How To Make A Custom Hole

[ThePieMonster]

In the below picture I need to cut out the rectangles on either side of the board. Is there a hole tool that allows you to trace the rectangle or something similar? I don't need any electrical connections here just a place for the grips on the part to go threw. 

Side Question

The part that this is for has pins that go threw the board so is using "Pads" or "SMDs" the right choice for that?

[huayuliang]

Hi, what's your means that "trace"? I feel annoyed for "rectangle" in EAGLE.

I always use CAD software to do comlex board outline or package. such as free nanoCAD.

you could use polygon draw on copper or other layer which you needed. but if you want do electrical connection, you must place a smd pad on copper layer, do not forget uncheck the stop mask if you need.

[rachaelATWH4]

---

@ThePieMonster wrote:

In the below picture I need to cut out the rectangles on either side of the board. Is there a hole tool that allows you to trace the rectangle or something similar? I don't need any electrical connections here just a place for the grips on the part to go threw. 

Side Question

The part that this is for has pins that go threw the board so is using "Pads" or "SMDs" the right choice for that?

---

I think you need to add these cut-out slots to the milling layer. Then you'll probably want to add some notes somewhere to describe what they are for and also speak to your PCB manufacturer to let them know what this is to make sure they see it. I don't know what PCB manufacturer you are using but Eurocurcuits have an online board visualizer and if your cut-outs / slots haven't been correctly detected automatically you can correct it there and see that it's going to be correct.

Best Regards,

Rachael

[ThePieMonster]

Hello,

I was planning on using Seed Studio to manufacture the PCB.

Also about the smd's vs pad's. Since I need a hole threw the board I should use a pad (green) correct? I lined the pad and smd next to each other but it seems there's only a round hole in the center and I need a rectangle. How would I go about this?

[jorge_garcia]

Hi @ThePieMonster,

What you are trying to make is called a slot drill. EAGLE doesn't have a nice way to handle those yet, but we do have a workaround. It will require that you have good communication with your manufacturer.

In order to make slots follow this procedure:

1. For the moment ignore the drill hole worry only about getting the overall pad shape close to the size you need.

2. Once the pad is approximately the correct size you can draw in the opening using the WIRE command on a non-copper layer such as milling Layer 46.

3. When you go to generate the gerbers you will generate a separate gerber file containing only layer 46. You will tell your board house that the info on that gerber needs to be milled from the board.

4. If you're board has internal copper layers then you need to isolate the slot from them manually. You can use cutout polygons for this purpose. If you run the autorouter you will have to make sure that none of your traces run through the slot.

Please accept as solution if my post fully resolves or you issue, or reply with additional details if the problem persists.

Let me know if there's anything else I can do for you.

Best Regards,

[ThePieMonster]

Hey jorge.garcia,

Just wanted to confirm that this is what you were referring too. The turquoise lines behind the green pad are mill layer 46.

[rachaelATWH4]

I'm not sure the overall dimensions of this part or the pins but do you actually need to do the slot drill for your pins? I'm not sure you do. I'd personally consider just using a regular pad with the drill size set to 10-20% larger than the diagonal distance of your square/rectangular pins and see how it goes.

Then all you need on your milling layer is the rectangles for the grips to go through to hold it down. In general if you can get away without additional milling then it'll save on board cost so also consider if the grips could just be done with suitable sized regular holes.

Best Regards,

Rachael

[hudriwudri]

Hi pie monster,

in addition to what Jorge and Rachael already said:

I can confirm that Seed Fusion do milling as specified in the .GML gerber file produced from the milling layer. For example, look at their part library (OPL) micro USB connectors. The line width of the milling outline should be 0. It is best to also include a text on the milling layer outside the board dimensions, stating whether you want the slot to be plated or not, and what tool diameter to use.

Second, the slots are milled with a round tool, so you will never get a true rectangle. The corners will always be rounded off by the tool radius. I know Seed can use .5mm diameter tools, but tools with bigger diameter are much easier (read: faster, less risk of tool breaking, less scrap).

If you really need rectangular cutouts, you can do "dogbones":

[rachaelATWH4]

---

@rachaelATWH4 wrote:

I'm not sure the overall dimensions of this part or the pins but do you actually need to do the slot drill for your pins? I'm not sure you do. I'd personally consider just using a regular pad with the drill size set to 10-20% larger than the diagonal distance of your square/rectangular pins and see how it goes.

Then all you need on your milling layer is the rectangles for the grips to go through to hold it down. In general if you can get away without additional milling then it'll save on board cost so also consider if the grips could just be done with suitable sized regular holes.

Best Regards,

Rachael

---

As a quick follow up, here is a useful guide to sizing plated through holes for various pin styles: http://www.pcb-3d.com/knowledge-base/pth-dimensions

Best Regards,

Rachael

[jorge_garcia]

Hello @ThePieMonster,

That is the idea, you can use a larger copper pad to make sure you have enough copper outside of the cutout, the S pad above looks a little tight.

Please remember to click Accept as Solution on the posts that you consider to be the solution and to give Kudos to posts that help. In this way other users can find answers to similar questions and forum members are rewarded for their participation.

Let me know if there's anything else I can do for you.

