Engineering

Cut Outs, Slots, Routes, and Border Files: Revisited

MacroFab’s PCB Assembly supports plated and non-plated cut outs, slots and routes. Last time we touched this subject was in the article Plated Slots: Stop Fitting Square Pegs in Round Holes where we explained why a PCB designer should use plated slots instead of large drills for connectors. In this article, I will show a couple examples of how to draw plated and non-plated cut outs and slots so we can build your PCB according to spec.

The Border Gerber File

MacroFab looks for cut outs and slots in the .BOR or border gerber file. In the EDA Tool Eagle this is generated from the Dimension layer 20. Other EDA Tools will call this the PCB border. If you are uploading an ODB++ package you will have to make sure the cut outs are drawn on with your border tool. You can check after uploading to MacroFab by reviewing the Border Layer in the PCB viewer. DRC rules for cut outs and slots can be found on our Assembly Specification Page.

MacroWatch Example PCB. Checking if the cutouts exist in the PCB viewer.

 

Make sure the width of the lines is at least 1 mil or larger. The board is milled/cut to the middle of the line, so thickness of the line does not impact the result. Making the thickness of the lines a non zero number will reduce problems down the road with external gerber viewers.

Drawing Cut Outs and Slots

I used Eagle as my example EDA Tool but others should follow suit to get the desired outcome. I drew the cut outs on the dimension layer for Eagle which is Layer 20. The red areas are Copper. The example shows three different kinds of cut outs or routes; external cut out, internal cut out, and internal plated cut out.

Example Board with three different types of cut outs or routes.

Close up of the USB connector which uses plated cut outs. The cut outs are drawn over the copper pads.

 

When uploaded to MacroFab, the cut outs can be seen in the PCB view under the Border Outline layer.

MacroFab PCB viewer example cut outs

Non Plated or Plated Cut Outs?

If you draw your cut outs over copper it will be assumed to be a plated cut out. This is similar to a drill placed in the center of a copper pad for a via. For non plated, pull the copper back at least the recommended distance from copper to board edge DRC. That is all you need to do to denote the difference in your design files.

How the PCB will be milled

When the cut outs are machined out of the FR-4 material (what PCBs are made out of) the PCB fab uses a round bit similar to a CNC machine. Thus inside corners of cut outs will not be sharp but will have a round edge to them. This is something to watch out for in enclosure designs. The smallest inside corner radius possible at MacroFab is 0.5mm. This is because the smallest tool used for routing out boards is 1.0mm in diameter.

Below is what the above design will look like after the PCB is made. The inside corners are rounded and the edge of the PCB is cut to the middle of the border line.

What about external exposed plated cut outs?

Ah! Castellated Edges are an example of external plated cutouts. These are used on breakout boards and similar module style boards. We will be cover these in another article.

Recap

  • Border gerber file should include all routes and cut outs
  • Border lines will be cut to the middle
    • Width does not matter
    • Kerf of the bit will be in the waste area of the route or cut out
  • Inside edges will be rounded due to router bit
  • Route will be plated if through copper planes
  • Jose I Romero

    Why don’t you support G85 oblong PTHs in the drill file, as produced by KiCad (among others)? Most fabs I’ve used (all of the Chinese, and Advanced Circuits stateside), both prototype and medium run productions have dealt with them just fine. It is only for OshPark and Macrofab that I have to go to the extra, error-prone step of duplicating the callout on the mill layer.

    Is it because Chinese fabs can afford to have a human sitting in front of cam350? (and Advanced will happily charge you extra for the privilege of having oblong holes)

    • Parker Dillmann

      Basically Jose. No board house does the G85 drill function anymore in terms of actually using the CNC drill machine to drag the bits across the FR4. We try to minimize the engineering questions we get back from our PCB fab as just one of those slows down the entire process and this is part of that process. Sorry if it is an inconvenience.

      • Jose I Romero

        I know that, virtually all places will also not drill large holes with a drill but use an endmill instead. They also don’t use photoplotters that drag an aperture to draw traces (as they are described in the gerbers) but use raster protoprinters or direct imaging. Yet, most can lift all that information transparently from the files, without having to manually repeat information in separate layers or add manual notes, it just seems to be a CAM issue on the fab’s side. The only time I got a comment back from G85 holes was when I accidentally violated their minimum slot size by a tiny amount, they expanded the slot slightly and the board got fabbed just fine.

        • Parker Dillmann

          Understood. I would like to add an auto G85 -> Gerber conversion to the upload process. Sometime in the future 🙂

  • Tim Kay

    You said that the routing is centered along the border line, but your second-to-last diagram shows the green routing path adjacent to the border line, not centered on it. Am I misunderstanding something?

