I'm a student and am almost ready to have a PCB I designed fabricated, but I'm confused about how the board outline should be defined.

Here's what I currently have:

enter image description here

I also have a 20mil keepout line centered on the board edge, but hid the layer to make the board outline visible.

I'm planning on ordering the board from a company called Gold Phoenix PCB. I've emailed them several times about this, but haven't been able to get a clear answer. They said:

You only need to design the board in the way you want, size tolerance +/-10mil

Not helpful!

Then after sending the above image:

Make things simple, you need keep everything 10mil from the edge of the board.

Ok, 10mil from the edge of the board, but what do they consider to be the edge? Is it the center of the 10mil track I placed on mechanical 1, or is it the edge of the track?

The example I gave them when asking how the outline should be defined is:

Let's say your router bit diameter is 90mils and it follows the center of the line defining the board outline -- that means it would be cutting 40mils too deep into the board, which would not only mess up the connector alignment but also create a risk of shorts since I only have a copper pullback of 20mils.

I've already emailed them four times about this and don't want to get on their bad side, so can anyone explain the correct way to define the board outline to meet my requirements?


You can define the board shape either way you want.

If you tell the shop that you are providing a board outline, they will make the outer edge of the board follow the center of the line in your gerbers.

If you tell the shop that you are providing a route tool path, they will make the routing tool follow the center line, and the edge of the board will be offset from that by the radius of the cutting tool.

For a simple board, it's better to provide a board outline and let the fab shop generate the route tool path for the size of tool they want to use.

If you want to have inner corners, or only partially depanelize the boards or something, then you might want to provide a route tool path. In Altium, look for the "Generate Route Tool Path" command to generate the path easily.

In Altium, for a board outline, typically you just use the Keepout layer to define it. Of course if you want you can redefine one of the mechanical layers to be the board outline and use that instead. If you generate ODB++ output instead of gerbers, there will be board outline information in the ODB++ based on the actual defined board outline in Altium, not any paths on any particular layers.

Since different layout tools name their gerber files differently, I suspect that most shops just look through the gerbers for a layer that looks like it has a board outline and use that (but it's better if you give them a readme file that says what each gerber file represents)

In a comment you mentioned,

No, I don't have a "fab drawing." I'll try to figure out if this is possibly in Altium.

Typically for simple boards Altium users just use the Drill Drawing layer for the fab drawing. If for some reason you want to have separate fab drawings and drill drawings, then you can again just rename one of your mechanical layers to be the fab drawing.


The middle of the pink line is the board edge you are defining. The width of that line is a CAD/visual construct and means nothing to the fabrication process. The keep-out applies only to electrical (i.e., metal) portions of the design. You can typically take silk all the way to the edge of the board. Based on the polygon you have just above the "RAW" PTH, you likely are as close as you can get to the edge of the board with this connector (looks like a pin header). If you want to have the yellow (black plastic of pin header) directly to the edge of the board, you will have to decrease your keep-out.

The keep-out is for your own protection so that when they cut the PCBs from the panel, and apply mechanical stresses to the edges of the board, they aren't inadvertently breaking any of the metallization causing random opens/shorts.


I would say you should define the dimensions of your board in your fab drawing, you do have a fab drawing right :) Showing your stackup, and board outline, and clearly labeled finished dimensions? Maybe some notes about finishes, and hole tolerances? That will take the ambiguity out of trying to communicate with them.

Also you shouldn't be worried about getting on your fab houses bad side, if they are tough to work with, or can't give you answers go somewhere better. Of course at the same time it's a two way street so you want to be respectful when dealing with them. Ideally your fab house is your partner, and part of their job has and will always be educating new engineers/customers ;)

Good luck.


It might depend on the board house.

I use a 100mil line as the outline of my board and treat it as the kerf of the router. That means if you want to align a component with the edge, align it with the inside edge of the outline.

If you still haven't got a satisfactory response from the board house, use a different one. There are hundreds of options. I suggest OSH Park.


You have the board outline defined with the dotted line, so you don't need an outline on the mechanical layer, and the Gerber files should come out with the correct board outline. You can check that the Gerbers are correct by viewing them with a Gerber viewer like GC-Prevue.

  • \$\begingroup\$ Altium shows the dotted board outline in the editor, but it's not included in the gerber files. That why I manually drew the 10mil (pink) line on the mechanical 1 layer. \$\endgroup\$ – Nate Mar 13 '15 at 20:47
  • \$\begingroup\$ That's strange. With the Pulsonix software I use there is an "Insert Board" command which puts the board outline on all the board layers. It then comes out correctly on the Gerbers. It's all very easy. \$\endgroup\$ – Leon Heller Mar 13 '15 at 20:51

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.