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.
While routing the design, I want to assign etch width of 0.2mm for particular package symbol having 48 pins & for rest of the design I want to set minimum etch width as 0.3mm. One way I think to assign pin level property but don't know which one.
Thanks in advance
There is a couple ways of controlling the etch width automatically:1.) You can define a Constraint Area around the component and specify that the etch width in that region to be .2mm. If you are using Allegro prior to SPB 16.0 the Constraint Area etch width will be applied thru all layers of the design just make sure to update the Physical Assignment table to call out the .2mm Constraints Set for the Constraint Area. This can be a pain because you may only want the etch width reduced on the external layer where the 48 pin component is placedIf you are using Allegro SPB 16.0 and above you would define a Constraints Region on the Top Layer and just specify the etch width in Constraints Manager under the Physical Section in the Region worksheet tab.2.) If you are planning on manually pin escaping this 48 pin component you change your Physical Neck Width to .2mm and the Line Width to .3mm to avoid any DRC Errors (You would also need to specify a Max Neck Length as well). You can temporarily change your Line Width from .3mm to .2mm then pin escape the 48 pin component then change it back to .3mm when you are done. Recommendations:If you are using Allegro prior to SPB 16.0 I would use step 2 above.If you are using Allegro SPB 16.0 and above I would use step 1 above.Hope this helps,Mike CatramboneUTStarcom, Inc.
Hi Mike,Actually for Option 1, using v15 (.1,.5,.7) and some time back, you can define the constraints area to adhere to all the 'other layer' properties (.3mm), and only set the Top Layer to something different (.2mm). I'd do it by copying the DEFAULT constraint (.3mm) and having a "BREAKOUT" physical property with Top Layer at .2mm. This will route from the device (constraint) area at .2mm width, then change to .3mm beyond the area.I do this with my BGA that route out of my constraint with .1mm, then changes to .125mm once I'm beyond the BGA breakout. I can set my internal layers to anything else, if I want, by mod'ing the PHYSICAL CONSTRAINTS.Good day.Mitch
Mitch, This is very true, that you can modify your .2mm physical constraints set so it just has the modified etch width for the Top Side. The point I was trying to make is that Constraint Areas are defined thru all layers for the designs prior to SPB 16.0 while in SPB 16.0 you can simply define a Constraint Region > Top then assign rules to it and never have to worry about what happens on any other layers.Mike