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.
Get email delivery of the Cadence blog featured here
The Allegro 16.5 release was made available on May 17, 2011!This release adds additional improvements and efficiencies to your design process.New technologies in Allegro 16.5 include advanced miniaturization capabilities, integrated power delivery network analysis, DDR3 design-in kit, bolstered co-design featured and flexible team-design enablement to address global designer productivity.Today, I’ll discuss the enhancements to the Allegro PCB Editor for a new standard EDMD schema. The EDMD schema is a new XML based data exchange format.
Historically, design data has been passed between ECAD and MCAD domains using interim file formats such as IDF and DXF. These formats have numerous limitations that prevent accurate and/or complete representation of data from the source design (whether ECAD or MCAD) in the target domain. Additionally, there has been no effective way to communicate proposed changes from one domain to the other without sending the design in its entirety. As a result, collaboration between these domains has been cumbersome, and it gets worse as the design progresses. Designers are forced to either extend the time it takes to do the designs or risk going to manufacturing with design errors, resulting in rework and delayed time to market.
This new approach allows ECAD and MCAD designers to pass changes they made to their designs in an incremental fashion. Additionally, the new standard provides a way for designers from both sides to accept/reject the changes proposed on an object by object basis. This provides a level of control, traceability and collaboration that has never been possible before. With only incremental design data being passed between ECAD and MCAD domains, designers spend very short time reviewing, accepting/rejecting the changes and ensuring that the two domains are in sync. This avoids any miscommunication that can result in rework and improving chances of first time success significantly.
Allegro PCB Editor 16.5 supports this new standard v2.0.
What is EDMD? EDMD Schema (file extension) is a file format for the Incremental Data Exchange (IDX) of data between Electrical and Mechanical data systems referred to as EDMD (Electrical Design Mechanical Design). Version 2.0 of the format contains the same data as IDF 3.0 without panelization data. IDX is Managed by ProStep iVip, a European based consortium
IDX formats give you the ability to preview changes graphically before accepting or rejecting the data. The main benefit of the IDX interface is it provides support of collaboration by using incremental changes with accept/reject and comments defining intent.
New in Allegro 16.5 is the IDX Import command idx in (File— Import — IDX).
Selecting "Import" will open the file browser to select the IDX file you want to import. Selecting "Import" again will open the "Select Items to Import" dialog to select the objects to import. All the items will be dimmed except for the changed objects.
Allegro will reject any Via changes.
There is no batch interface for importing IDX data. The new import process allows you to accept or reject individual changes; this is the heart of the IDX’s support for incremental change management and ECAD-MCAD co-design.IDX Export
The idx out command (File — Export — IDX) allows the export of IDX data.
The baseline will be created for the first export and the baseline will be attached to the database. If you want this new configuration to be the baseline, select the "Re-Baseline" button. The base filter configuration can be changed at this point using the button “Filter Options” button:
Just as in IDF import, the base filter configuration is used to exclude objects from the IDX file.
Selecting "Export" will open the "Select Items to Export" dialog:
One single IDX file will be maintained, and the new IDX data will be added to the existing processed IDX data.
Batch interface for IDX Export
The idx_out executable can be used to write an IDX file out of Allegro. The file extension is the same as the GUI output - “.idx”.Command syntax:idx_out <design_name > [-obsh] [-c <base_config>] [-f <increment_config>] [-i <baseline>] [-xp]-o Output file base name. Name of the resultant IDX files. Default: <design_name>.idx-c Base configuration File. Name of the file to use to filter the specified parameters from the resultant IDX file.-f Incremental configuration File. Name of the file to use to filter the specified objects from the resultant IDX file.-b Board Version. Valid Arguments: user specified integer. Default: 1-s System ID.Valid Arguments: user specified string. Default: ""-i Baseline used to create incremental data file.-h Default height. Applies this value to all package symbols without a specified package height.Valid Arguments: a floating point value consistent with the original design units. Default: 0.0-xp Export Plane_shapes, Clines, Pins, Vias, Test_points onlyExample 1: Baseline File:idx_out test.brd -o test_base -c idxFilterOut.config -h 150.00
Example 2: Incremental Data File:idx_out test.brd -o test_delta -c idxFilterOut.config -h 150.00 -i test_base
Example 3: Export Plane_shapes, Clines, Pins, Vias, Test_points onlyidx_out test.brd -o test_copper -c idxFilterOut.config -xp
Note: The format of the filter file is:(filter Vias Pins Plane_shapes Clines Test_points)
IDX versus IDF
When importing IDX data into a design that has IDF data/properties in it, the following prompt will appear:
Click No to exit. Click Yes to proceed and display “IDX In” dialog. When importing IDF data into a design that has IDX data/properties in it the following prompt will appear:
Click No to exit. Click Yes to proceed and display IDF In dialog.
As always, I welcome your comments about how you’re using this new 16.5 capability.Jerry “GenPart” Grzenia
Yep - "stump1019" and I exchanged Emails on this topic.
Hi Jerry, looking for the most up to date info on IDX transfer between Allegro and Solidworks. Actually my main interest is to find out how the communication between ECAD and MCAD works to communicate updates and comments during the IDX transfer.