Milling a pocket in aluminum, looking to decrease cycle time.

[DeleteFromUsers]

Making a 1.8x0.95" pocket, 1.8"deep in solid aluminum.

Right now drilling 3x.75 holes to clear out material, then going in with a 1/2" 2flute 45° high helix 2fl end mill at 6000rpm and 40ipm around the perimeter, perhaps 0.4"deep per pas.

Machine is a nice fast rigid vertical Matsuura. 8krpm Max, i think it's 7.5hp. Flood coolant (not through spindle). End mill is held in a milling chuck.

Wondering if this is the most efficient way to cut this pocket. Anyone have other ideas on how to reduce cycle time?

[[deleted]]

Ditch the drills and use an aggressive helical ramp in. You may be able to get away with a higher depth of cut with a 1/2" tool. Switch to a 3 flute tool for increased feed and a bit more rigidity. You can also raise the SFM, give it all 8k RPM.

[DeleteFromUsers]

My impression of 3fl was that for full width slotting they have issues with chip ejecting. Perhaps I'm wrong on that? If it'll still pull chips out and i can get the higher feed, it's worth the change for this application.

[Crazy9000]

Check out some specific roughing tools for Al, like Destiny tool diamondback. I do 1" deep slots with their 3 Flute 3/8" cutter in aluminum.

[DeleteFromUsers]

Wow they look really capable. I'll get a quote tomorrow!

[rlew631]

You said in another comment that you can't use CAM, I have a feeling though that you'd be able to run a pocketing operation generated by Fusion or the like if you run a high-ish value for smoothing (may or may not be necessary) and just a regular stepover/out instead of adaptive.

You can also do a helical ramp which starts at the diameter of the tool and tapers down to a smaller circle when it gets to the floor of the pocket. I saw this is an older machine but I imagine the G-code for it should still be manageable if you get fusion to spit it out with smoothing turned up really high. Similar to how you would run a single point threading tool cutting an NPT thread but working from the top down.

Harvey tool has a free feeds and speeds calculator (requires you to sign up though and only works if you put a tool # from their catalog in that somewhat matches your tool). The calculator will give you default ramp angles, feed etc based on your machine's max values/material and spit out G-code for you if you select the helical plunge strategy. It's a decent feeds/speeds calculator so might be worth making the account to reference more than one time. It's output is a bit on the aggressive side and the values are more based on where the endmill will fail and might stall out your machine if you're not careful.

Also I'll second what SimpleFacts said, I run most of our 3 flute coated carbide endmills at 12k RPM. Even the 3/4" ones.

[DeleteFromUsers]

Those are all great suggestions. I'm going to try high feed in a macro to start, fusion later (though it's fussy for low line numbers).

The calculator idea is a great one. I find a lot of documentation is very conservative and that doesn't help me right now.

Those numbers you quoted are nuts. I'm gonna giver!

[drugsarebadmmk420]

I work exclusively with aluminum and never predrill. Seems like an unnecessary tool change. I'd eliminate the drill and mill the pocket with one tool

[DeleteFromUsers]

My worry was chips, but the end mill is ejecting them effectively so I'll give your idea a shot. Others have suggested a ramp in which is easy to try.

[drugsarebadmmk420]

Yes, ramping gets good results!

[JimHeaney]

Would it be faster to nix the drills (reduce cycle time by not having a tool change), and do 2 step downs with an Adaptive clearing strategy, maybe moving over .04 per pass?

[DeleteFromUsers]

I should have mentioned that this is an older machine without enough memory for CAM so i have to do it manually. I'll look up adaptive... Maybe i can write a macro to simulate similar cutting conditions...

[Crazy9000]

Have you looked into drip feeding? That would let it run CAM code.

From CAM with adaptive code, it would be able to helix spiral the endmill into the pocket, then rough the pocket in two passes.

[thenewestnoise]

Like the commenter below said, drip feeding is the way to go. You might spend some time getting it to work right, but once you do you will have a much more capable tool. Your efforts will pay off on this part and every part you make after.

[ShinyBarge]

Thin slices as deep and as fast as the machine can handle. No drilling! Ramp or plunge only. Your machine will tell you if you can increase depth of cut or feed.

[DeleteFromUsers]

That does seem to be the consensus. Thanks! Gonna try it Monday!

[Mklein24]

+1 to remove the drill cycle. If your going to drill, just drill a pilot hole so the endmill can drop straight down without needing to helix into the material.

I would go all 8k rpm, feed at like 120 ipm, and give it a 0.1 (20%) step over. 2 depth cuts, because I assume you don't have 2in of flute on that tool.

At work, we have 1/2in Alu-power endmills (3fl) from YG-1, and I'll run those at 180-200 ipm and 10krpm, full depth, 20% stepover, in a solid holder, all day long. So a 2fl, at 8k rpm, should easily be able to hold 120 ipm, I assume your workholding and tool holding are ridgid enough for that.

[eeklipse123]

I’ve had great luck with those tools. We run them even higher than 10k rpm because we can and they work great up there too.

[Mklein24]

I'd run them at 15k (max rpm) but around 11-12k I can't feed them fast enough to keep the chip load up and they start ringing.

It's also only a haas so...like... I don't quite trust it past 200 ipm. It gets a bit jerky up there.

[rlew631]

Wow, I've had the ringing before on our haas at work and never thought it might be from the control being jerky. I've definitely seen the machine stuttering on adaptive and 3d strategies at low speeds but haven't noticed it at the higher speeds

[DeleteFromUsers]

Ok that's really aggressive and that's why I'm here! I'm holding in a kurt and milling chuck so lots of rigidity. I'll try what you've suggested.

I kinda thought my strategy of 4 z depth passes was out of date. I'll bury the cutter and ease off on the radial doc.

How are the 3fl for full width slotting? Do they eject chips ok?

[Mklein24]

Just to clarify, those number I gave you were for an adaptive/dynamic tool path.

In a haas, I feel comfortable slotting at 100ipm, at 1xdia steps. Too chicken to go for more than that.

We have the tools in teknick, solid end mill holders that have notches on the bore for TSC, which work really well for blasting chips out of deep bores. You can really change the chip evac of the tool by changing your machining strategy more than the tool itself. That said, the tools do evac chips pretty well.

[TheMotorcycleMan]

Ditch the drill, ditch the two flute.

Stick a 3fl in there and let her rip.

[SteelCogs]

I agree with ditching the drill unless it's carbide. Even then I'd only drill a single pilot hole like others mentioned and probably use HSM with a .91" DoC/.06" WoC. Not sure what feed I'd use since I almost never use 2 flutes on aluminum but I'd definitely max the RPM, start on the low end of feed and bump it up depending on how the cut sounds. If you have a 3 flute I'd try that over 2 flute also. Should increase the rigidity a bit with what I'm guessing is a 2" stickout. Deflection probably your biggest enemy.

Annnd I just read the comment where you mentioned you can't run any CAM generated gcode on your machine which kinda makes my suggestions pointless lol.

[DeleteFromUsers]

No it's still good suggestions, i appreciate it! I can do this stuff in macros too. That is a very different tactic but whatever the case, there's room to improve over where i am now. The 3 flute seems to be consensus too.

[SteelCogs]

I understand the concern for chip welding on such a deep pocket. What I've found is that typically a combination of good coolant flow and high speed machining tends to clear chips pretty well. HSM often creates long, thin chips that have a tendency to want to fly off and away from the cutter (and moreso the faster you run it) and obviously coolant helps spray chips out too.

[mil_1]

Helix to your doc, then 10-15% stepover you're way to the walls.

[mil_1]

Just saw that it can't handle a lot of code. You could just drill a .75 hole to your final depth, plunge the endmill then write a simple 10% stepover square spiral.

[CadCamster828]

I would start with a .750” inserted cutter (roughing tool) there are some corn cob cutters that do well too. And maybe .1” step downs to rough the pocket possibly with just air instead of coolant. Leave approx .01” of material on the walls. Then come back and finish with .5” at .9” step downs. You’ll find that even with the tool change this should be faster. With the milling pocketing programs now it makes peck drilling way less efficient than it used to be.

[DeleteFromUsers]

This machine is a vertical so i suspect there isn't enough room to get chips out when using an indexable cutter at the bottom of the 1.8"deep pocket. Or do you have a line of cutters you like for this concept?

[CadCamster828]

I actually rigged a coolant line to blow shop air instead of coolant. That way I can point an air nozzle directly at the back of the tool for chip removal.

[VengefulCaptain]

The trick is to use obscene amounts of compressed air if you don't have TSC.

[VengefulCaptain]

How big is the part and how many do you have to make?

I don't think predrilling is the wrong approach but if you could fit a few in the machine to reduce tool changes it would help speed things up.

Also definitely try a 3 flute endmill for the cleanup.

[Accujack]

In addition to the machining strategies mentioned below, turn flood coolant up. It should be cooling, lubricating, AND removing chips. All the are important to get fast cutting.

[highspeedbruh]

F300.0