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.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
This course combines our Allegro PCB Editor Basic Techniques, followed by Allegro PCB Editor Intermediate Techniques.
Virtuoso Analog Design Environment Verifier 16.7
Learn learn to perform requirements-driven analog verification using the Virtuoso ADE Verifier tool.
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 would like to hear about users that are successfully using allegro DFA and have integrated their contract manufactures rule set into this process and how the integration was accomplished.
All replies are appreciated
Sorry for the delayed response. Just getting caught up with the new community. I will be at CDNLive! in September and we can get together and go thru how I integrated the DFA checks into our PCB Design flow.
OK Back to your question:
We have been using the Real-time DFA Checks for a while now with great success. We had our own in-house manufacturing group that developed amatrix of component clearances which we imported in the Allegro DFA Spreadsheet. We already had a Microsoft Spreadsheet of the component clearance matrix so I was able to output a tab delimited file and with some tweaks I was able to open it up inside of the DFA spreadsheet in Allegro.
Here is a breakdown of some migration issues that I ran into which may be helpfull (Using SPB 15.7 during migration):
DFA_DEV_CLASS can only be placed inside of the.dra symbol. Adding at the Board level has no effect.
Adding DFA_DEV_CLASS properties can be added to the symbol library using DFA_DLG but it also added the DFA Boundary.
DFA_DLG would not run on large directories of symbols. Wildcards which contains over 100 symbols tends to crash with a Fatal Software Error. Ran on SPB 15.7 on WinXP and did not see an issue. Appears to be limited to Solaris/Linux installation.
DFA_DLG would generates only sqaure DFA Boundaries even if the Assembly Outline is round.
DFA_DLG generated DFA Boundaries using all Assembly Outline data including pin 1 markers. Wrote SKILL routine to delete oversized DFA Boundary, then copy Place_Bound_Top to DFA_Bound_Top to correct issue. Place_Boundary was created correctly in library going out to the edge of the pins so it was OK to copy it to DFA_Bound_Top.
DFA_DLG does not have an option to just add the DFA_DEV_CLASS property for library which have the correct Place_Bound_Top defined.
DFA_DLG updates dra symbols and generates PSM in the same diretory so it needs to be manually moved into the symbol directory. Not a major issue but would be nice to have an option to specify location of output .psm file.
DFA Spreadsheet can be created using Microsoft Excel but be careful of blank spaces in Class names and clearance values.
Sorry for the brain dump but it may be usefull to you.
Hope this helps,Michael CatramboneUTStarcom, Inc.
In reply to mcatramb91:
In reply to TamiWright:
DFA_DLG is the standalone program of the DFA Spreadsheet in Allegro. At the symbol level you would add a property called DFA_DEV_CLASS to define the DFA Group or Classification for the symbol. These classification are loaded in the DFA Spreadsheet then you can define clearances between the different classification of symbols.
It is really a lot to explain so I would recommend checking out the "Best Practices: Working with Real-Time DFA Analysis" in the Cadence documentation to give you a good idea how it all works. You can also access a PDF version of the Best Practices by browsing to it in Windows Explorer by entering %CDSROOT%\doc\algroDFA.
Good luck,Mike Catrambone