Best Regards,

[uniZ7L2P]

any updates on this issue? my manufacturer rejects designs like described in this thread cause they need to come up with me to clarify if i intended to make slots or holes. this feedback costs additional e-mails and results in more overhead when producing PCBs. so... if there was either holes or slots in the design it would be much better for production. is there nowadays (using eagle 9.1) a better way to achieve custom holes?

[jorge_garcia]

Hi @uniZ7L2P,

I hope you're doing well. Currently nothing has changed in this regard for V9.1.0 of EAGLE. We understand that this creates an additional overhead when manufacturing the boards and we will be addressing. I don't have an ETA for this but it is definitely something we want to take care of.

Thanks for visiting the forums and bumping this suggestion.

Let me know if there's anything else I can do for you.

Best Regards,

[Anonymous]

That's great to hear Jorge. The 9.1 update had great features that couldn't come any sooner. I hope features like the one brought up in this thread and others are implemented in future updates.

Is there a list that is public to users that contains up and coming features that are being developed for future updates of the software? 

[Anonymous]

This failure to provide a way to cut slots is pretty upsetting.    Things are hard enough than to need to deal with special instructions to people who don't speak my language (China does my boards).    I'm currently using OrCad and the export of a routing file is something a FAB house understands without explanation.    How can you sell this product as a professional offering without this basic feature?

How would you explain to a FAB house the special instructions on which slots are plated and which are unplated?   You really need to publish a video dealing with this topic directly.

[rachaelATWH4]

---

@Anonymous wrote:

This failure to provide a way to cut slots is pretty upsetting.    Things are hard enough than to need to deal with special instructions to people who don't speak my language (China does my boards). I'm currently using OrCad and the export of a routing file is something a FAB house understands without explanation. How can you sell this product as a professional offering without this basic feature?

---

Honestly it would be nice if it handled it more directly but I've never found myself being upset by the lack of this feature. The extra time needed to sort this hasn't really ever been that much of an issue as it doesn't take long to sort, but I agree if you need to explain to a fab who doesn't speak your language it could be a lot more difficult. To be fair to EAGLE, I have used a number of other (very expensive) packages and often they have required notes on a build drawing to detail what is required too much like EAGLE does. If OrCAD is not requiring that then that's good.

When you generate your outputs from OrCAD, what does it produce for these slots? How is this information conveyed in the generated Gerber files? Could you give some examples of the OrCAD outputs to show this?

---

@Anonymous wrote:

How would you explain to a FAB house the special instructions on which slots are plated and which are unplated?   You really need to publish a video dealing with this topic directly.

---

I normally have a drawing layer for build notes and on this I annotate the places which are slots with unique markers depending on the type of slot (plated/unplated) and then write a simple one liner for each to say which markers are which. I then create the Gerber output by combining this notes layer with the dimension and milling layers.

Best Regards,

Rachael

[one-of-the-robs]

Further to @rachaelATWH4's comments, the reason for needing to deal with special instructions to your fab has very little to do with Eagle's capabilities and lots to do with some of these features being sufficiently "less common" that there is no global standard for what you need to send. If such a universally accepted format existed, somebody here would have posted the instructions for persuading Eagle to produce it.

That doesn't change the fact that we'd all like Eagle to handle slotted holes more cleanly but there's very little AutoDesk can do about fab houses having inconsistent requirements.

[Anonymous]

I simply generate a routing file -- and there is nothing else I need to
explain.

Routing is a pretty serious portion of all non-rectangular boards -- or
boards with unusual parts like USB receptacles, for example.

I hadn't made it to the exporting of the artwork yet -- I just can't get a
USB receptacle modeled correctly in a footprint... and that a sticking
point early on in the process.

[rachaelATWH4]

---

@Anonymous wrote:

I simply generate a routing file -- and there is nothing else I need to
explain.

---

Ok so what is the format of the routing file? How is plated vs non-plated defined? As @one-of-the-robs says, there isn't a standard used across all board manufacturers for this so it's not clear what OrCAD would be doing in their outputs to specify this. Could you create a simple board with sample outputs so we can see what is being done?

---

@Anonymous wrote:

Routing is a pretty serious portion of all non-rectangular boards -- or
boards with unusual parts like USB receptacles, for example.

I hadn't made it to the exporting of the artwork yet -- I just can't get a
USB receptacle modeled correctly in a footprint... and that a sticking
point early on in the process.

---

You need to use the known work arounds previously given for creating the slotted holes and the technique I described in my post above to make annotations on the drawings to describe what is required for the manufacturer so there is no ambiguity. It's not ideal, it should be easier, but it's not a show stopper issue, not for me at least, I've done parts which require this and it's a little fiddly but workable. 

Best Regards,

Rachael

[Anonymous]

Are you asking for a set of Gerber files to see how the plated output is
defined?

[rachaelATWH4]

---

@Anonymous wrote:

Are you asking for a set of Gerber files to see how the plated output is defined?

---

Yes pretty much. I was thinking if you had a small example board with just a couple of components which use slotted holes, examples of both plated and non-plated and then generate all the outputs you'd send to the manufacturer so we can see how OrCAD is generating it's outputs, to see if there was any other file or annotation which were being automatically generated to define these properly. I do agree, creating these in EAGLE is a bit of a pain sometimes, hopefully there'll be some effort put into fixing things like this at some point.

Best Regards,

Rachael