Single Sided PCBs

Single sided PCBs tend to generate unusual errors, since many of the typical layers are missing. However, these designs are possible to fabricate using our 2 layer service.

SMD Designs without through-hole components

Designs with only SMD components do not require corrections. The missing layers won’t cause any fabrication issues in this case, and the errors can be ignored.

Simply verify that the previews match the desired PCB, and use the checkbox to approve the errors raised by our system.

Through Hole Designs

These designs typically only contain a single Copper and Stop Mask file, which isn’t sufficient to fabricate the board properly.

To make the correction process more straightforward, rename the existing files so they match our Suggested Naming Pattern.

When the design contains only Top files, you’ll perform the following

  • Make a copy of the GTS file, using the GBS extension for the copy.
  • Make a copy of the GTL file, using the GBL extension for the copy.

If the design instead originally contains Bottom files, then do the following

  • Make a copy of the GBS file, using the GTS extension for the copy.
  • Make a copy of the GBL file, using the GTL extension for the copy.

Optionally, you can use a tool such as GerbV to unwanted objects, such as copied traces. However, removing traces is not required: They will have identical electrical connectivity as the original layer.

Through Hole Designs with SMD components

This process is identical to process for through-hole designs without SMD components.

However, in this case using GerbV to clean up the SMD footprints on the layer copies. Due to how how the fabricated files will be, multi-pin SMD footprints will be “backwards” from the component, and accidental assembly will likely cause electrical issues. It’s simpler to correct now, and ensures you don’t make assembly errors.


Why does this cost the same as a 2 layer board?

We cannot fabricate a true “single sided board”, like you might seen in volume manufacturing. This involves a different process than anything we offer. However, with the correct layers, we can simply fabricate these boards alongside other 2 layer boards. Since the process is the same, the cost is too.

Why do I need the second stop mask file?

The “Stop mask” layers tell us where the copper on your PCB should be exposed so you can solder to it.

On through-hole designs with only a single stop mask file, this means your design files state “Expose one side of this plated hole, and cover the other side in epoxy”. However, when fabricated this way the hole will often be filled with epoxy, and be very difficult to assemble.

What if I don’t have any stop mask files?

This is a problem! Some older PCB files were generated with the intention of home-etching, and don’t contain all the layers needed for professional fabrication. In extreme cases, these projects may consist of exactly one copper file.

As long as the generated files are in Gerber format, it’s often possible to use a tool such as GerbV to duplicate and generate the missing layers via copying and editing. If you encounter trouble, email [email protected] for assistance.

What if I don’t want any epoxy on my board?

If you want to expose the entire board, then you need to provide a Stop Mask file file that indicates this. Omitting the Stop Mask files will not prevent epoxy application to your board.

Why do I need the second copper file?

Strictly speaking, this is not necessary. However, the via plating process results in better plated holes when the copper pads are present on both sides of the via. This typically also makes boards easier to assemble.

Do I need to do anything with the silkscreen files?

Generally, no. The silkscreen is almost always generated for Top or Bottom. Due to how how gerber files are generated, duplicating the silkscreen will just create reversed text that’s fairly meaningless.

In some cases, the design tool simply generates a “silkscreen” or “legend” file, and does not indicate Top or Bottom. Simply rename it according to the Suggested Naming Pattern to ensure that we detect it for the correct side of the board.