Plated and Non-Plated Slots and Cutouts

About this tutorial

This tutorial shows you the capabilities and what you need to do to achieve elongated holes, plated and non-plated slots and cutouts.


  • For Plated Slots a maximum length of 15.0mm (5/8 Inch) and diameter of 0.7mm (0.027 in) to 2.8mm (0.11 in)
  • For Inner Millings (i.e. cutouts), use at least 1.6 mm (0,063 in) diameter and always confirm with our Board Viewer
  • Non-Plated Slots must be realized as inner millings (min. diameter of 1.6 mm (0,063 in))

Plated Slots

We support plated slots with a length of up to 15.0mm (5/8 Inch) and a width of 0.7mm (0.027 in) to 2.8mm (0.11 in).

              (Typical use case of plated slots)

Typical use case of plated slots.

As we give a gurantee on our renderings you should always use the Board Viewer to check if plated slots are detected properly. Use the “Highlight Drills” Button for this.

Screen Shot 2019-07-26 at 11.48.53

        (Highlight drills function)

Enable drill highlight

Screen Shot 2019-07-26 at 11.50.48

                       (Plated Slots in the Drawing)

This plated slot will be manufactured properly, shown by the orange color.

Eagle Users should always check if a slot was detected as plated or non-plated slot.

Cutouts and Non-Plated Slots

Cutouts and Non-Plated Slots will always be milled and may have any shape you like. Please note that our smallest milling tool diameter is 1.6 mm (0,063 in) and ensure, that all Cutouts or Non-Plated Slots have at least this size.

Screen Shot 2019-07-26 at 12.19.11

      (Cutout with milling path highlighted)

Cutout with milling path highlighted.
Screenshot from 2021-03-30 11-05-42

      (Non-Plated Slots with milling path highlighted)

My PCB has plated slots for USB connectors, 0,7mm wide. The slots are not shown by the board inspector. Which layer should I use in Eagle so that Aisler detect these slots? Now I use milling layer 46, but that doesn’t work. I have tried the drill layer 44 and dimension layer 20.

1 Like

There are some ways to do those slots in EAGLE. :sweat_smile:

In the picture I have done it with the Milling layer. Note, that you have to do a closed line and not one line, see the following picture:


For the Pad itsef, you combine many parts, as seen the following pictures:


One note: In this picture the polygon on BStop is missing, it is the same for the bottom layer as on TStop (top layer).

The ‘SMD’ will define the outer size, the golden area you see here:

The inner part is defined by the Milling Layer.

Have you uploaded the EAGLE file or Gerbers? This makes the following difference: If you upload the EAGLE .brd file everything is done automatically. For the Gerbers, you have to select the Milling at export.

I hope this helps :smiley:


I stumbled into the difference between plated and non-plated slots, and I wonder why it’s not possible to have non-plated slot with less than 1.6mm width?

It’s clear that the smallest milling tool has a diameter of 1.6mm, but somehow you must be able to mill a slot with roughly 0.7mm width if it’s plated. In fact, the plating will add some thickness after the milling, i.e. the milled slot must be bigger than 0.7mm. But I cannot imagine that the gold layer is 450 microns thick (would be a 1.6mm slot + 2x0.45mm gold plating).

So, how can you make slots smaller than 1.6mm and why only when they’re plated?

1 Like

I am not able to design my milling-coutouts the way, that the board-designer gets it.

I tried it in different ways, here with a milling path (as It believe a closed path)

But if I ignore this warning, no milling is done.
Before 2 years I ordered a PCB with milling-pathes that has only been lines and it worked.
I could realy need some help,
Thanks :slight_smile:

I solved it, I had to enlarge the area so the minimum milling diameter can mill it.
Thanks :slight_smile:

1 Like

Hi @js_qat,

Welcome to the community!

Indeed, technically it’s not a problem to manufacture non-plated slots smaller than 1.6 mm. The same tools (special nibbling drills) are used for both plated and non-plated slots / elongated holes.

The reason why we do not support non-plated slots < 1.6 mm: The manufacturing of an elongated hole with a nibbling drill is an extremely time-consuming process. In contrast to a conventional milling segment, the nibbling drill must plunge into the material hundreds of times. Using a 1.6 mm milling tool would be much more efficient.

