Estlcam - holes missing in 3D milling ...

Hi all,

I have an issue with a model in Estlcam which I hope one of you may help clarify … I would appreciate this :wink:

I am new to CNC milling, however, as I am very interested in learning to use a CNC I recently bought a CNC (WorkBee) with the software EstlCam to control everything. Having spent the better part of a week assembling the WorkBee - and gaining some initial familiarity with Estlcam - I yesterday did my first “real” CNC milling.

It worked out reasonably well yet for some reason the holes in the model I was milling wasn’t milled (the attachment shows a small part of the model and settings for generating the CNC program) …

I later realized that the end mill I used was larger than the hole so there would be a - possible - explanation for this …

However, today I have simulated the model again in Estlcam (generating a CNC program) with a 1.5mm end mill instead but it still doesn’t look as if the holes are included (the two last screendumps in the attachment) …

So I wonder if I am doing something wrong here … And if so, then what … ??

I would much appreciate if someone here may help clarify this :wink:

Cheers & thanks,


estlcam.pdf (1.88 MB)

It probably won’t ever cut those holes like that. You’re 3d milling an stl, which is more for decorative stuff. To actually have it drill down, you need to start from a cad(DXF) drawing of the part you’re milling. Here is what I’m talking about.


If the part is really round and fancy and needs to be 3D milled (looks like a rounded handle half), you can then do a second operation with a DXF to mill/pocket/drill the holes. Small straight holes do get missed for some reason, in tutorial Barry linked It missed the screw hole in that as well.

Hi both - & thank you very much for your feedback!

I will look into the tutorial Barry has linked to and - I reckon - likely learn something very useful.

Cheers to you,


Hi again,

I have now read Barry’s link and I see how it can be done with the model I would like to make. However, it does have a needed 3D curvature that must be reproduced quite accurately so some kind of 3D CNC programming and milling likely is required …

Another option may be to use a rounded end mill but I reckon there could be an issue with the force acting on the rather thin “spines” (the beginning of a spine is shown in the middle of the cut-out) in the model. I guess this has to be tried out in practice.

A couple of brief questions, though:

  1. Can I be sure that if I import a DXF file into EstlCam then the zero point alignment will be identical with e.g. an STL file of the same model also imported into Estlcam? It would be very useful.
  2. You’re 3d milling an stl, which is more for decorative stuff.
Ok, good to know. Is there a more suitable file format for 3D milling? I have access to the file formats shown in the attachment.
Have a good evening ...
Jesper [attachment file=67676]


Ooups - looks like something didn’t work out as intended with the quotes … hope it is readable anyway.


Here’s a question. Does the part you already milled out have any indentations where the holes are supposed to be? If so, you can just use a drill press or hand drill to finish the part. Otherwise you’ll need to use something like fusion 360. Estlcam doesn’t currently have the capability to mix 3d and 2.5d milling.

If you use the free machining option there are actually a few options. You can extract a 2D outline to use later, import an outline, or just move the zero. It can be really powerful and save a ton of time. Most want to, for example, 2D mill/pocket out a small box lid and just 3D mill a rose or something small, this can save hours and make for a much better end product.

Barry’s suggestion is the fastest option. A lot of harder materials can just be marked and drilled.

1 Like

Hi Ryan & Barry,

& thanks again for your feedback and suggestions.

@Barry: This part needs be very precise (< 0.1 mm tolerance for the holes) so hand drilling the holes is not really an option - at least not with the precision I can work with.

@Ryan: Thanks for the tip with the outline. I tried it out this morning and at least with the 3 point circular zero point selection feature the zero point can be set identically for the 2.5D outline and the 3D free machining mode. I think this solves the “challenge” - thank you for helping out here :wink:



Hi again,

I will be going a bit off-topic relative to what this thread is about but hoping that you may know about this as well …

As it is I would like to CNC mill some PCBs (electronics) and I need it to be very high quality - essentially production quality. To this end I have bought some 10 degr. 0.1 mm V-shape engraving cutters, however, I have a couple of challenges:

  1. Translating Gerber files to a format that Estlcam will import and use. I don't use Eagle to layout my PCBs (Diptrace instead) so I need a way to convert the Gerber files to an estlcam compatible file.
  2. Calculating the depth per pass and particularly the feed rate for this V-shape cutter (spindle speed can be 8000 - 24000 rpm). The cutter deliberately is small as I will be making PCBs that may include SMD components with a pin pitch of 0.5 mms and pin width 0.2 mms.
Might I be lucky that you also have some ideas for this?

Thanks again … Jesper


Hi … it seems that I may be able to use Flatcam to convert diptrace gerbers to g-code. So likely no reason to reply to my questions as of now …

Have a good day :wink:


1 Like

Nice find. I did some manual editing the last time I tried it, FlatCam seems to be what I should have used.

Jesper, what are you making?

Hi both …

I have just started a new “single post” thread to link to the videos that describe how Flatcam can be used to convert Gerbers to Gcode that can be used e.g. in Estlcam. This way others may also be able to use this process which actually appears to be quite straightforward:

@Jeffeb3: Hi … I am making various things but mostly audio related like DACs, ADCs, headphones, and the like.




Oups … It looks as if my reply to Jeffeb3 cannot be read so here it is again:

@jeffeb3: Hi … I am making various things but mostly audio related like DACs, ADCs, headphones, and the like.




when working with STL files the tool needs to be significantly smaller than the smallest hole or feature you want to machine.

The X and Y machining strategies create toolpaths with fixed spacing:

  • Lets say we have a 10mm tool and 50% stepover
  • This will create toolpaths with 5mm spacing
  • If you now have a 10mm hole it will only be machined if it is "accidentially" located right along one of those toolpaths
  • If it is just slightly off it will not be machined as machining it would cause it to be at a wrong location
  • The hole needs to be at least 15mm (10mm tool diameter + 5mm stepover) to always be within reach of a toolpath. If it is less it will be machined sometimes, sometimes not.
  • In fact it even needs to be a little larger than 15mm to take STL facetting and computing precision into account.
The waterline machining option is less critical but still requires the tool to be somewhat smaller than the hole in order to work properly.



Interesting, thank you for the clarification.

Huh. Thanks.

In the example of a 15mm hole, it will still only drill a 10mm by <15mm hole, because there will only be one toolpath would cross it. Is that right?

@Christian Knuell: Thanks for clarifying. I will try again with a somewhat smaller bit.