Preventing collisions in Fusion 360

I would do the finishing passes (only) with your previous downcut endmill, downcuts are wonderful to clean-up those top edges. And if you can get your hands on a downcut endmill that has a 30mm LOC, even better, do a single finishing pass at full depth, it should leave you with smooooth walls.

Nope, you should not be generating earthquakes :slight_smile:
My gut feeling (that I mentioned above, somewhere) is that an optimal load of 2.54mm is too high, even in wood. I would dial that down to say 1mm and retry.

Probably the same: reduce optimal load.

Ok, I’ll give that a try. I think I don’t understand optimal load. I thought it was essentially just the step-over, but I gather it might be more than that. But basically I’ll be going from 40% to 15% of cutter diameter, which I think will make the cuts take way longer. If I kept the optimal load higher - say 2mm or 1.75mm - but went shallower, would it have the same effect?

You’re absolutely right, optimal load is basically the stepover (well…technically not quite, because adaptive toolpaths aim at maintaining a constant tool engagement, so they will dynamically reduce stepover in corners for example). Adaptive clearing toolpaths tend to be associated to HSM (High Speed Machining), which favors large depth of cut with a small stepover, over the traditional approach (on hobby machines) of a shallow depth of cut and large stepover. You could do a bit of both, reduce DOC but maintain optimal load. My way to view it is that what matters in the end is the amount of tool engagement, in 3D. It’s possible to have the same tool engagement using large DOC, small WOC, or using medium DOC, medium WOC, or using small DOC, large WOC.

You will have to experiment a bit to figure out which approach is best for you.

Since you are cutting wood, it’s worth considering a more traditional set of toolpaths (2D pockets & contours) that would cut at small DOC (say 50% of the endmill diameter) but at a large stepover (40 to 50%). They may be faster too. I did not comment on that initially since your project had adaptive clearing toolpaths so I assumed you wanted those.

1 Like

I like the adaptive ones, they seem smarter to me, and I think it’s super neat that the tool will be cool to the touch after running 15mm deep in some hardwood. Plus, at this point I just need to get these things cutting, so I don’t want to switch strategies now, when we’re so close to getting it dialed in.

Same here, I tend to use and abuse adaptive toolpaths :slight_smile:
Allright then, let’s finetune those sweet adaptive toolpaths then. I forgot to ask: how many flutes does your new upcut endmill has ? (and how did you adjust the F&S accordingly ?) Can you share the project in its current state ?

1 Like

https://a360.co/2Wbc0n0

Ok, here’s the latest version. The stock height is different because I faced off the piece of stock today to a slightly lower height, just to see how it would look.

The program ran pretty well! Still some tear out, and a bit of chatter throughout - you know that really ugly squealing noise it will make when it’s not exactly right, but no other issues.

I’d like to get it to be faster, but slower is fine if the results are better.

Hi @MrHume,

I had a look at your latest toolpaths, here are a few comments for you to consider:

  • About that chatter:

I initially said that your F&S looked ok,

But…that’s when you were using a 3 flute. You are now using a 2 flute (Amana 46321K). Since you kept the feedrate at 100ipm, the new chipload is therefore 100 / 2 x 18000 = 0.027", which in hardwood may be a bit too much (that’s outside of my goto range anyway). Now, you also reduced optimal load to 1.54mm from 2.54mm, so after chip thinning you chip thickness is down to 0.0023", still a bit high to my taste.

Mix this with a long reach endmill (1.5") and high DOC (0.6"), and I’m not too surprised you get chatter (do you have a stock Shapeoko ? standard Z ? which type of wood is it ?)

Here’s what your current F&S speed look like in @gmack’s excellent calculator:

Tool deflection is high : not directly a problem for surface finish since this is only for the roughing ops, BUT the tool may have a tendency to oscillate slightly under the cutting forces, and then chatter is just around the corner.

So I still think you may be pushing your machine a bit too much. You could reduce depth per pass (to say 120%D instead of 240%), feedrate (to bring it back to a more comfortable 0.001 to 0.002" chipload), or optimal load (I like 0.8mm, but 1mm should be fine)

  • About the finish quality / tearout:

use your previous downcut endmill (46052K) in all finishing passes, instead of the upcut you are now using for roughing, reduce feedrate to 60ipm, and my bet is you will get better walls.

1 Like

Hi Julien,
thanks very much for looking into this, as always, the help is greatly appreciated!

I think I must not understand how to use g-wizard correctly, since I ran all the numbers through there with the new cutter, and it seemed like it would all be good – and for the most part it wasn’t too bad. Here’s the screenshot of the results I get in g-wizard, in case there’s some obvious information that I’m not understanding: (very likely!)

The wood type is walnut. It’s two pieces, glued cross grain to one another for strength of the finished rings.

As for the wall finish, I would really prefer not to have to change the tool during the job. My eventual goal, once this is perfectly setup, is to create a jig that allows me to do 3, 6, (or even 9?!) of these all in one go, so I can batch them out.

The wall finish is pretty close as it is, but I think part of the issue is tearout on the roughing passes. I will set the optimal load even lower, and then slow down on the finish passes, and see if it helps. Do you think I should also leave more material behind after the rough?

Ha, the infamous “turtle-hare” slider. You have it set at “rabbit”, which is the most aggressive setting. And G-Wizard is done with more rigid CNCs in mind, so from my experience (with G-wizard), I rarely went above ~30-40% on that slider for the Shapeoko.

To be honest, I purchased G-wizard, played with it…and haven’t launched it for a year or so, because you can make it tell you what you want to hear with that slider, again on a Shapeoko that is. I have a feeling this is tuned for Tormachs and the like. Or, I just did not understand something, but Mr Warfield was not very helpful when I asked him about that.

Others are welcome to comment, I don’t want you to get just one voice on this, but to me 100ipm at 0.6" DOC in walnut, even with adaptive passes, is just too much.

Ok, if you prefer to stick with a single tool (understandable), I think you should do a single contour pass at full depth (that you can now do, thanks to the 1 1/4" length of cut…nice) for finishing, at a slower feedrate, to shave off the 0.5mm stock left in one go. Only increase the stock to leave (from 0.5mm) if you see remaining tool marks after the finishing passes.

Side note: for the fun of it, I’m checking how things would look with non-adaptive toolpaths only. I don’t want to derail you from converging to that optimal toolpath design you are after, it’s just so you have a reference point, if cutting time becomes an important factor down the line (and my guess is it will, since you do this for business)

1 Like

Yeah I’ve been thinking about the non-adaptive thing a lot, actually. I’m not married to adaptive - despite what I said above - I just thought that was the fastest possible way to do stuff, since you can go so deep. The real goal is to cut these as fast as possible, with the greatest possible reliability, and an excellent finish on the walls to minimize sanding. If contour is the way to go, so be it!

As an aside, the first batch of these I actually made on my Nomad, using a stock 1/8" cutter and just contour toolpaths from carbide create. They were only 25mm tall instead of 30, but the top of the cutter was still rubbing for a lot of it. There was a fair bit of tearout, and I had to go very very slowly so the chips could be evacuated, but they worked. The second batch I had cut by a professional CNC shop, but they charged me almost as much as a Shapeoko, which is why I bought it.

1 Like

Allright, I’m almost done with my little experiment in Fusion360 and contour toolpaths only, I’ll report soon.
(vacation time + coronavirus roaming the streets is an excellent combination for me to be spending a lot of time in the garage :slight_smile: )

So, here’s what a full 2D-contour approach could look like:

https://a360.co/39RLFyy

Basically, that’s:

  • roughing passes for each circle = slotting at 3mm depth per pass, 18000RPM, 54ipm (0.0015"chipload)
  • finishing passes for each wall = single pass contour cut at full depth, same F&S, but reverse direction (conventional cut instead of climb)

The total time is down to 37min, versus 56min for the current adaptive toolpaths (which I find too aggressive, still).

Just something for you to play with, not saying this will be better, but worth trying ! Keep in mind I have not actually run this, so double-check it.

Love this. The only question is whether a 30mm slotting operation will always go well. Is it possible to make the slots like 1.5x or 2x the cutter diameter, just to give it some wiggle room? I’m happy to change it myself, I’m just not sure how.

In wood, with a good dust shoe, I think it’s doable (especially since the cut goes from the inside to the outside, so there will always be a good amount of stock surface left under the shoe to not lose too much suction).

But, yes, slotting can be hard. You could indeed do most of the toolpaths as pockets instead of slots, by adding extra geometry (say a circle that is 1.5xD larger), and use pocketing toolpaths instead of contour toolpaths. @WillAdams has a nice thread about this for CC here.

Note that this would work for cutting the medium and medium to L parts, but that space between the L and XL circles is only 6.5mm wide I already had to tune stock to leave and lead-in/lead-out to avoid collisions there, so that part will remain a slotting toolpath…or you would need to change to a smaller endmill.

Also note that somehow we are already taking care of the slotting situation with the 0.5mm radial stock to leave, and subsequence finishing passes: even if the slotting passes are a bit brutal (well not that brutal, 50%D for DOC is not that high), we don’t really care if they will a poor finish.

If it were me, and cutting time was paramount, I would do this: try the full-slotting approach at an even more conservative DOC (say, 1.5mm), if it works increases DOC and see if it still works ok / until it doesn’t.

1 Like

Completely unrelated to this I was watching one of @wmoy’s recent videos about the excellent pokemon ball trophy , and if you check at 05:18, you will see a loooooooooooong endmill slotting around the piece, with no problem in sight :slight_smile:

1 Like

That unidentified “long reach 1/8 inch endmill” is apparently supported by Fusion 360, even though it appears to be cutting much deeper than the height of the cutter. :wink:

1 Like

Lakeshore Carbide Long Reach Endmills. Consider it identified. Also, I enable a roughing pass so it does 2 loops around the part per stepdown, one roughing one finishing. Benefit being that the endmill has some breathing room, isn’t rubbing both inner and outer walls of the cut at the same time. Could sketch in 2 circles to do it as a pocket, but the 2D Contour w/ Roughing is better.

2 Likes

@wmoy Thanks!
So there weren’t any “collisions” because the endmill’s shank is only rubbing one wall at a time, because you “lied” to Fusion about the 3/4" cutter length/shank diameter, or?
Care to share your speeds and feeds? Did you use Lakeshore’s guidance for plastic?

There’s no collision. The shank doesn’t stick out further than the flutes. It will rub a little bit, but as long as you don’t stop moving you shouldn’t cause any burnishing or scorch marks on the wood. Fusion doesn’t stop you if the final cut depth exceeds the length of the flutes.

2 Likes

This topic was automatically closed after 10 days. New replies are no longer allowed.