Slot holes for DC jack connector in Eagle CAD

Hi Charly,

It's a common problem with these connectors. There are a couple of options. One is to draw the shape on a new layer and send it with a note to the manufacturer to explain what you want (they will mill it, so you need to let them know what diameter tool to use) or the other (simpler) method is to have a huge hole (i.e. design a custom part with a much larger pad) and accept that it will be mostly empty when you solder the part (only useful for prototypes). I just do the latter for prototypes to be honest.

Hi Shabaz,

Thank you for your quick answer. I'm interested in the first option (i.e. "draw the shape on a new layer and send it with a note to the manufacturer to explain what you want (they will mill it, so you need to let them know what diameter tool to use)".

That might sound naive but how do I export (what job do I select) a single layer? I read somewhere that some manufacturers use layer 20.

Also what the note to the manufacturer should contain?

Thanks

Charly

Hi Charly,

The layer number doesn't matter, but best to use a unique number (e.g. 100). That way, the board outline cutting tool doesn't need to be the same as the one for the small slot you need for this part. You can just select the layer when you are in the CAM processor view, assuming your board contains a part with that layer.

The note should just say "Please cut a slot based on the following filename: MYBOARD.SLOT and please use a 1mm tool to cut the slot, and please plate through-hole for the slot".

I selected the layer when I was in the CAM processor interface but can't get the right information. I enclosed a doc file with what I did.

Attachments:

Support Eagle.doc

Hi Charly,

I just tried it, but I used CAM Processor and then File->Open->Job and selected gerb274x.cam, and then clicked on 'Add' to create a new tab, gave it a name (e.g. bob) and set File to %N.bob and then just selected the desired layer (I wouldn't advise 20, better to use a unique layer, otherwise it's going to be confusing if the slot is not the only thing on the layer).

Then, the generated file (filename.bob) contained some long text string inside which I believe is the machine command for the slot.

Hi Shabaz,

I followed your instructions and it worked.

I ordered 3 boards today. Hopefully it'll be ok.

Thank you for your support.

Charly

Let me add the section of the manual that deals with exactly this subject:

8.13 Components with Oblong Holes

If the board manufacturer has to mill oblong holes, you have to draw the milling contour of oblong holes in a separate layer. Usually this is layer 46, Milling.
The milling contour for components that need oblong holes can be drawn with WIRE (and possibly ARC) with a very fine wire width near or even 0 inthe Package Editor. Take a pad that has a drill diameter which lies inside the milling contour, or SMDs, for example in Top and Bottom layer, as basis forthe oblong hole.

In case of a multilayer board you should draw a WIRE in the used inner layers at the position of the oblong holes so that it covers

the milling contour and leaves a kind of restring around the opening.

Please inform your board manufacturer that they have to take care on the milling data drawn in this layer. Also tell them whether

they should be platedt hrough or not.

Any other cutouts in the board are drawn in the same way:
Use a separate layer, typically layer 46, Milling, and draw the milling  contours. Tell your board manufacturer that they have to take care with  this information and make special note.

Regards,

Richard