Anyone else tired of modern CAM pushing adaptive clearing on deep pockets?

[u/CelinnLee]

Had a batch of 316L manifolds with 4:1 deep cavities this week. CAM programmer insisted on full-depth adaptive with an 8% stepover, swear they think trochoidal fixes everything lol.

Tool pushed off nearly .003" at the floor and left a nasty taper from deflection. Swapped over to a 16mm high-feed cutter taking .025" steps instead. Directing the cut forces straight up the spindle dropped cycle time by 20% and honestly saved the floor finish. Are CAM defaults making everyone forget basic tool deflection, or did we just botch the speeds here?

[u/albatroopa]

I don't get it. You're complaining about adaptive clearing and your solution was to switch tools? Strategy and tool are two different things. I run adaptive clearing with high feed mills all the time.

No offense, but your post comes off like it's chatgpt.

[u/computekmfg → u/albatroopa]

Why are you using adaptive with HFMs? Your cycle time will sky rocket and your tool life will suffer. HFMs like a full cut. Adaptive guarantees a consistent non full cut.

[u/TwoDudesOnACamel → u/computekmfg]

You can run an adaptive toolpath with a full width stepover... 

[u/computekmfg → u/TwoDudesOnACamel]

Why would you? It won't make it more efficient. The idea of adaptive is to go full depth. You gain nothing with a HFM

[u/TwoDudesOnACamel → u/computekmfg]

No, the idea of adaptive is to have constant engagement so your tool can run at maximum parameters more of the time and avoid shock loads. You can do that with whatever flute length your tool has. It works for both HSM and HFM tools. HSM is high axial and low radial engagement, and HFM is high radial with low axial engagement, both benefit from keeping that engagement steady throughout the cut, which is what adaptive toolpaths do. 

[u/computekmfg → u/TwoDudesOnACamel]

The end result when you use adaptive on HFMs is longer cycle times and worse tool life. You are running HFMs wrong.

[u/zmaile → u/computekmfg]

So you're saying when you run HFMs with adaptive you get worse results, and therefore ... the other person doesn't know how to use them?

[u/computekmfg → u/zmaile]

Adaptive works fine for HFMs but the air cuts and arcs when it should just be long cuts makes it a bad choice. It will be worse. HFMs already chip thin based on the geometry of the inserts. By adding more Radial thinning toolpaths does not improve performance. It will work but is entirely not as good as a well thought out spiral or offset toolpath. Even better if you make a custom toolpath to create a full width constant toolpath.

[u/TwoDudesOnACamel → u/computekmfg]

I get what you're saying, and I have had parts where adaptive sucks for HFM, but my experience is that it's generally pretty good. 

[u/computekmfg → u/TwoDudesOnACamel]

O it will work. It's just a waste of time.

[u/CelinnLee → u/albatroopa]

fair point, you're right that strategy and tooling are different things. english isn't my first language so i definitely butchered the wording there.

what i meant was full-flute adaptive with a solid carbide vs shallow .025" steps with an indexable high-feed body. in 316 at 4:1 depth, the radial load from standard flute engagement around corners was pushing the tool off hard. swapping to the high feed took that side force away and directed the cut straight up the spindle.

[u/albatroopa → u/CelinnLee]

But you still used adaptive? Or did you use something else?

And I swear to god, if the response starts with "Great catch!" ...

[u/Oldoutoftouchgamer → u/albatroopa]

This. Adaptive should not have a problem with corners . It's whole shtick is thick to thin chip formation/consistent engagement. Sounds more like either not actually adaptive patching or mismatch between programming and machine capabilities. Also to albatroopa, true high feed endmills do not benefit directly from adaptive motion. They are already chip thinning.

[u/albatroopa → u/Oldoutoftouchgamer]

They still benefit from not shock loading on entry, which is the actual purpose of adaptive. Chip thinning (radial, at least) is a phenomenon that has more to do with the ratio of feedrate to stepover, which is also seen in most adaptive toolpaths, but not necessarily. In fact, high feed mills prefer a greater than 50% stepover, meaning that radial chip thinning is pretty much out of the question, and they rely on axial chip thinning.

[u/CelinnLee → u/albatroopa]

no, dropped adaptive completely. just plain 2d pocket. at .025" depth adaptive just burns cycle time on air moves.

