Altium Designer Documentation

Solder Mask Expansion Enhancements

Modified by Jason Howie on Apr 11, 2017
All Contents

With today’s board designs, situations can arise during PCB development where the applied solder mask needs to offer different expansion settings for the top and bottom layers.

In the case of through-hole pads and vias for example, those used as test points need to be closed on one layer and exposed on the test contact layer. This need is resolved with the release of Altium Designer 15 which now offers pad and via expansion settings that can be individually configured for the top and bottom layers.

The new pad and via solder mask expansion settings are reflected in all the applicable definition points within Altium Designer, such as the pad/via property dialogs, and the relevant Inspector panel, and implemented via expansion rules.

Expansion settings

Via/Pad properties

Solder mask expansion settings for individual pads and vias can be defined through their properties dialog (Pad dialog, and Via dialog respectively). Select a pad/via and choose Properties from the right-click context menu, or double-click and select the desired pad/via.


The solder expansion for an individual pad/via is specified through the Via/Pad dialog.

The Solder Mask Expansions settings, normally configured to adopt the expansion set from Rules, needs to be set to Specify expansion value to define specific values for that via or pad. Here, the settings will default to matched values for the top and bottom layers until unlinked with the  button.


Unlock the Top/Bottom settings to define individual solder expansions.

PCB Inspector Panel

Individual Solder Mask Expansions settings can also be defined in the PCB Inspector panel by checking the Solder Mask Override object parameter to enable the settings. Separate top and bottom layer settings become available when the Use Separate Solder Mask Expansion checkbox is enabled.


Use the PCB Inspector panel to define pad/via solder expansion setting in bulk or individually.

Using the PCB Inspector panel to define specific solder expansions provides the added benefit of being able to reconfigure multiple pads of vias in one action. Select several pad/via objects in the workspace using Shift or Ctrl + click, the PCB Filter panel or the Inspector's Include... option. The top/bottom -layer expansion settings can then be defined in the PCB Inspector panel for all selected vias or pads.

Design Rules

Solder Mask Expansion Rules that apply to board pad and vias can be defined or modified through the PCB Rules and Constraints Editor dialogDesign » Rules on the main menu. Select the Solder Mask Expansion rule category in the rule navigation tree. Not the checkbox to enable separate top/bottom -layer solder expansion settings.


The Rules and Constraints Editor now offers enhanced solder expansion settings for pad and vias.

To apply specific top and bottom expansion rules for a particular Net for example, define the applicable Net in the query match (upper section of dialog), check the Use Separate Solder Mask Expansion option and enter the desired expansion distances for the Top and Bottom layers. The rule will apply where pad and via expansion settings for that net have not been individually overridden.


Creating a rule for separate top and bottom layer solder expansion settings.

 

If you'd like to comment on the content on this page, use the Ctrl+Enter keyboard shortcut to send us your feedback. To include a section of the page in your comment (a typo, missing/wrong info, or incorrect imagery), highlight the text (max. 200 chars) and/or image first. Please restrict your feedback to documentation issues - for technical assistance refer to the Altium Forums.

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:
Request Free Trial

Complete this form to request a free 15 day trial of Altium Designer: