Home > Community > Blogs > PCB Design > what s good about allegro via patterns during group routing see for yourself in 16 5
Login with a Cadence account.
Not a member yet?
Create a permanent login account to make interactions with Cadence more conveniennt.

Register | Membership benefits
Get email delivery of the PCB Design blog (individual posts).


* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

What's Good About Allegro Via Patterns During Group Routing? See for Yourself in 16.5!

Comments(4)Filed under: PCB Layout and routing, PCB design, SPB, Differential Pair Support, Allegro PCB Editor, High-Density Interconnect, HDI, Allegro, via, PCB Editor, PCB, layer stacks, layout, PCB Capture, "PCB design", global route, design, routing, differential pairs, diff pairs, blind vias, buried vias, SPB16.5, Allegro 16.5, inset vias, via rules, staggered vias, vias, group routing, via patterns

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


By Ronald Gatdula on June 27, 2012
Can you include this in SIP?

By Jerry GenPart on June 27, 2012
Hi Ronald,
Are you asking if this functionality can be made available in PCB SI?
Jerry G.

By Kyle on September 26, 2012
Is group routing, including all of the features described above, available in OrCad PCB Designer Professional suite?

By Jerry GenPart on September 26, 2012
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:
Add Via
Via Pattern
Route Spacing
Single Trace Mode
Change Control Trace
Neck Mode
Enhanced Pad Entry
You can see the available options by using the RMB while in the Route command.
Jerry G.

Leave a Comment

E-mail (will not be published)
 I have read and agree to the Terms of use and Community Guidelines.
Community Guidelines
The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. 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. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.