Eagle Pro: Dimension layer on all gerber files.

Hello,

Ive just done a 4 layer pcb in eagle pro.

I see its recomended in youtube video to only put the "dimension" layer on the silkscreen gerbers.....but shouldnt the "dimension" (board outline) be on all the gerber files?..eg top copper , top cream , inner2, etc etc

No. It would end up as copper or solder paste (and the solder paste mask would fall apart). Just put it on the dimension layer and combine it with the top silk screen for the Gerbers.

Keith

i thought it (dimension) had to be with the bottom silk screen too?

I don't think it should matter either way as long as it is on one layer, but it won't do any harm (unlike putting it on the solder paste layer). It is really just there so the PCB manufacturer knows the final dimension/shape.

Keith

Hello,

I only put the "dimension" layer on the top and bottom silk gerbers.

The boards have come back from the manufacture...and the inner cutout has not been cut out....it is a solid PCB with no cutout, and has silkscreen line where they should have placed the cut.

The silkscreen line depicts where the edge of the cutout should be.....i cannot understand this, it was on the "dimension" layer, so how have they managed to put a silkscreen line there?

Do you know what's gone wrong....?

Should i have put the "dimension" layer on all gerbers after all?

The board is a solid PCB of the right outer shape, but there is no cutout.
The cutout was to be a rectangle of approx 5mm by 20mm

I looked at the silk gerbers and i can see the cutout shape on there.

What has gone wrong...is it my fault, or the PCB house?

You never mentioned that there was a cutout! That would normally be routed (milled) out and drawn on the 'milling' layer. You would then need to add the milling layer to the list of Gerbers you produce and make sure the manufacturer knows what the layer is for.

You can draw it on the dimension layer as well but because the dimension layer is not normally plotted on its own it is not enough information to know what should be milled out.

Keith

Thanks,

its strange because the first lot of boards we got made, were made by a different place, and we sent the dimension layer on all the gerber files, and they did do the cutouts, even though we had not done a separate milling layer.

Anyway, do you think we can send these pcbs back and get the cutouts laser cut out of the pcb?

I cant understand what you say about the dimension layer not being enough....the dimension outlines depict exactly the cutouts and board external edges, so howcome its not enough?...if i do a separate "milling" layer, then that just duplicates the info that's already on the "dimension" layer

The dimension layer would be sufficient for the milling if it was plotted separately but it is not so clear if it combined with the silk screen layer unless you provide additional notes. A 'box' drawn on the silk screen layer does not mean you want a hole in the PCB.

You should be able to get the holes milled out afterwards. A machinist can do it.

Keith

I wonder how the pcb makers new the external edge of the board was where it was.....why did they not think that was silkscreen?
...right , i am getting it now, even though Eagle declares it as a "dimension" layer, they in the board house simply dont see that info, all they see is a line.

Correct. You have to consider what information you have given them in the Gerbers, not the information in Eagle.

Keith

If you want cutouts or slots etc in your board then it helps the manufacturers if you tell them so, perhaps by providing a mechanical drawing (often referred to as a drill drawing, but with more than that on) which includes dimension markings and text to identify the cutout etc.

You can also include other information such as the board dimensions, dimensions from board edge to a mounting hole, laminate, plating, finish information etc.

While the data may contain the information it can be helpful to the manufacturer to have the information that you are trying to give them in such a drawing. If they are in doubt they can refer to it.