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.
Hi all, I'm working my way through transitioning from OrCAD 10.0 to 16.5.
I've started a new design and have a few questions regarding board outlines in OrCAD PCB Editor:
1) How can I create board oultines where the lines are not at 90degree angles?
2) How can I type in coordinate points for my board outline?
3) Is there a way to copy a board outline from an existing .brd file and paste it into an existing design? The Help -> Documentation mentions a "boardoutline import" which is supposed to be under File -> Import -> Board. This doesn't seem to exist and the command is not recognized when I type it into the console. Am I missing something? I did notice the documentation pulls up Allegro PCB Editor and there is no entry for OrCAD PCB Editor...
Add>Line, Options: Board Geometry / Outline, Line Lock set to "Off" for any angle, 90 or 45 are possible, also Arc can be used instead of Line for arcs.
Add>Line, Options: Board Geometry / Outline, type x<space><XLoc><space><yLoc><enter> at the Command line for each point, you can also use the incremental "picks", ix<space><xInc><enter> and iy<space><yInc><enter> if you prefer increments. Like:x 0 0ix 250iy 1000
and so on, you will need to add points until the outline is completed in one go. Entering co-ordinates won't care about the line lock.
You could display only the outline and Export a DXF from that and then Import the DXF to another BRD file. You could copy and rename the BRD file in Windows Explorer and load the Logic into it - in 16.6 one BRD file can be a template for another design.
In reply to oldmouldy:
Thanks, oldmouldy. I'm surprised under Setup -> Outlines -> Board Outline, the same options for line locks don't exist!
It sounds like unless the board outline is really complex, it will be easier just to construct a new board outline.
Is it true that it is impossible to copy shapes, lines, etc from design to another? This was a very normal part of OrCAD 10 which I miss. I can't even find a way to open 2 designs simultaneously just to visually compare them.
In reply to B Price:
You will find many things you miss from the old program.
You can not open two files at once. You shouldn't have been able to do it in the old one either, but you could. I had a designer at one time who kept opening two files at once and saving the wrong one................
Can you not do a file>export>sub-drawing of the outline in orcad? That's an easy solution in Allegro.
Actually you can open two designs if you are running Allegro PCB Editor.
Make sure to also have an install of OrCAD PCB Editor, even if you don't have a license.
You can open open OrCAD PCB Editor in demo mode and have the other board open in Allegro PCB Editor.
I do this a lot to compare changes between the same boards.
In reply to Kurt222:
Genious, Kurt222. That sub-drawing export is so simple and clean - this is the easiest way I've seen to copy/paste between designs.
Thanks everyone for your valuable input!
I was able to create a polygon for the board outline by using the Add Line tool and choosing the Board Geometry/Outline class/subclass.
I was hoping to do the same thing for the Package Keepin and Route Keepin, but those classes are only available for Add Rectangle. I can't change the class of an existing poly line either...
Is there any way to designate non-rectangular Package Keepin and Route Keepin ?
If you already have a board outline then use Edit - ZCopy to create the package and route keepin. Check the options fold out menu on the right hand side to set the layer to copy to and the "offset" amount (contract / expand) then click on the board outline.
In reply to steve:
I am having trouble with this concept. I don't see where the 'options' are for the export so it is not clear how to specifically export the board outline as a sub-drawing.
Do I need to be in a specific mode?
What steps should I take before executing the Export->Sub-drawing to get a sub-drawing of the board outline?
In reply to DCowl:
Update note: in the OrCad 17.2 version of Allegro there is no zcopy but Shape->Copy Shape seems to have the same functions. The documentation still talks about zcopy but entering zcopy in the command line just gets E-command not found: zcopy
In reply to bpTech:
I see, Thank you very much!
Learn Vietnamese online( free for all cadence's members ):
Lession 1: nho ninh thuận