    • Gabe Ayers

      Tim, I read that as saying that the board is cut to the middle of the border line. If you look at the edge of the green tool path it is at the middle of the border line as stated in the article.

      • Tim Kay

        Interesting. Apparently I misunderstood the article. I read it as saying that the routing is centered with the center of the border line. This way it is unambiguous.

        I think you are saying that the *edge* of the route aligns with the center of the border line. That way is ambiguous: how do you know *which* edge of the route path aligns with the center of the border line, the inside or the outside? You might answer “oh, the inside edge, of course”, but it’s not always apparent which is the inside edge.

        • Jose I Romero

          The outline is meant to represent the edge of the pcb material. Unless your outline is malformed, inside and outside are very easy to tell, as any vector program that does filled polygons can do. The milling path will just be whatever ensures that the outline edge gets milled within tolerance, this is done automatically by the fab, the exact path shouldn’t concern you except for this detail:

          What this blog is telling you to mind about is that the milling tool will have a radius, so internal sharp corners will get rounded, and you need to avoid making cutouts that would “trap” the bit, that is, put two edges too close where the standard bit wont fit. That would either make that slot impossible to make, require a more expensive smaller bit and more milling time, or be silently expanded by the fab. All three result in potential delays and/or unhappiness. If I can get away with it I usually design my boards with a 1 or 2mm radius, and always put all radiuses in the outline layer, that ensures the board will get manufactured exactly as drawn by pretty much any fab without any surprise rounded corners or off dimensions.

          • Tim Kay

            The PCB is cut so the bit is outside the boundary. A cut out is cut so the bit is inside the boundary. Is it always clear which is which? Suppose I have a large project that has a big dead space in the middle. I choose to put another project in that dead space. Does it cut outside or inside the boundary of the inner project?

          • Jose I Romero

            Almost no fabs will let you do that. What you are describing is called panelization. To put a board inside another you need to specify a region delimiting the material to be removed between the boards. And you want to keep all boards connected with tabs so that pieces dont fall out when they process the board. In my experience it is usually more hassle and expense to combine boards like that instead of just leaving it up to the fab to panelize themselves. (Many proto fabs will charge you extra if you self panelize, because it makes the board more complicated to CAM and it reduces the amount of boards they can cram in a proto panel.

          • Tim Kay

            I appreciate the reply, and I understand that the fabs have restrictions on aggressively priced product offerings. However, the scenario is legitimate and could come into play in certain circumstances. So the question still stands, how do you control the routing given the inside/outside ambiguity?

          • Parker Dillmann

            You can write “ROUT” or “ROUTE” in the areas that you want routed out to clear up and ambiguity. I did this recently with a custom panel that had traces connecting all the individual boards together for quicker testing. https://uploads.disquscdn.com/images/b3485ace89cd39ac06f5be5347e6c6f52fa259148b0d53bad12d7aff81a4db24.png

          • Jose I Romero

            You either use thick lines and specify the line is the routing line, or more unambiguous, just outline the _region _ of board to cut out from the pcb adding hatching or the words CUT OUT inside of the area to cut out. For a board within a board you can put 4 L shaped regions around the inner board with the tips almost touching. Then you can separate the boards using diagonal cutters.

          • Tim Kay

            I like the “4 L shaped regions” approach. To be clear, by “region”, do you mean a closed region surrounded by a border line? In that case, the router bit will cut out the inside, and the outside of the cut will align with the center of the border line?

            If so, the region needs to be at least as thick (center-to-center) as the router bit. Will it always require a pass in both directions, or can I make the region just as wide as the router bit, so that it can make the cut in a single pass?

          • Jose I Romero

            Indeed, a closed region. As for the multiple passes, that is 100% up to the fab house. For proto runs they will use whatever tool is more convenient to them for that particular panel. They will guarantee you that both edges will be within their tolerance, and they will probably reject your board if the region is too small to fit their smallest bit into. For large scale production, since your board will be the only one in the panel, you might be able to get better pricing/yield if you optimize your design to their tools. Prematurely trying to optimize without that input is pretty useless as there may be other constraints in the panel that make that irrelevant. The point of the article is not to optimize your design to reduce things like numbers of passes, but ensure that 1) the board is manufacturable 2) it is manufactured as designed, with no surprises coming from the limitations of the pcb routers, or the designer leaving things open to interpretation.

  • hexafraction

    Do you support chamfers on edges (as would be used for board connectors)?