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.
(Highlight drills function)
Enable drill highlight
(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.
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.
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 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?
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.
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.
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?
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?
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.
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).
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