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.
HiIn the Orcad capture schematic environment when we try to copy a page in a project file and paste it into an another project all designators automatically changes.How can I preserve them from changes?It is important to me to save all designators without changes.Thanks a lot
Go to Options - Preferences - Miscellaneous tab and check the box for Preserve Reference on Copy.
In reply to steve:
steveGo to Options - Preferences - Miscellaneous tab and check the box for Preserve Reference on Copy.
Thank you for your answer. It was a good idea , but according to the product help this option is not supported for complex hierarchical design. I tested that option in a complex hierarchical design , all designators changed to “?” sign after paste action , for example U1A to U?A, but in a flat design it worked properly and all designators remained without change.
unfortunately all my designs are complex hierarchical design.Do you have a better solution for complex hierarchical designs?
In reply to 09127751201:
In a complex hierarchical design, Capture has one schematic and "n" sets of properties for the parts, if you copy a part, which of the "n" sets of properties to copy? No simple answer so, as things stand, no simple solution. And, for a PCB Design you need to get to unique references, so what real purpose to preserving the reference?
In reply to oldmouldy:
oldmouldyif you copy a part, which of the "n" sets of properties to copy?
I agree with you. It has no simple answer. In this condition if you have a “brd” file (PCB File) based on a complex hierarchical design , if you copy these files (including Schematic and PCB files) to another project you will lose designator synchronization between schematic files and PCB file.
You will not lose the designator information unless you re-annotate the schematic. If you need to copy the whole project either do it in Windows Explorer or in 16.6 use File - Project Save as.
I have a similar problem, except that I am using a flat design (not heirarchical), and I am using OrCAD 16.6-S001.
The Options->Preferences->Miscellaneous->Automatically reference placed parts is unchecked/disabled, and Preserve reference on copy is checked/enabled.
When I try to copy entire pages from Capture project A to project B (both flat designs), the reference designators are reassigned to ?.
When I try to copy one or more component symbols from project A to project B, the reference designators are reassigned to the next logical unused reference designators for project B.
OrCAD is behaving like it is either operating on a heirarchical design, or something else is preventing the preservation of reference designators, such as perhaps I don't have another setting defined properly, or don't understand a concept that I thought I understood.
I realize I have not got the most recent service patch for OrCAD, so perhaps this is a bug that is now fixed?
I am unable to progress unless, I suppose, make a copy of design A that I wish to have the designators preserved in and copy paste over the design B that can have its reference designators reassigned, and then save it as design B.
In reply to bradenmarr:
What mode is the design in Instances or Occurrences ? I would also say I've just tried this using S027 (latest hotfix) and it works as expected so get to the latest hotfix if you can.
Thanks for putting a lightbulb over my head, steve!
Using your hint about Instances and Occurrences, I found this blog page:
and on project A pushed all occurrence properties to instance properties by doing,
1. Select the .DSN in the project tree (for project A)
2. Accessories->Transfer Occ. Prop. to Instance->Push Occ. Prop. into Instance
and in the dialog box chose the first option, "This option will push the occurrence level values of the part reference and PCB footprint properties as instance level values." and checkboxed the "Use this to remove all the Occurrence properties from the design and change the preferred mode of your design to instances"
This generated a report of all components changed, and though it noted that each affected component's reference designator was being changed to ?, it correctly preserved the reference designation on each schematic page. (I haven't yet checked to see if other properties were preserved in this conversion.)
I was then able to select the pages from project A, copy, and paste them into to project B and the reference designators were preserved on copy! :-)
I'm not sure why some components were "occurrences", but perhaps this could have happened when editing the schematic with copy paste commands, pasting from other schematics outside of project B, or properties were edited (such as our custom "Populate" property that is either blank/invisible or "DNP"/visible), or perhaps the components added to the schematic from CIS were somehow altered. Now I know that a "flat" design, while it is being created and edited, can somehow spontaneously begin to contain components with modes that are otherwise normally expected for a heirarchical design.