Trochoidal milling - anyone not doing this?

[eaglemike]

I'm using this whenever possible (almost always). Started a few years ago. Greatly improved tool life and cycle times. Just wondering, is anyone not using this? I've used code created by BobCad and OneCNC with success. Seems like I read somewhere a lot of companies are using the same underlying engine and creating their own overlay, or interface. Is that true?
My VF-2 without high speed machining used to choke on the code, but the little MiniMill2 with that option turned on handled it well. Anyone have machines that don't like it? Success stories? I'm interested in hearing your experience. TIA.

 

[lobust]

Are you talking about actual trochoidal, or adaptive? I'm confused because of the choking on the code...

Featurecam has had trochoidal milling for about as long as I have been using it (15+ years) and I have used it a LOT.

It generally works really well as a substitute for adaptive on older machines because the code is much leaner.

I still use it sometimes as Featurecam's adaptive toolpath (called Vortex) can be a bit fussy in some circumstances and not work properly, but the older trochoidal toolpaths always work.

 

[primeholy]

I use gibbscam and we have a plug in called "Volumill" that we use for that. I program 3 makino f series machines (two f5's, one f8) so choking on code has never happened. I had never used it, or heard of it till this job I took almost 8 years ago. Before that I was using a base level bobcad on fadals(along with programming at the controller) and before that old ass mastercam on old fadals. My first job I was using Bridgeport EZ mill on a Haas, bridgeport tree, bridgeport Interact machining center, and doing some hand coding.

 

[primeholy]

Oh, to add, I dont know what we would do without volumill. Well, actually I do. We would take a lot longer to make parts, and go through a lot more end mills.

 

[Herding Cats]

I haven't tried every HSM path but I think you would be hard pressed to find one better than iMachining. But it is only available for SolidCAM, InventorCAM and NX.

It's pretty easy to choke up an old control with but it can be made to work by adjusting some settings.

 

[SD&M]

We’ve got Volumill in TopSolid 7 and use it quite a bit. We’ve also got trochoidal but don’t use that nearly as often because VM is a better fit. Yes, I can see an older/slower control being unable to really take full advantage of a VM toolpath, and in that case a trochoidal path might work better (I suspect you’d have to do a proper test on your machine to determine this). If you open up the calculation tolerances in VM you can greatly decrease the size of the code and this may help with an older/slower control.

Google “radial chip thinning” if you want a better understanding of how and why these two related but different strategies actually work.

 

[eaglemike]

My first experience was with BobCad, close to 10 years ago maybe (I don't think he lower levels have the adaptive roughing). When doing pockets with islands in aluminum, the Haas machines were pretty jerky, and the programmed feed rate was never reached. Maybe I should have called it adaptive? Using arcs does improve/shorten the code.
Back then I just guessed about which Haas machine to pay the $2500 to turn on the high speed machining option. It made a HUGE difference in cycle times, and the movement got a lot smoother.
The stuff I'm using sounds a lot like Volumill. I'm switching to OneCNC,* and happy with how their pocketing is set up using this feature. Scared the heck out of my helper when I had the non-cutting moves set to 750ipm. He freaked out when he saw that in the code.
I need to figure out how it decides to start the path, using either program. Selecting the outer boundary/stock, then any islands to avoid, using open pocket, it sometimes starts where I would not anticipate. It works very well, sure removes material fast, and as noted above, tools last a lot longer.
*BobCad's new subscription pricing and level of customer service model is pushing me away. They just don't seem to be as helpful or customer servoce oriented as they used to be. OneCNC seems to process faster and doesn't crash like I've had several versions of BobCad crash over the years.

 

[vmipacman]

Would you say Trochoidal is a specific adaptive path? It’s what I use for slot clearing. The way I use it, not the right way probably, it’s slower than conventional paths but much more reliable and easier on tools. I can set that up on a big slot or channel at full depth and leave it for a 45 min cycle and know I’ll still have a tool when I come back. Conventional path I’d have to take multiple depths and it likely not evac the full slot and break the tool.
I also just run the adaptive at normal tool speeds and feeds so I’m not taking advantage of that like I should.

 

[g-coder05]

Featurecam has had trochoidal milling for about as long as I have been using it (15+ years) and I have used it a LOT.

One thing about FC is it had chip thinning many years before they announced it. In FC hover the mouse on the bottom right of the widow and left click. They had loads of hidden features in there. Whirlwind, Chip thinning, auto program optimization, post add ins, so much that they don’t tell users.

 

[eaglemike]

I've been using HSM advisor, seems pretty useful. I was able to beat the spec's though on my 17-4 job using chip thinning/adaptive roughing/trochoidal milling. I upped the RPM a fair bit and then increased the feed until it sounded good. Tool life is wonderful and cycle time is down. It's only a 1/4" tool, and I ordered a bunch from Frank with .020 radius and coated. I'm running flood, although I know some run air.
One slot it's slightly better to use "conventional type slotting" by a bit. Having the 1.5 second tool check (for broken tool) on the Brother is pretty nice, if a bit scary the first few times.
This cnc stuff is just a little bit handier and faster than the days of leather belts, lacing devices and lineshafts.

 

[lobust]

Would you say Trochoidal is a specific adaptive path? It’s what I use for slot clearing. The way I use it, not the right way probably, it’s slower than conventional paths but much more reliable and easier on tools. I can set that up on a big slot or channel at full depth and leave it for a 45 min cycle and know I’ll still have a tool when I come back. Conventional path I’d have to take multiple depths and it likely not evac the full slot and break the tool.
I also just run the adaptive at normal tool speeds and feeds so I’m not taking advantage of that like I should.

A trochoidal path is a specific motion of overlapping circular movements joined tangentially by a short line. It's a misnomer as it's not a true trochoid, just looks a bit like one I guess.

The point being, that it's a specific motion that is inserted in a toolpath, not really a toolpath in and of itself.

 

[Mike1974]

Would you say Trochoidal is a specific adaptive path? It’s what I use for slot clearing. The way I use it, not the right way probably, it’s slower than conventional paths but much more reliable and easier on tools. I can set that up on a big slot or channel at full depth and leave it for a 45 min cycle and know I’ll still have a tool when I come back. Conventional path I’d have to take multiple depths and it likely not evac the full slot and break the tool.
I also just run the adaptive at normal tool speeds and feeds so I’m not taking advantage of that like I should.

I think that's a fair question... what's the difference between trochoidal (?) and adaptive? Mastercam uses "dynamic".... I would *guess* adaptive means the cam figures out the best/fastest way, and trochoidal is defined by the user with parameters like doc woc...? Curious...

 

[lobust]

I think that's a fair question... what's the difference between trochoidal (?) and adaptive? Mastercam uses "dynamic".... I would *guess* adaptive means the cam figures out the best/fastest way, and trochoidal is defined by the user with parameters like doc woc...? Curious...

Trochoidal is as I described above. "Adaptive" means that some variables of the toolpath are "adapted" "dynamically" to maintain continuous tangency and constant or maximally limited tool engagement, those variables being stepover, engagement angle and tangential velocity (by means of feedrate)