Altium Designer Documentation

Custom Coverlay Support

Modified by Jason Howie on Apr 11, 2017

A common feature on rigid-flex boards is the selective use of coverlay material. This insulation layer is cut and laminated onto specific areas of the board, and because of this selective use, custom coverlay is often referred to as bikini coverlay. As well as its use in specific areas of the board, custom coverlay can also be positioned anywhere in the layer stack.

Custom coverlay is added in the Layer Stack Manager dialog and the shape manipulated in Board Planning Mode, once the Custom Coverlays option is enabled in the Board Region dialog for that region of the board. 

Adding and Configuring Custom Coverlay

Custom coverlay is added in the Layer Stack Manager dialog, as a dielectric layer.

To add custom coverlay:

  1. Select the required layer stack in the lower region of the Layer Stack Manager dialog.
  2. Add a dielectric layer into the stack in the upper region of the Layer Stack Manager dialog and adjust its position in the stack.
  3. Define the properties of the coverlay, including the Coverlay Expansion property.


Add the coverlay layers into the required stack and configure the layer properties in the Layer Stack Manager dialog.

Enabling and Viewing the Custom Coverlay

Custom coverlay must be enabled for each board region where it has been added to that region's layer stack. To enable the custom coverlay:

  1. Switch to board planning mode (View » Board Planning Mode) to examine and edit custom coverlay layers.
  2. Set the PCB panel to its Layer Stack Regions mode, and double-click to edit the required Stackup Region.
  3. In the Board Region dialog, enable the Custom Coverlays option.
  4. In the main workspace, there will now be additional tabs for each custom coverlay layer added in the stack, click on a layer tab to make that layer the current layer, and examine the layer contents.


Custom coverlays must be enabled for each Stackup Region that includes them, note that this coverlay extends into the rigid region, as per the Coverlay Expansion
defined in the Layer Stack Manager dialog.

Editing, and Placing Additional Custom Coverlay

Coverlay is automatically added to cover the entire area of the board region is was added to, as shown in the image above. Behaving like an additional solder mask layer, openings are automatically created for component pads in accordance with the applicable Solder Mask Expansion design rule, or else the settings in the Pad dialog if the Solder Mask Expansions setting has been configured to override the design rule.

  • The automatic coverlay is formed as a polygonal object, it can be selected and reshaped (or deleted) as required.
  • User-defined coverlay shapes can also be placed if required, using the Design » Place Coverlay Polygon and Design » Place Coverlay Cutout commands. Note that these commands are only available in Board Planning Mode.


An area of user-defined custom coverlay has been placed (with curved corners), including a cutout. To the right of this, the automatic coverlay has been moved away from the left edge of the board.

Keep in mind that user-defined coverlay changes, such as modifying the shape of the automatic coverlay or placing additional coverlay objects, are removed if the Custom Coverlay option is turned off in the Board Region dialog.

Configuring the Coverlay Layer Color

The color of Custom Coverlay layers is defined on the Board Layers And Colors tab of the View Configurations dialog. Custom coverlay layers are listed in the Mask Layers region of the dialog.


Custom Coverlay layers are added into the list of Mask Layers in the View Configurations dialog, click to set the color of custom coverlay layers.

Understanding the Behavior of Coverlay Objects

Custom Coverlay is a mask layer, behaving as an additional Solder Mask layer. Solder Mask layers normally display and output as a negative, that is, the objects you see on the screen become holes in the fabricated mask layer. The on-screen presentation of Solder Mask can be configured to display as a positive, if preferred.


The central flex region of the board has a custom coverlay enabled, the view must be set to Board Planning mode to display it.


The Solder Mask layer is normally displayed as a negative.


The Solder Mask layer has been configured to display as a positive, when it is the custom coverlay is also fully displayed.
Note the manually placed custom coverlay shown on the left end of the flex region.

It is possible to view solder mask layers as positive layers, to do this enable the Show Top Positive and Show Bottom Positive options on the View Options tab of the View Configurations dialog, press L to open the dialog when in 2D mode.


Solder Mask layers can be configured to display as a positive, if preferred.

The 3 board images above show the top solder mask layer for the same board:

  1. In board planning mode, the custom coverlay can be viewed and edited.
  2. In 2D mode (single layer), note that the solder mask is shown as a negative, the objects displayed become holes in the fabricated solder mask. Note that in this mode, the software displays the solder mask for the upper and lower rigid areas in the same color as the central flex area. Note also that in this display mode it does not show manually placed custom coverlay.
  3. In 2D mode (single layer), the top solder mask is now shown as a positive. Note that in this mode, the software displays the solder mask for the upper and lower rigid areas in the same color as the central flex area. Note also that it shows manually placed custom coverlay.

In standard 2D display mode the custom coverlay is shown as if it was on the top/bottom solder mask - this is simply a display feature, when output is generated the top solder mask and the top custom coverlay are written out as separate data, as are the bottom solder mask and bottom custom coverlay.

How Output is Generated for Custom Coverlay

When output is generated, each layer is output as separate data. For example, when Gerber is generated, the top solder mask is written to one Gerber file, the top coverlay is written to another Gerber file.

The output for a custom coverlay can be divided into 2 categories:

  • Pad/via openings - the output for pad/via openings is generated in the same way as regular top/bottom solder mask output: an object of the correct size/shape is flashed, in accordance with the applicable solder mask expansion design rule, or the object settings if the local override is enabled.
  • Polygonal areas of custom coverlay (both automatic and manually placed) - a closed polyline outline is generated, defining the outer edge of each region of custom coverlay. The outline can be used to define a cutting path for the custom coverlay. Cutouts (user-defined irregular-shaped holes) defined in the custom coverlay are also output as a closed polyline for cutting path generation.

The centerline of the 1mil wide closed polyline is the edge of the custom coverlay.


Examining the Gerber output in a CAM viewer - the blue is the custom coverlay layer, the purple is the top solder mask layer.

Zoomed in, a custom coverlay cutout is selected - as with the coverlay outline the cutout is also defined as a closed polyline.

Supported Output Formats

Custom coverlay output is supported by all of the appropriate output formats available in Altium Designer. 

Coverlay film outputs

  • Gerber RS-274X, X2 - Openings defined over objects, such as pads and vias, are flashed. The outer edge of the coverlay, as well as user-defined cutouts, are rendered as outlines - these outlines can be used by the fab house to generate a cutting path.
  • ODB++ - Specific layer stack material regions are output (polygons and polygon cutouts) in ODB++ v7.0 and later, which properly supports multiple layer stacks and rigid-flex definitions.
  • IPC2581B - as with ODB++, supporting multiple layer stack definitions and polygons of layer stack regions.

Layer Stack Outputs

  • ODB++
  • IPC2581B
  • Layer Stack Report

Tool Outputs

  • NC / Excellon Route Tool Path - generated from outline for polyline objects.

Prints

  • Prints can be configured as required.

 

 

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: