I can get these imported into fusion easily enough, and have started playing around with the software settings to get a simulation I like, but there seems to be quite a few operations that aren’t possible with mesh files. I know you can convert mesh to brep, but any of those are going to have to be heavily simplified (the one I tried was around 67k facets), and I wanted to see if there was a way to get something that looked decent.
I have a feeling just looking at the models that they’re sort of impossible, since there are overhangs, but perhaps the right bit could get those. Besides that, I seemed to be able to get close with a 3d adaptive clear and then a Parallel pass, but that still didn’t get the depth on the letters on the banner at the bottom. Anyway, just trying to get a sense of what different operations do, so interested in how others might approach the problem.
Unfortunately Fusion really doesn’t do well if you want to try and convert a mesh. Anything organic simply has too many facets for it to convert.
If you’re trying to modify the mesh or combine with an object it’s a problem. You’re better off using another program like meshmixer or meshlab to edit it.
However, for milling that really doesn’t matter.
I think most of those models are doable. They will be different slightly and probably look okay. Whether it bothers you is up to you. What happens with the overhang is it just ends up looking like it emerges from the background and from straight on doesn’t look any different.
I think the biggest problem you’re going to have is the detail and that’s dependent upon what size bit you’re using. On inside corners you’re limited to the diameter of the bit and it will be rounded accordingly. So on the names at the bottom is where you’re going to have the most problems because you won’t get the sharp edges. And depending on the overall size of the piece you’re carving you may or may not be able to engrave them at all.
I’ve used bits as small as .8mm. Can’t push them too hard but even in oak or maple I’ve been able to use them without breaking them (well, except when I’ve done something stupid).
As far as paths go, try pencil and/or morphed spiral at the end. Pencil does a nice job of going in and doing some of the deep little details that sometimes get missed.
Make sure you’re using rest machining on your passes so they’re only doing what hasn’t been done before.
-S
I ended up starting this with a 3d adaptive clear pass, a parallel pass, and a pencil pass. Results looked pretty good in the fusion sim, so trying them on a piece of MDF now. Using a 1.5mm flat end for everything to see how it works out. The only difference seems to be the time to machine. I was just going to let it run overnight, but I got a little nervous around midnight when I went and checked on it and saw how much MDF dust it was having to wade through on each pass. Probably OK, but I also didn’t want the bit or head to jam, and I wasn’t sure if there was a chance of it catching fire in the middle of the night. Paused the job and restarted this morning after clearing off the removed material, and will keep an eye on it through the day.
I did figure out that Fusion can do some basic mesh scaling at least if you enable it in the preview, which is what I was looking for.
I picked up some replacement bits that go as small as 0.6mm. Depending on how the first attempt turns out, I can try another pass with one of the really small bits to try and clean things up.
The dust in itself should not burst into flames spontaneously under normal circumstances. However, fire is a real thing when you’re using a cnc on wood. Winston Moy has a video on the subject that’s definitely worth watching: I Almost Set My CNC on Fire - Let's Talk Shop Safety - YouTube
Personally I’m also using some dust collection to keep the work-area clean while milling and I’m really happy with this. It has been discussed in other topics as well: CNC vacuum (too much wood dust) - #8 by brvdboss
I have it connected to an old home vacuum in the lowest setting and with a cyclone dust collector in between and I must say I’m very pleased with the result.
Yeah, I saw some of the dust collection solutions, and might work out a system for that if I can figure out something other than the shop vac to use for it (which is probably overkill to keep running all the time). Thanks for sharing that video though-definitely food for thought. I don’t think I’m going to stay in the room for a 20h CNC job, but it definitely has me thinking about monitoring setups. I like the idea of the smart plug combined with the wifi smoke alarm, but that seems like a lot of dependencies on the networking as well.
Neither do I :-), but I do tend to check up on it regularly (every 2 hours or so) and never let it running while not at home. The dust itself will rarely be a problem. It’s more when your workpiece gets loose and you end up grinding the workpiece vs milling it. Basically it’s the same as rubbing two sticks to each other like they do in cartoons to create fire (Or when you’re hitting metal parts & create sparks)
As the cuts got deeper, I was wondering about the pile of dust clogging the rotation or getting into the air intake and causing the motor to sieze up. Probably not likely, but MDF seems to generate a large dust volume (the pile off to the side is what I’d scraped away late last night). I’ll probably keep checking in every couple hours, pausing the job, and taking a pass with the shop vac (so far, all the resumes have been OK).
I’ve had a couple pieces come loose and have done some damage to some bits and clamps. Never had thought about that being a fire danger though. But ever since I’m definitely on the overkill side of clamping stuff down and also having some fixtures pushing against the sides too.
I haven’t set up a vac system yet. I just vacuum every so often depending on the amount of sawdust I’m creating (don’t usually even bother with pausing) I just don’t want a vac constantly running. I may set it up with a smart switch to run every so often. I’d think the bigger danger than the dust on the workspace would be the airborne dust. Do a web search for ‘flour dust explosion’.
I use an old iPhone to monitor mine. I do need to add a smart switch to it to shut it down remotely. The fire extinguisher balls are a good idea too.
Give a ball end a try for your final pass. For things like this the finish will be much better. Just leave .5mm or so for it. Whether you use pocket or parallel or another type depends on how you want tool marks to be and how much you want to sand if you want to remove them.
-S
So here’s what I ended up with on a hunk of MDF using the 1.5mm bit:
Tried adding a finishing pass with a 0.6mm bit this morning, and managed to break it, so I probably had the stepover set too high.
For rest machining, do you typically change the adjustment setting? It defaults to “ignore cusps”, but it seems like it calculates more cuts if you set it to “use as computed”.
There seem to be quite few varieties of mdf and different materials used to make it. Yours looks like some of the more coarse stuff I’ve seen that reminds me more of cardboard where some is more like fine sawdust. That’s where you’re getting more of the rough fibers. It’s great to play around with and test, but you’re going to get much better results with a good fine grained hardwood like maple or walnut.
The ignore or machine cusps was the hardest thing to find out info about and get my head around in Fusion. I may still not completely understand what it does and how it calculates, but I’ve at least figured out how to apply it to my real world usage. (If someone can explain it clearly, please do). In practice machining cusps well help reduce the stair-stepping you get from stepovers and on curves and angles on the horizontal plane. So until your final pass or passes (if you’re doing sections at different times) you can ignore it. Leave it at “ignore” and the default adjustment offset of .5mm seems to be fine. On your final pass change it to either ‘use as computed’ or “machine cusps” (I think I’ve been using latter) and set the adjustment offset to 0. Then it will do as much smoothing as is possible with the path chosen and selected bit.
There are a lot of different ways you can break a bit. Especially such tiny ones. Usually stepover isn’t the problem. That just tells how close the center of the next parallel path will be. It’s not how much the bit physically moves over. Generally you want stepover to be somewhere between 1/3 to 1/2 the size of the bit for finishing. For clearing it can be just less than the diameter of the bit, but some of that depends on the wood and size of the bit. More likely is that work speed (or ramp, plunge etc) were too fast or your step down was too great. There are also some paths that won’t account for the size of bit or what’s been cleared (or assume you’re running them after a certain type of pass) and will make sudden moves that pushes the bit through the stock. Make sure you run ‘simulate’ to see what your paths are going to do and pay attention to error messages and know when and why you can sometimes ignore them.
-S
(Or when you’re hitting metal parts & create sparks)
