5
\$\begingroup\$

I'm trying to make a hole partially through a PCB in Eagle to allow a reverse mount led to shine through to the other side. I got this idea when I saw a torch shine through a pcb where there was no ground plane on either side as shown below.

enter image description here

I have some 1206 SMD leds and want to figure out how to design a hole in Eagle that only cuts through about 1/2 of the pcb or layers 1-15. I did some googling and couldn't find anything relating to this.

\$\endgroup\$
  • 2
    \$\begingroup\$ Use a milling machine. \$\endgroup\$ – Andy aka Sep 19 at 9:51
  • 4
    \$\begingroup\$ That would be something you arrange with your PCB fabshop. \$\endgroup\$ – Peter Karlsen Sep 19 at 10:20
  • \$\begingroup\$ Surely there is a way to specify it in Eagle \$\endgroup\$ – Vinson Cai Sep 19 at 10:24
  • 5
    \$\begingroup\$ Can you elaborate why you think there is a way to do that in Eagle? What you request is a post processing step to be done after manufacturing, and before assembly. You will probably need to arrange for the bare PCBs to be shipped to a machine shop where they can mill the PCB for you, and then ship them out to the assembly house. This is not standard, and thus probably not included in Eagle. \$\endgroup\$ – Vladimir Cravero Sep 19 at 11:02
  • \$\begingroup\$ I thought it was common enough for it to be possible in Eagle, I guess not. This is a low volume piece so I guess I'll mill them myself. \$\endgroup\$ – Vinson Cai Sep 19 at 11:40
5
\$\begingroup\$

This is something which is usually not covered by the functionality of common EDA-Tools like EAGLE.

Here's why: This is done by milling after processing all other production steps of the PCB. It can't be done by just omitting something in the prepregs used, as they can contain only drills for vias. And the latter is only done when buried vias are needed.

Milling through some of the layers is rarely needed, so there is no standard in handling those special requests. It can't be defined in gerber or drill files. There is no need to describe it in an EDA tool, as this doesn't make any sense, when no CAM file can't be generated to describe the necessary milling actions.

There is a milling layer in EAGLE, but it it's only purpose are millings through all layers of the PCB.

You might need some luck to find a PCB manufacturer who is even able to do such millings.

I recommend to add a new layer for each milling depth you want to have on your PCB and export it as DXF along with the alignment marks. Then explain your demands to your favourite PCB manufacturer and see what happens.

Edit: There are further arguments, why EAGLE doesn't provide mechanism to describe intricate millings. Most layers describe electrical features and the copper layers can hold information only on the distinction where to remove copper and where not. There are no layers describing the prepregs and where they should have gaps or not.

\$\endgroup\$
  • \$\begingroup\$ Thanks for the lengthy explanation. Good to know that it isn't actually possible to do in Eagle, I was looking around for a couple hours to no avail. I'll contact my manufacturer or mill it by hand. Thank you! \$\endgroup\$ – Vinson Cai Sep 19 at 11:39
0
\$\begingroup\$

If your going to do this, you might be able to create an additional mechanical layer and supply that to the manufacturer. It's been a while since I have used eagle, and it's my understanding that you can't create additional layers. One way to get around this would be to use a gerber editor (like viewmate) and create the mechanical layer in viewmate.

Either way an additional file would need to be used. Contact the manufacturer and ask them if they could create a hole in the layers that you want. This will create additional cost for you (and it might be a lot of additional cost), as the manufacturer will have more steps in their process. Realize that some manufacturers might reject this, but you should be able to find one that will do something like this.

Another "much less coolness factor" option would be to use two through holes around the LED as shown below (or one directly below the LED if it is large enough): enter image description here

Other options include: - Not using a cutaway and removing all copper in the PCB - Using a light pipe with a complete cutaway

\$\endgroup\$
  • \$\begingroup\$ Wrong. You can create a real stack of arbitrary additional layers. It just can't be converted to something really useful during a CAM-job. Best thing is to have a DXF created resembling the contour. As this is not a standard format for such millings, it still has to be communicated to the manafacturer thoroughly. \$\endgroup\$ – Ariser Sep 19 at 17:32
  • 1
    \$\begingroup\$ I've created custom layers before and had manufacturers follow special instructions with flat flex cables which use a similar stackup, but not with PCB's A file is only an instruction on where to cut, if the manufacture can change their processes then something like this would be possible. If I were a manufacturer, I would take the additional file an run it on the panels that contained layers on one half of the prepeg. \$\endgroup\$ – Voltage Spike Sep 19 at 17:39
  • \$\begingroup\$ We are both thinking basically the same. If something other than vias, holes copper and outline is needed, one has to negotiate with the manufacturer. Of course, one could program a special CAM job to generate a file able to be loaded directly in a CNC mill from a designated layer. But in most cases this is rather complicated in comparison to sending an extra DXF and some text. \$\endgroup\$ – Ariser Sep 19 at 19:17
  • \$\begingroup\$ A DXF also works, I prefer to use a gerber file and check it with layers in a viewer to make sure the board house can't screw it up, they'll always find a way though. \$\endgroup\$ – Voltage Spike Sep 19 at 19:35

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.