwork... ;-)
In reply to N i z e:
Check that the undefined line is set on a film by film basis. It's not a one time set for all artwork films. Click on the film name and check the value.
Every single film had undefined line set at 0.05mm - the outline showed up in none of them. Hence, I suspect this is more a question of my outline being wrong. Something like a rectangle (in the Allegro terms - not the geometrical sense ;-) not being a proper outline. (I still not quite understand why Allegro is so picky with the different types ;-)
Guess I should check some of the other designs - I don't remember it to be problem earlier...
You have always been able add a thickness to a line item not a rectangle in tne Allegro sense. Do you have a photoplot outline Colors - Manufacture - Photoplot_Outline) set to the same size as the board ? This would probably clip the outline off the artwork, Personally I never use the photoplot outline but if you must make it 1000 mils larger than anything you want in the artwork.
Steve, you are absolutely right: The Photoplot_Outline was the culprit!
I still have a felling that there might be a better "best practice" for this - but using the undefined line width is definitely a fair, usable solution. (Only strange the parameter can only be set one film at a time ;-)
Thanks for the insight! :-D
After reading this thread I felt the urge to respond. The PHOTOPLOT OUTLINE was used years ago to restrict the output file to a certain length and width. I think this was used by people that use to put formats on their artworks rather than just a title block. I think most, if not all fabricators read the gerbers into their CAM system where they can check and manipulate anything that they need to. Then, they will either go directly into the photoplotter or generate their own artworks. So 99.9% of the time it is not needed. If it is there, the system will reduce the extents of the gerber data to just that window. If it is not there, it will use the Film Size Limits specified in the General Parameters section of the Artwork Control Form which I think is 24 x 16.
Next, I think just about everyone who is fabing boards these days can read 274x format at a bare minimum. I would not even mess with the old 275 format. Even better, if you are using CAM350,ADIVA, or Valor to check your artworks, I would be using ODB++ or IPC-2581 if you can. We have been using ODB++ for over 3 years without any issue and it puts eveything into ONE file. We even include our Fab Drawing, Board Outlines, Panel Outlines, and anything else we think the fabricator might need. We leave the board outline and other things like dimension lines and text on the fab dwg at 0 line width and it still transfers into ODB++. Heck, even the free ViewMate gerber viewer can read ODB++ data. Time to get out of the Dark Ages boys and girls. Just MHO.......;-) I feel much better now thankyou.
In reply to Boma:
Thanks for your thoughts! Actually I think the photoplot outline is a fairly good feature*. As are many of the Allegro features. My main problem is that the help system primarily (only?) waste time - so this forum is ususally a much better help. I try to remember writing notes - at some point someone should read a nice, short "Allegro essentials" guide. It might be out there already - but I failed to find it so far! ;-)
Interesting stuff! I always felt the 274x should be obosolete - but I've never had the energy to convince everybody that it was a sensible move...However, ODB++ surely sounds nice! Checking around I've (unfortunately) found no manufacturer that claims the capability (Macaos, EuroCircuits, PCB123, 'all' the Chinese). And I'm way to small a customer to ever impose anything on a manufacturer.
Regarding "everybody [...] can read 274x", I actually had to give up on Olimex (a small, cheap Bulgarian manufacturer that I've loved to use for simple prototypes and test circuits. And cheap shipping!). The initial response when I changed to Orcad PCB/Allegro was:
"Your gerbers contain composite layers and negative
plots (G36 G37 commands).On such gerbers we can't do DRC check, panelization
nor to ensure correct phototools plotting."
After several tries to solve this we had to give up. One manufacturer less to choose from - sadly!
Have a great weekend! :-D
*) PS: I'm fairly convinced that Allegro either made the photoplot outline for me - or reported an error about needing it! At least it does not seem probable I've suddenly felt an urge to create it on impulse... :-P