PCB DFM: how would I go about cutting a hole in the PCB?

[Andrei_Dragan]

Hey guys and gals, I'm in the middle of designing a "portable-ish" wireless speaker and I'm stuck on the control interface of the thing.
I want the control panel to be a capacitive touch interface, with the PCB as the front panel, and a screen behind it to display stuff, but I don't know how to draw the cutout for the screen in the PCB.
I want to use Seeed for manufacturing because they are dirt cheap for boards less than 100x100mm, but they have little to no information about milling on their site, and I think they're intentionally trying to avoid my questions. I've asked them how would I need to go about for doing this for a week now and no response. There's somewhere some information about panelizing that says the minimum milling slot width is 2mm, so I'm guessing they have 2mm milling bits and larger, so I've made the window with rounded corners (with a radius of 1mm), but I need someone to help me out here a bit.
Do I leave it like this? Do I need to draw milling slots around the perimeter of the window and put in break vias (or what they're called)? How is this done?
Below is a screenshot of the board view along with the whole eagle project (including the libraries).

https://mega.nz/#!d9FkFaLb!L0w0c8DNDrJTtDovOp3QAmnM2lryJw0HYStKQhUHBmM

[T3sl4co1l]

That looks good.  Add a dimension (X and Y) from outer edge to inner edge, to fully define the shape.

2mm diameter I think is pretty conservative, and if that's fine for your application, great!  I've never had a problem with specifying 1mm diameter (40 mil minimum width slots).  Usually somewhere in the 0.8 to 1.2mm range is the minimum they do standard, and if you ever need less, you can probably do it in a custom run.

I don't know what Eagle uses, but other tools have a PCB cutout object, or you draw a shape on the board outline layer, or something like that.  For Gerber generation, generate an output for the board shape as well (layer usually being outline, or keepout or mechanical or drill drawing, one of those).  Fab only sees what's on the Gerbers, so no matter how the shapes get there, make sure you have this.

Tim

[Andrei_Dragan]

They provided the cam jobs, and the mechanical layer includes the dimension and milling layers by default. Can I put the dimensions on those layers as well, so they appear in the gerber files, along with some text or what not, or it's better left with only the shapes and nothing else? It's my first board that goes to a manufacturer and I have no idea of what I'm doing

[T3sl4co1l]

Dimensions should be on the drill drawing, which is usually printed (say to PDF) but not plotted to Gerber.

When they see an e.g. MyBoard.GKO file, they'll expect to see the board outlines here, and nothing else.

Tim

[Andrei_Dragan]

Got it, thank you very much for the feedback and info.
Have a wonderful day!

[hcglitte]

There is an acute angle on the track going from the ground plane to the resistor in the lower left corner.

[Andrei_Dragan]

I've moved the tracks a bit to get more room around the touch pads, and there's no right angles anymore. And that thing is not a resistor, it's a side mounted LED on the bottom side of the board, for a bit of backlight illumination, and a small copper pour in the top layer to act as a reflector. I don't know if it will actually work, I've not done it before and I don't think the PCB material is transparent enough to illuminate all the buttons, but it's gonna have an effect nonetheless . I'm curious to see how opaque the black solder mask is.

[hcglitte]

See the arrow.

[Andrei_Dragan]

Ah okay, is there a problem with it? I know it used to be a problem back in the day because the feeric chloride can accumulate there and can etch away too much copper, but now I think the manufacturing technology evolved a bit to not be an issue anymore. Like I said, I'm kinda new to this so if you can explain what's the matter with it it would be great.

[hcglitte]

I would remove them if you can. Better to be on the safe side. I have also read online that some manufacturers may complain.

[Gribo]

You have few via in pads, try to avoid those, it drives PCB cost up a bit.

[T3sl4co1l]

The length-matched traces are adorable, considering the ground plane underneath is chopped up to hell and there's no stitching.   (Add top side pour, and place GND vias generously around traces cutting through both pours.)

Tim

[chhrisedwards]

The X-ray drill tool is used to make hole in the PCB. Hole can be made through the centre of the inner layer pads. To set up the drill the operator first puts a panel of exit material on the drill bed. This stops the drill tearing the copper foil as it comes through the PCB.  Then he loads one or more PCB panels, and a sheet of aluminium entry foil. The drilling machine is computer-controlled. The operator selects the right drill program.  This tells the machine which drill to use and the X Y co-ordinates of the holes.

[Pack34]

Are J1 and J2 rotated the wrong way? If side-mounted it looks like the connectors would collide with other components.

[Andrei_Dragan]

Nope, the connectors are mounted the "right" way around. The panel is supposed to be hot-snotted around the edges to a case (with a reasonably large hole for the cables), so inserting the cables from the outside of the panel was not an option since it wouldn't sit flat. It turned out to be okay, if it didn't it's nothing a dremel can't fix in a personal project
I was slightly disappointed that the pcb manufacturer didn't put any silkscreen on the bare pcb material, and I also learned that the FR-4 isn't as transparent as it seems, and it can't be edge-lit in a reasonably uniform manner, so I need to redesign the board at some point in time and come up with another way of lighting up the thing.