In the past, we often experienced that non-plated slots were used to realize large “conventional” milling sections (e.g. to realize user defined subpanels). In most cases, these sections could just as well have been milled with a 1.6- or 2.4-mm milling tool achieving the same functionality.

In our experience, non-plated slots in components tend to be the exception, which is why we have decided that this restriction is permissible.

However, we will consider allowing non-plated slots (maybe length and amount depending on the board size) to a limited extent. In this case we will inform about it here.

Best regards,

1 Like

Missing: the minimum width of non-round holes and similar cutouts. In this detail from one of my boards the cutout is supposed to be the same width as the hole to its left.
Also there’s this extra ring of no-copper space around one end of the cut (presumably the location where the milling tool enters the board?) which is somewhat annoying because if we really do need that empty space I’d like a way to control which end of the cutout has it.

Screenshot from 2022-04-25 10-50-08

Here’s (mostly) the same view in kicad:
Screenshot from 2022-04-25 10-52-01

Hi @MatthiasU ,

Welcome to the community!

We have moved your post, as your question is better addressed in this thread.

Our system has made a mistake here. As I have already written above, non-plated slots are normally converted into inner milling paths by our system. In a further step, we select (if possible) a suitable milling tool (1.6 or 2.4 mm) to mill the cut-out. This conversion does not seem to have worked properly in your project. What you see in your upper screenshot (blue color) is not a milling path, but a non-plated slot. As a consequence – but not intended – our system has removed nearby copper (analogue to conventional NPTHs, see here) but only in the area of the starting point.

Would it be possible to draw these elongated holes with a diameter >= 1.6 mm on the EdgeCuts layer?

Best regards,

1 Like

Thank you for the prompt reply. That works better, except that one of the four cuts I placed is now shown as plated for no good reason.

Hello @MatthiasU ,

I have sent you a PN, also with a few more project-specific comments.

I will later include this case (intended milling path is shown as a plated-through slot) in the article.

Short version: If the start or end point of slot is located in copper, it is classified as plated through and will be manufactured with a nibble drill.

Best regards,


I have a question regarding slots files. I’m using Allegro PCB editor, and this tool does not allow me to create slots and drills in a single file - it’s creating sepparate Excellons for circular holes (drills), and for slots (route).

What should I do in such case? From the gerber filename guide I see there is just one file for plated holes, and other for non plated holes. Any option for a router file?


By my shorter millings i get plated slots instead of millings paths. I tried to change the thickness but this does not helps.

Hi @karol-itworky-com ,

welcome to the community!

Sorry for getting back to you so late. We are currently working on the possibility of uploading more than two drill files. As soon as this is possible, I will get back to you!

EDIT: Upload of multiple files of the same layer are possible now! Please also see our Article about Traditional Gerber

Best regards,

Hi @julian ,

welcome to the community!

Our system classified these intended milling segments as plated slots, as they fulfill all criteria (length <= 15 mm & 0.7 mm <= diameter <= 2.8 mm & located in copper)

If you clear the copper in the area of each segment, they should be recognized as conventional milling sections. Note: To avoid the milling tool cutting through copper (risk of unwanted short circuits), there shouldn’t be any tracks or surfaces within 300 µm around the milling path.

Best regards,

Hello Manuel,

Thank you for your fast answer. Did you also know how to change this in eagle. To change a line to the outline of the line.

Thank you


I got this warning message in the board inspector:

The related part of the board are:

Can someone explain me what is the issue ?
The Gerber files are produced by Fritzing. (If this helps)



I’m running into an issue. My design includes two small cutouts that I can make 1.6mm wide (they should be 1.4mm per the specs, but it’s not critical), so should be OK. However, they are on one side of the board and seem understood as part of the ‘outer milling’ - and the online tool complains as they are not 2.4mm wide.

Any chance of making such a design works ? (an earlier revision of the design with 1.4mm cutouts could be made by a well-known competitor, but I’d rather switch to a more local manufacturer).

Thanks in advance & cordially,

Seems Aisler has changed the behaviour. I tried both versions, both are working.
I named the layer for the milling gerber data as board.milling.ger
This naming of the milling layer is not documented by Aisler in the Article about Traditional Gerber

1 Like

Usually, the milling paths are combined with the outline data.

It is also possible, as you described, as a separate milling layer and Gerber file. :slight_smile: