Altium Designer Documentation

Routing Via Style

Modified by Jason Howie on Apr 11, 2017
All Contents

Rule category: Routing

Rule classification: Unary

Summary

This rule specifies the style of vias that can be used when routing. You have the option to define specific Min/Max/Preferred values for the via's diameter and hole size - defined as part of the rule's constraints - or use via templates available to the board design.

Via templates can be local (for vias that are saved with the PCB design file), or can be sourced from one or more Pad Via Template Libraries (*.PvLib), installed as part of the available libraries set.

Constraints

Default constraints for the Routing Via Style rule.

  • Mode - use the drop-down to choose from the following two modes:
    • Min/Max preferred - choose this mode to set the permissable values (Minimum/Maximum/Preferred) for the via's diameter and hole size as part of the rule itself.
    • Template preferred - choose this mode to be able to use via styles defined through via templates available to the board.

Mode = Min/Max preferred

When this mode is chosen, the constraints region changes to present the following options:

  • Via Diameter– specifies constraint range values to be adhered to with respect to the diameters of vias placed when routing the board. The following individual values are definable:
    • Minimum – the minimum permissible value for the via diameter.
    • Maximum – the maximum permissible value for the via diameter.
    • Preferred – the preferred value for the via diameter.
  • Via Hole Size– specifies constraint range values to be adhered to with respect to the hole sizes of vias placed when routing the board. The following individual values are definable:
    • Minimum – the minimum permissible value for the via hole size.
    • Maximum – the maximum permissible value for the via hole size.
    • Preferred – the preferred value for the via hole size.

Mode = Template preferred

When this mode is chosen, the constraints region changes to present the following options:

  • Templates List - lists the available via templates that can be used with the rule. These are via templates (local or defined in Pad Via Template Libraries) that are made available to the board design as part of the Local Pad & Via Library (accessed through the PCB Pad Via Templates panel). For each available template the following information is presented:
    • Template Name - the read-only name of the template. For a local template, auto-generated naming is used, in compliance with IPC standards, For a template sourced from a PvLib, this naming can be customized as part of template configuration within that library.
    • Description - the read-only description written for the template.
    • Library - the library from which the template is sourced. This can be <Local> (where the via is defined and saved with the PCB document) or the name of the external Pad Via Template Library (<LibraryName>.PvLib) which has been made available to the PCB document.
    • Enabled - enable this option to have the template made available for via placement during Interactive Routing.

How Duplicate Rule Contentions are Resolved

All rules are resolved by the priority setting. The system goes through the rules from highest to lowest priority and picks the first one whose scope expression matches the object(s) being checked.

Rule Application

Online DRC, Batch DRC, during autorouting, during interactive routing.

When the mode of the rule is set to Min/Max preferred, the following considerations apply:

  • The Preferred via attributes are used by the Autorouter.
  • The Minimum and Maximum via attributes are obeyed by the Online DRC and Batch DRC.
  • The Maximum and Minimum via attributes also determine the range of permissible values that can be used during interactive routing - when you press the + (or *) key on the numeric keypad to toggle routing signal layers and drop a via, press the / key on the numeric keypad to place a fanout via, or press the 2 shortcut key to place a via without changing layer.
  • Press the Tab key while routing to access the Interactive Routing dialog, from where you can change a value within its defined range. If a value is entered outside of its range, a dialog will appear alerting you to this fact. You will be prompted to either continue, in which case the value will automatically be clipped, or cancel and change the value yourself.

When the mode of the rule is set to Template preferred, the following considerations apply:

  • When a routing via is placed, you can cycle through the available via options by pressing the 4 key. In this case, the options will toggle through the via templates that have been enabled as part of the applicable rule.
  • Press the Tab key while routing to access the Interactive Routing dialog, from where you can change the via template currently applied.

Tips

In order to control the size of blind and buried vias, individual rules can be set up targeting the different layer pairs. For example, to control the via size for blind vias between the top layer and mid layer 1, the following scope (Full Query) can be used:

(StartLayer = 'Top Layer') and (StopLayer = 'Mid-Layer1')

To control the via size for buried vias between mid layer 2 and mid layer 3, the following scope would be used:

(StartLayer = 'Mid-Layer2') and (StopLayer = 'Mid-Layer3')

Alternatively, instead of creating individual rules, you can expand the one rule query using ORs as follows:

((StartLayer = 'Top Layer') and (StopLayer = 'Mid-Layer1')) or((StartLayer = ' Mid-Layer2') and (StopLayer = 'Mid-Layer3'))

 

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

You are reporting an issue with the following selected text
and/or image within the active document:
ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.

Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.