Has anyone done any CNC with a tiny cutter? I want to use a .5mm bit. Basically I’m looking for a starting point with cutting speeds/depths for 1.5mm basswood plywood. I know I will have to experiment, but I figure if there is anyone with experience, perhaps I can avoid breaking too many bits.
1 Like
It’s tough because they break really easily.
.8 seems to be the smallest that I can really use without worrying too much about.
But it is possible and here’s what I’ve found:
(I assume you’re using Fusion. I wouldn’t even start to try using Luban. Not enough control and settings choices.)
Buy cheap ones and buy a lot of them
They will break even if you do everything right. You’ll hit a harder spot in the wood or the bit might have a weak spot.
Don’t use adaptive clearing. The paths it chooses seem to be more likely to snap a bit. (Works fine over 1mm)
Pocket clearing works well. Parallel as long as you’ve cleared almost everything so that the .5mm has as little material to move as possible.
Pencil as a final pass will clean up the last little details.
Set step-down to .5mm or less. Start with .3mm and see how it does.
Work speed try 240 to start. Keep all the other feed rates under that. 200 or so.
For step-over keep it to half or less of the bit diameter.
I’ve heard that ball end are less likely to break. Less likely to catch and the force of the cut is spread out. No personal experience but makes sense.
Think that’s about all the pointers I can give. Hope this helps.
-S
1 Like
Much appreciated… Fortunately, it’s just cutting out shapes, so that should be easier than clearing. I’ve been trying to do it with the laser, but it’s taking hours for just a single layer and after 6 passes, still not a consistent cut, and the material is only 1.5mm thick. (I’ve played with focus, step-down, speed, pass count, etc. It’s just never going to be able to handle it, like a CO2 machine would.)
If you’re just cutting out then you might be able to get away with Luban.
But I still would suggest Fusion and then you can use a contour tool path.
-S
1 Like
I will be using Fusion. I’m hoping the tiny bit will give me a decently sharp inside corner for some of the bits.
I’ve used 0.5 mm bits quite a bit on my cribbage board and Christmas ornament projects. My experience was 0.2 on the depth per step. Generally when I started doing this, I reduced the cutting speed to 50% of the whatever the suggested speed was and then gradually increased it until I saw dragging issues (or the bit broke). As was mentioned above, expect to break a bunch of bits because the 0.5 bits are as fragile as glass straws.
1 Like
Apart from all the valuable advice you already got, my personal experience is mostly from small experiments with cutting pcbs:
I practiced first on a piece of styrofoam. You’re not very likely to break a bit on that material and you can get a feeling on how it behaves, speeds & accelerations. Helped me a lot to “safely experiment”
Also considering using multiple bits If you can do parts of it with a larger bit, do so and then do the final clearing with the tiny bit.
Also make sure your material is well secured. Let’s say you’re cutting out a square, depending on the amount of tabs you leave, the part you’re cutting out completely could start vibrating/get loose anyway. This might squeeze the bit a little etc. and that might be enough to break the bit.
And finally, expect it to take a long time 
2 Likes
Very cool! Only other suggestion I’d have is to only use it for a final clearing pass after doing the bulk of the work with a larger bit. Use the Rest Machining option in Fusion and export as two passes perhaps?
It was simply cutting. No clearing. It’s four 1/8th inch layers.
Calling it “just” in “just cutting out” risks minimizing the problems. You’ll have two kinds of problems, both involving non-ideal behavior of the cutting tool.
The larger one is vibration in the tool itself. This is primarily due to “run out”, where the tool does not have a perfect axis of rotation and/or the axis of rotation is displacement from the axis of the tool. It is secondarily due to sideways deflection of the bit because of cutting load, which combines with run out to make vibrations larger. Static run out can be measured by turning the shaft through a full rotation and recording the maximum and minimum excursion, but that’s needs machinist’s tools. Some run out is in the motor itself (bearings) and some is in the collet. The easiest way to remediate run out in the SM is to buy a high-quality collet. Larger interventions probably mean you need a new machine.
The smaller problem is vibrations in the work piece. Are you cutting shapes out of larger stock, so that the waste is outside the part? Or are you cutting a shaped hole into larger stock, so that the waste is inside the part? You’ll need to make sure you can fix your work to the table so that it doesn’t move, and you’ll want to make sure the table itself doesn’t move. Away from Y-center, the table moves easily under cutting force, and there’s only so much you can do before needing to rebuild the Y-axis system.
Cutting a groove is pretty much a worst case scenario for a tiny tool. Even following an already-cut groove could break tools because of vibrations. The basic remediation is to use a larger tool for everything but the final cutting pass. A roughing cut on the waste side with a stronger tool at an offset of 1/3 the diameter of the final tool should be adequate. If you have parts of the shape that such a tool can’t get to, you’ll have to go very slowly, but you’ll want to retain the roughing pass principle. To do this, offset 1/3 the diameter of the tool and cut a shallow groove. Then interleave a finishing pass at the same depth.
Don’t expect software to do all this automatically. Do expect to do some G-code wrangling to get all this working.
I appreciate your advice, but I don’t think my wording minimizes anything. It was intended to impress upon the reader that I was not using a half millimeter bit to clear out a pocket. Simply tracing a contour to cut out shapes. Everything was a final cutting pass. Each layer is only 1/8th inch deep and I was very conservative with my speeds and depths.
The main issue, I think, is that some of the cutouts were very small and could not accommodate tabs. Even though I used a repositionable adhesive to tack down the board, some of the smaller bits just didn’t stick and occasionally the bit got snagged. If I was watching the cut, I could clear any that moved around, but I couldn’t sit there and watch the entire time. I never actually saw a bit break, it only ever happened when I wasn’t there to tend to the cut.
As for vibration… Perhaps. There was no appearance of an issue with the tool. Spinning above the surface, I did not notice any wobble, and the cuts were very clean .5mm grooves.
I hadn’t thought about cutting from the waste side… I can see how that would help, if there is room to accommodate a wider bit. Some of the detail cuts just don’t have the space for that, in this case.
It does minimize the issue. It’s instantaneous stress on which breaks tools, not how much total work it has to do. The stress on a tool is larger when cutting a groove and smaller when cutting along the side, assuming depth and feed rate are the same. When cutting a groove, 180° of the tool surface is in contact with the work. When cutting on one side at half the diameter of the tool, only 90° is in contact. Side deflection increases as contact surface increases, and side deflection is the main stress that breaks tools.
You can’t see run out by eye unless the problem is particularly bad. You have to measure it with a gauge. A spinning tool generally appears as a cylinder, but you can’t measure its diameter by eyeball.
If you’re getting 0.5 mm grooves, that can be anywhere from 0.50 to 0.55 mm in actuality, and you won’t be able to measure the difference with inexpensive calipers. You might get a reading (enough resolution), but underlying accuracy may not be good enough to trust it.