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:
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?
Best Answer
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,
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.