[u/mykiebair]

Few things going on here. Adaptive is not the way to rough pockets. It doesn't allow for great chip evacuation and often times has a much longer cut time than a pocket. High feed endmill will always win on this stuff. They are beasts.  The defaults in cam are just that defaults.  Your programmer should know how to massage the parameters for the material and part geometry. 0.003 deflection isn't great but it should still be within your clean up. 

[u/Mklein24]

At 4:1 depth, I would shoot for a dynamic/adaptive/constant radial as well. But what's the actual size? 2in square with 0.5in radi? Or 10in square with 2.5in rad? Those at both 4:1 but will dictate very different tooling solutions.

There's a ton of benefits to constant radial engagement tool paths. 0.003 of deflection is more than acceptable for roughing. It's roughing, it doesn't matter so long as there's enough material for a cleanup.

Some cutters have special flute geometry that will keep the tool perfectly straight during a cut so long as you use the whole flute length.

[u/TimeWizardGreyFox]

Using adaptive clearing and not leaving excess for a proper cleanup pass using conventional/climb milling on the walls and facing the floor is a choice. Sounds like user error, adaptive clearing isn't meant to be an accurate process and has built in stock to leave baked into fusion360 specifically to run cleanup passes with accurate cam posts. Doing step downs is going to create more wear on a smaller area of the end mill, you pick your poison but HSM using full tool engagement is very efficient with a proper endmill and endmills last far longer. 

[u/TwoDudesOnACamel → u/TimeWizardGreyFox]

High feed mills only cut at the tip, so his second strategy is actually using the full flute depth. They're meant for that. 

[u/Impossible_Bar955]

I'll use adaptive on deep pockets, but I'll predrill. Use adaptive down to where I no longer get enough axial engagement, then switch to a traditional method with shallow passes.

[u/Paddle-111]

I always found adaptive to be great for outside bosses/perimeter cuts where you can keep the chips from clogging the cutter. Deep pockets can be tough when the flutes get packed, especially on vertical cuts. Horizontal can help a lot. If I run into problems with being too deep sometimes use a mix of both, adaptive down to the sweet spot then conventional step down the rest. Lots of variables.

[u/BartlettComponents]

The bigger issue for me going deep in stainless is chip evacuation/ recutting chips. I don’t have TSC, so I pre drill, and adaptive at multiple depths to save the end mill.

[u/computekmfg]

Adaptive has its place but definitely has places where it is the wrong choice. HFMs are great for your application.

[u/yeet-ism]

4:1 cavaties taken in 1 depth. Interesting choice.

[u/Ok-Amphibian1447]

I think it is a mix of both. Experience and fundamentals both matter

[u/milehighxr]

When i do "adaptive" or HSM tool paths i program a 2nd tool as a finisher. The rougher leaves .01" floor and wall stock minimum material dependant, and then my finisher comes in after that. I have one AL rougher that runs at 300+ ipm and .05" stepover(1/2" endmill) at 5x doc. Then my finisher comes in at 75ipm. Again 1/2" diameter tool. Rougher is 5fl with coolant ports, and the finisher was 5-7fl iirc. Haven't looked at that part in 2 months or more....

[u/z00k79]

I don't think cam programs really push anything, per se... Fusion especially doesn't "suggest" a type of toolpath for a given geometry. It's up to the user.

The marketing definitely focuses on specialized features, but in the actual program, the user is choosing what to use. Sounds like your programmer learned a valuable lesson and will probably consider traditional pocketing with HFM tooling for pockets like this in the future. It's pretty common in the industry. 

Another aspect: A lot of newer programmers or people who learned on less-than-industrial machines (hobbyists, students, etc) learned to use adaptive on everything because of lower quality tooling and more predictable behaviors, with essentially zero focus on MRR or quality. 

[u/Shadowcard4]

HFM are designed to maximize tool life and be a roughing strategy that must be finished. Though 4:1 sounds very deep and i believe HFM stays in its stride at 2x. It is also more demanding on the machine, vs swapping to a high feed like you did works better with bigger ratios as deflection is less and it potentially evacuates better especially in a pocket. If the HFM path isnt using like 1.25-1.5x feeds and speeds compared to recomended (unless thats the spec the manufacturer put on the tool) then thats also wasting money at that stepover as HFM reduces heat and has a lot of chip thinning that must be accounted for when using the path compared to a high feed where they are given the parameters for ballz to the wallz out the gate to account for the chip thinning already.

[u/Artistic_Science_981]

Try the free smart rough plugin. It takes into account tool bending limit, power, torque limit to find right set of parameters.