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.
Okay how do the pros set this up quickly? I find for each board it is a very tedious and painful process to get the correct folders set up and the classes and subclasses to get the silkscreen and soldermask and etch all setup. I turn colors on and off in the workspace then add the folders and still find I work to do to get it all correct. In this regard I definately liked the simplicity of Layout but hope it's just operator ignorance.
Setup the films that you need for the data other than "ETCH" layers. Then in Film Control, select these layers checkboxes, NOT the etch, hover the mouse over a film name and right-click>Save All Selected - this will write a file called "Film_Setup.txt". Move this from the design folder to "somewhere" that you store common design data. Then, for the next design, go to the Artwork, Film Control and use the "Add" button, pick the saved "Film_Setup.txt", and your "other films" will be added to the output list. NOTE: the Film_Setup.txt file will have the parameters from you original design embedded so check carefully if your designs have some english and some metric databases, or use differing resolutions, decimal places - since the parameters stored are "numbers" and do not have units attached.
In reply to oldmouldy:
Allternatively you can use a Parameter file. Go to a board that has everything defined and use File - Export - Parameters, Make sure that at least Artwork is checked but there is also design settings, color layer and palette, text size and application / command parameters, export the file, then on your new board file use File - Import - Parameters, browse to the location and import, everything is defined.
You could try the attached skill program, place it in your skill folder and run using "ns_gerber" command. Feel free to edit the code to suit your needs.
In reply to Ejlersen:
why i can not run Revision 15.7?
oldmouldySetup the films that you need for the data other than "ETCH" layers. Then in Film Control, select these layers checkboxes, NOT the etch, hover the mouse over a film name and right-click>Save All Selected - this will write a file called "Film_Setup.txt". Move this from the design folder to "somewhere" that you store common design data. Then, for the next design, go to the Artwork, Film Control and use the "Add" button, pick the saved "Film_Setup.txt", and your "other films" will be added to the output list. NOTE: the Film_Setup.txt file will have the parameters from you original design embedded so check carefully if your designs have some english and some metric databases, or use differing resolutions, decimal places - since the parameters stored are "numbers" and do not have units attached.
In reply to steve:
I had the same question as the OP. The methods steve and oldmouldy outlined both look great.
If I save a board template with the film control configured correctly, will it carry into a new design if I use that template board as an input file?
I guess it boils down to whether the Parameter file contents are automatically part of a .brd template...
In reply to B Price:
No, the parameters will not follow your board file.
I would recommend you to setup a site environment, it involves the following
1. create env variable inside system settings and call it cds_site with a value of a path on the Network e.g., u:/rd/Cadence
2. create folder structure u:/rd/Cadence/pcb/nclegend and place your golden nc_param.txt in this directory.That will be the basis for all your new boards with respect to drill parameters
3. inside folder structure u:/rd/Cadence/pcb/ place your golden art_param.txt in this directory.That will be the basis for all your new boards with respect to artwork parameters
You can enhance this with a lot more functionality if you want, for example
site.env file with default shortcuts, settings etc. inside u:/rd/Cadence/pcb folder
If more than one user, just create the cds_site variable on each client and then you share the setup.
You can read more about this in the readme.txt file inside C:\Cadence\SPB_16.6\share\local\pcb
Also a complete example configuration directory structure is shown at C:\Cadence\SPB_16.6\share\local\pcb
Thanks, Ole - I'll give this a try. It sounds very reasonable.
Edit: I looked into that readme. Am I correct in assuming step 3 should read as follows?
3. inside folder structure u:/rd/Cadence/pcb/parameter place your golden art_param.prm in this directory.That will be the basis for all your new boards with respect to artwork parameters
thanks Regards, Mani