Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
System Development 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'm having a great deal of difficulty completing/verifying what should be an easy task - I would like to generate a .art (gerber) file that describes the board outline. In this case, I just want to generate a simple rectangular outline. I'm using 16.5.
What I have done:
-turn off all layers in Display->Color Visibility
-turn on Board Geometry->Outline in the same color dialog box
-set active layer to Manufacturing->Photoplot_Outline under Options
-trace the Board Geometry->Outline layer in the Manufacturing->Photoplot_Outline layer
-turn off Board Geometry->Outline layer so that my newly drawn Manufacturing->Photoplot_Outline layer is the only layer shown
-go to Manufacture->Artwork, rt-click on existing film, Add
-leave undefined line width as 0 for the new layer (or change to non-zero values 1 or 10 - tried multiple values)
-open a new job, File->Import->Artwork, select newly created Outline artwork
-in the same import window, leave default class/subclass options (or select new options, but Manufacturing/Photoplot_Outline is not a selection option)
-try to load, get a message that says No Photoplot file specified
1) Am I generating the board outline gerber in a wrong/difficult way, or am I trying to view the board outline gerber in a wrong/difficult way (or both)?
Any help or advice is greatly appreciated! Thanks in advance.
Manufacturing->Photoplot_Outline subclass is used to define the overall extents of your gerber file and it is not used to define the board outline. The Manufacturing->Photoplot_Outline subclass is not required as Allegro will default to the drawing extents when generating Artwork, if it doesn't exist.
Basically, the Artwork film record must contain Board Geometry->Outline subclass and the Undefined Line Width must be set to a number higher than 0. I updated your steps below:
What I have done: (updated)
-set active layer to Manufacturing->Photoplot_Outline under Options (SKIP)
-trace the Board Geometry->Outline layer in the Manufacturing->Photoplot_Outline layer (SKIP)
-turn off Board Geometry->Outline layer so that my newly drawn Manufacturing->Photoplot_Outline layer is the only layer shown (SKIP)
- leave define the undefined line width as 0 10 for the new layer (or change to non-zero values 1 or 10 - tried multiple values) ---> You must define an Undefined Line Width and it cannot be 0. I normally use 10.
Hope this helps,Mike Catrambone
In reply to mcatramb91:
Thanks for the detailed and quick response Mike.
I tried your modified procedure, but I find that I am still unable to import the generated file in order to review it (maybe I'm missing a setting somewhere else entirely?) In fact, when I open the "Load Cadence Artwork" window, I can select "Board Geometry" Class, and "Outline" Subclass, but when I actually point the Filename field to my generated file, I hear a beep and my subclass field selection automatically changes to "Plating_Bar", and "Outline" is no longer offered as a subclass selection. I am not offered a "Load file" button to select in the bottom middle of the window as I am with my other artwork layers.
If it helps, here's what I see when I look at the contents of my outline file in a text editor:
G04 ================== begin FILE IDENTIFICATION RECORD ==================*
G04 Layout Name: C:/SPB_Data/test.brd*
G04 Film Name: Outline*
G04 File Format: Gerber RS274X*
G04 File Origin: Cadence Allegro 16.5-S014*
G04 Origin Date: Sat Jan 18 14:00:43 2014*
G04 Layer: BOARD GEOMETRY/OUTLINE*
G04 Offset: (0.00 0.00)*
G04 Mirror: No*
G04 Mode: Positive*
G04 Rotation: 0*
G04 FullContactRelief: No*
G04 UndefLineWidth: 10.00*
G04 ================== end FILE IDENTIFICATION RECORD ====================*
In reply to mfris:
It seems "pretty likely" that, whatever Class / Subclass you drew the outline on, it's was not on Board Geometry / Outline since this file contains no data, "M02*" is the "end of file" marker and the preceding contents are just control records.
Check that you do not have any objects defined on Manufacturing>Photoplot_Outline since no Artwork data is generated for any design objects outside of the Photoplot_Outline objects, set only the Manufacturing>Photoplot_Outline colour to visible and delete all objects from that subclass. You can usually ignore getting the warning for not having any Photoplot_Outline defined.
Also, when you import the Artwork data back into PCB Editor, you should avoid using the "database" classes and subclasses in most cases since the "database" classes and subclasses can rely on some design intelligence and the Artwork data is just collections of instructions to control a photoplotter and, as such, contain no design intelligence. A typical practice is to use Setup>Subclasses and add user defined Manufacturing Subclasses to import the Artwork data into since these will not try to impose any intelligence onto the imported data.
In reply to oldmouldy: