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 have design I have done with buried resistors and and blind vias the
board vendors is stating that there are several shorts and several open
when they compare the netlist to the geber data. I do not have valor or
any other too analyze the netlist against the gerber data. I can view
the gerber data through GCPrevue and I can not see the shorts on the
nets they are stating that have the shorts and the same for the opens.
Allegro board has no opens or shorts either. Just wondering if anyone
else has seen a problem with the IPC356 netlist generated by alllegro
on release 1`5.2 s134.
Any help is greatly appreciated.
Thanks in advance
HiHow did you create the buried resistors? Did you create a seperate layer and build the resistors out of Lines? If you did then included the lines in your artwork you would receive shorts from the IPC356 Netlist. Since each end of the buried resistor is on a different net when the resistor is added to the artwork it creates a short. Buried resistors create challenges for Allegro. It and IPC think of resistors as components added after the board is built. If you are on current maintance you can get the ODB++ from Valor for free and it includes the Valor viewer. It is very dangerous and potentionaly expensive to send out gerber data without post process checking. The cost of one set of bad boards is more expensive than one seat of a gerber tool like CAM350. Hope I helpedBill
I couldn't agree with you more. I have preached
those same words to my management but they are so tigh that when you
hold them upside down their change doesn't fall out of their pockets.
Apperently they have more faith in me than they have in tools like that
and don't see the need as I have not yet given them a bad board to work
with. But I feel I am living on borrowed time here with the
technologies I am getting into and given the limits of Allegro DRC
system, which really in all is the best I have worked with as far as
PCB design goes.
I created the buried resistors as component which came from the ORCAD
schematic the pins are modeled as padstacks on the specific layers they
are designed on. There is a second artwork layer is generated for 2nd
etch process for the resistive material that is model as a shape on the
package geometry layer. I can't see any reference to that in the IPC
Anyway the problem turns out to be a netlist interpreatation problem on
Valors part but maybe someone from Cadence wants to look into this also
since they are connection partners. This is directly from TYCO
Silverstorm P/N 310034-000 Rev 0
Investigate/Document CAD netlist issue
After analyzing the data and the CAD netlist files, I
have found that all the issues were caused by translation errors.
Most of these have to do with the format of the buried
resistor networks and blind vias in the netlist text file.
I've detailed the issues below for customer information,
but I'm approving the CAD netlist as verified to Gerber data.
Part of the resistor network contains the pad the
resistor is tied to:
307MN_DQ31 R543 -2 P
Our input is interpreting this as access side bottom, and
creating issues when this runs into features on the bottom side. Due to the
method of analysis in the Valor software this generates both shorted and broken
Removing these lines from our file eliminates both
Can you raise a Service Request with Cadence? This way Cadence can look into the problem officially and pass it over to Valorif need be. Cadence will need a copy of the brd that you have, maybe also a IPC netlist pointing out the problemAndy