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.
On my design that I converted from Orcad I have several package to package errors. Since we had our library shapes set up so that components could be placed line to line this is an issue. Is there some place I can change this? ThanksSandy
Sure can. Edit the symbols (ORcrap symbols that you converted to Allegro), and change the PLACE_BOUND_TOP to the "actual" size of the part. I'm guessing the translation expanded the boundry. Next, create a text file (like UPDATE_SYMS.lst), and add the symbol names you've changed. Next, in Allegro, do PLACE/UPDATE_SYMBOLS; check the symbol list (browse to your file); and update the symbols. If your constraints are set right, your errors should go away.I know it sounds long, and drawn out, but it's fairly painless to do 10-15 parts. I do that on almost all my converted drawings (mostly coming from PADS). Also helps to have a 'generic' symbol library to pull from, so you don't have to continually mod common parts.Good day.Mitch
Ok, this makes sense and thats exactly what happened. How do I change the size of the place_bound_top box? I haven't ran across anyplace I can move these boundaries in. Does this make sense? ThanksSandy
Placebound_top is a shape. In the symbol editor, you can either delete and redraw the placebound, or edit the shape.Regards,Harold
OK, thanks to all of you I have that figured out. Now I need some advice on fiducials. In Orcad I had fiducials as part of the footprint and could move them to where I wanted them to be. Is there a way in Allegro to edit and move them locally or should I add them seperately? Also, how do I now get them off my translated PCB without the whole component being removed?Sandy
Sure can.Edit the symbol.set the property: UNFIXED_PINS to TRUE.You will now be able to move/delete the fiducials that are a part of the symbol.BE VERY CAREFUL you don't move other pins in the part though :)The 'local' package boundry can be mod'd too inside the layout. I do this all the time, when I need place things close together, and I know it's not a DFM issue.Good day.Mitch
Using SHAPES - tricksEdit Shapes - Move vertices around the shape (you can change from ALL LAYER grid to ETCH grid to increase accuracy.. good to know) Delete vertices - simply select a vertex and RMB delete Edit boundry allows you to REALLY modify the shape, good for quick changes Next is important for keeping the selections going.Good day.Mitch
Thanks for all you help. I am sure I will be here asking other questions as I get used to Allegro.Sandy
OK..one more question for now. Where is UNFIXED_PINS located? Is this done on the .brd file?
If you are in a boardMenu SelectEdit > PropertiesSelect the symbolIn the Edit Property GUI scroll down on the left to select the Unfixed_pins property to move it to the rightSelect OKThe property will be added to the symbol instance. You will be able to move the pinsIf you are in the symbol editorMenu SelectEdit > PropertiesIn the Find filter "Find by Name" section set the pulldowns to "Drawing" and "Name"Select "More..."In the "Find by Name or Property" dialog move "Drawing Select" to the right hand sideSelect "Apply"In the Edit Property GUI scroll down on the left to select the Unfixed_pins property to move it to the rightSelect OKThe unfixed_pins property will be added to the drawing and you can move or delete the pin(s)