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.
Hi, All. I need to get a solution to define a region which has the direction information just like 'horizontal' in Allegro PCB Router. Because there are many edge connectors that has different gap between horizontal and vertical. So I want to route with horizontal directon at the area where the connector will be placed. Is this possible in Allegro PCB Router? Any idea or solution will be really appriciated. Best Regards, JY Lee
Hi JY: I do not know of a way to define the solution in Allegro and just pass it to Specctra. I avoid using Specctra regions for Specctra auto routing unless absolutely stuck. (Stuck less that 5 % of the designs) I have done the type of connector you have by setting up special conditions in the Specctra do file that is used to auto route. 1. define a group (set of fromto's) by selecting the component and defining selected as a group conn_gr1. 2. Have Specctra route these first with a special temporary set of rules costs etc that will apply only to them since only they are routing while these costs rules etc. are in place. a) temporarily set the layer direction horizontal on all layers that these route into the connector on: direction SIG3 horizontal do for all layers b) cost way 80 (tells specctra that going vertical on a horizontal layer is not desirable. c) rule pcb (limit_bend 20) (wiggling up vertically will exceed the bend limit choose an appropriate number that will allow horizontal entry but limit vertical navigation. d) If there are few large blocks of unused pins and gnd pwr pins define a wire keepout over those few large clusters. (stops vertical navigation through them) Commands: unsel all routing sel group conn_gr1 route 25 clean 3 unsel all routing #change the above rules and costs back to default of what is normal including layer direction. direction SIG3 vertical (all layers that were temporarily changed) cost way -1 rule pcb (limit_bend -1) select all routing unsel group conn_gr1 # should route the other connections without serious movement of conn_gr1 route 25 # put in the number of route passes needed for the non conn stuff to get the conflicts down #to convergence stopping. # only if necessary (still too many conflicts) as clean may mess up the horizontal on vertical layers. # at this point change direction to direction 'L05-SIG2' orthogonal (on all layers.) unsel all routing route 25 1 route 25 16 #This will allow minor adjustments in the connector connections if necessary to clear the last few conflicts that are involved in with the other routing. Hope I am remembering this all right for you. Hugh Allen Specctra Specialist CopperCad Design Inc. www.coppercad.com firstname.lastname@example.org