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.
New to the 16.5 release of Allegro PCB Editor is the ability to establish via patterns during group routing.
Group Routing Review
The Allegro PCB Editor supports interactive group routing. Interactive group routing is the routing of more than one net concurrently. You can use this feature when routing a bus with traces that follow the same path and have common physical and electrical rules. To specify the nets for group routing, select the elements (such as clines, pins, vias, and ratsnests) from which to route either by using the Temp Group option from the add connect pop-up menu, or selecting the elements with a window. Routing proceeds from the selected elements.Note: You can initiate a route by selecting ratsnest lines provided that you have enabled Ratsnests in the Find Filter. To reduce the incidence of accidental ratsnest selection, the editor ignores the ratsnests if you also select other types of elements.Note: If you are routing from a component with a complicated pin pattern, route from each pin to a location outside the component area. Then group the routes together (outside the component area) in the order that you want to route them as a group -- that is, organize the routes outside the component area so that the layout editor can order and space them properly.Read on for more details …
Via Pattern Support
Via pattern support during group routing is available when you are in the add connect command. You can add vias during group routing in both the modes-Alternate mode and Working layer mode. With the Alternate use-model enabled, you can select the via from the Options tab. With the Working Layer use-model enabled, you can pick the target-layer from the Add-Via dialog box. For adding vias in group routing, the same padstack (or via-stack) is used for all selected clines, and is determined by the control-trace. A DRC may appear if a padstack is invalid for one or more of the selected clines.
Adding Via Patterns during Group Routing
Select the add connect command using Route — Connect and create group to add vias. In the following figure four cline segments are selected. The control-trace is shown by the white X:
Now select via-pattern from pop-up menu and add the via by double clicking the cline segments. The vias remain in the floating state until one additional click is made. New clines will gather, and then group route continues on the new layer. The via-pattern is created, and all the vias will slide dynamically as a group in the direction of the control-trace. The control-trace via is placed directly along the control-trace cline, with no extra vertices added. Extra vertices are added for the other traces if needed.
Types of Via Patterns
There are six type of via patterns. You can select the via pattern from pop-up menu. The Next Pattern option can be used to cycle to the next via pattern in the list:
The shape of the via-pattern can change depending on which cline is the control-trace. To change the control-trace use the pop-up menu. Taper patterns produces the same result as one of the diagonal patterns if the control-trace is at the either of the end. If the vias are small, and/or the selected clines are already far enough apart, in group routing vias are added in-line, with no extra vertices.
Adding Stacked Blind/Buried Vias During Group Routing
For designs using stacked vias, you can select only those layers that can be reached with a single via-stack. The layers that can only be reached with staggered vias cannot be selected for adding vias in group routing. The example in the following figure shows three via-stacks (labeled "1-3"). You can add stacked vias during group routing by invoking the command once:
If via-stacking is not allowed on layer three, then in order to add the vias from layers 3-to-6 you need to select add via second time, with layer six as the target layer. You can move vias labeled "3:6" vertically up or down until you click to drop them. To avoid any DRCs with the "1-3" via-stacks the "3:6" vias are placed in staggered form.
Please share your experiences using this new 16.5 capability.Jerry “GenPart” Grzenia
Hi Kyle -
Group routing is available in OrCAD PCB Designer Professional, but not all of the options are there.
Some of the options available through the Allegro PCB Editor XL license (but, not available through the OrCAD PCB Designer Professional) are:
Single Trace Mode
Change Control Trace
Enhanced Pad Entry
You can see the available options by using the RMB while in the Route command.
Is group routing, including all of the features described above, available in OrCad PCB Designer Professional suite?
Are you asking if this functionality can be made available in PCB SI?
Can you include this in SIP?