Common Errors with Board Outlines

Our service requires a board outline gerber, which indicates to us and the fab where the edge of your board is to be located. This layer is used by our service to generate the billing cost based on your board area, as well as enabling us to remove data that lies outside your board to avoid affecting adjacent designs. The fab also uses this outline to determine how to cut your board out from the panel.

There’s a large number of errors that can complicate generation of this layer, as well as several errors we commonly see submitted by users. If you’re not able to solve the issue with the following information, feel free to email your files to support@oshpark.com, and we’ll do our best to help.

Example of a well-defined board top preview Example of a well-defined outline preview

Errors and Issues

“My board preview is missing, but the layers look fine.”

This is due to the outline not being fully connected along the outer edge. In most cases this is due to a missing line somewhere, which means we can’t fabricate the board correctly. Once the outline is completed, this issue will resolve itself.

In some cases, this is simply due to a small gap where the outline wasn’t fully connected. Many design tool’s DRC checkers will help locate this gap.

“I can’t find a board outline file.”

If the file is there, check the suggested naming patterns for your tool. For many tools, we require the filename to have a .GKO extension.

If the file is simply missing, check out our design tool help for how to generate the file.

In some cases the outline might be present, but only on a different layer. You can use GerbV to create an outline from those files.

This is a problem: can't find the outline

“Board Outline Image: [Can’t be blank]”.

Either the board outline gerber was generated with no outline, or we picked up the wrong file name.

We have specific help pages for a lot of CAD packages, so check the list to see if we have instructions on how to generate board outlines for our service.

In some cases the outline might be present, but only on a different layer. You can use GerbV to create an outline from those files.

This is a problem: the outline file can't be blank.

“Board must be larger than 0.25”x0.25”.

This generally means the outline didn’t contain the information we need. Generally, make sure that the outline is drawn on the layer intended for your design tool.Our Design Tool Help page will typically list what layer works best.

This error sometimes occur when a design has non-plated drill hits, but the outline is missing. Several design tools (notably Eagle) generate circles on the outline layer around the non-plated hole. Putting the outline on the correct layer will resolve this.

If the design is actually less than 0.25” in one or both dimensions, we likely cannot fabricate it correctly. Increasing the size slightly is often the best resolution. Contact support for additional assistance if needed.

This is a problem: the area inside the outline is too small.

Circles on the outline without a board outline.

The size reported by the site is smaller than the actual size.

This is often similar to the above issue, with the outline not being present on the outline gerber.

In some design tools (notably Eagle), this is often related to the above issue with non-plated holes. For this, make sure the outline is drawn on the Dimension layer.

In other design tools (Notably Altium), this issue is sometimes related to assembly data in GM1 or GM2. Either ensure the outline is present in these files, or delete the files if they don’t contain the outline.

This is a problem: circles on the outline without a board outline.

This is a problem: Pick and place symbols without a board outline.

The size reported by the site is larger than the actual board size.

This is usually related to extra data on the board outline gerbers. Usually this is due to one of following issues:

For help with specific tools, see our design tool help pages.

Usually you can modify the CAM settings to avoid generating this data in the first place. You can also use a tool such as GerbV to remove any extra gerber information from the board outline file.

Eagle users sometimes see this issue when using TO-220 footprints with drill holes near the board edge (often mosfets and voltage regulators). The best solution is to use a “vertical” or non-drilled version of the part.

The problem is our site thinks the measurements are part of the board outline.

The problem is our site thinks the fab text is part of the board outline.