Feeds, speeds, and other topics for the home machinst

[Roger]

Dec 8, 2020 6:40:02 GMT David said:

Guess which profile here suffered from the cutter re-cutting chips and getting clogged up.

This was a brand new cutter. 2mm dia, 5000rpm, 45mm/min feed, 0.8mm depth-of-cut. This is why I cannot leave my automated machine unattended! Luckily I was in the room at the time and noticed the change in the noise being made. The spindle was already getting warm by the time I got there. I let it finish the cut figuring it would be easier to edit the g-code to start on the next bit. I got away with it and the cutter didn't break.



I was able to stop it, pry the jammed chips out of the flutes, edit the g-code, and continue.

They came out petty well really, just a few places where the burrs weren't great. Are you doing a roughing and finishing pass? You'll always struggle to get a decent finish if you try to do it in one pass. Personally I don't worry about chips. They don't really mess up the finish, especially if you're doing a light finishing pass after the bulk of the material has been removed.

[David]

I'm not doing multiple radial passes, just multiple depths.

I have a lot of trouble with chips clogging the flutes and then the cutter starts rubbing rather than cutting, and I'm not sure why you don't. If I stand there and keep an air stream going then the problem goes away.

The finish on the sides of all these except the obvious one was good.

I got a 4mm 3 flute carbide endmill not long ago to do the whistle body and it was fantastic.

[jasonb]

On parts like that I would probably use a Ramp cut which saves having to put in those entry holes that it looks like you used so the tool gradually drops down as it goes around the part and set that with a small amount of radial "stock to leave". Then do a final full depth pass at the finished size.

I'm with you on keeping the swarf clear as it will blunt the cutters and can affect finish, maybe more so with the feed rates I tend to use that give bigger chips and more of them.

I did run a bit of a slower feed than my usual last week but it was using a 0.5mm wide ended 60deg engraving cutter which is in effect only single flute and was cutting soft bending brass, it was happy with 60mm/min but could have gone faster, rpm was 5000.



Happy with how the letters turned out, all the aluminium parts have been done on the CNC too and they do produce a lot of swarf that needs to be cleared.

[Roger]

Jan 4, 2021 9:59:23 GMT David said:

I'm not doing multiple radial passes, just multiple depths.

I have a lot of trouble with chips clogging the flutes and then the cutter starts rubbing rather than cutting, and I'm not sure why you don't. If I stand there and keep an air stream going then the problem goes away.

The finish on the sides of all these except the obvious one was good.

I got a 4mm 3 flute carbide endmill not long ago to do the whistle body and it was fantastic.

I don't seem to have any trouble with chips sticking in the flutes, but then I don't think I push the cutters anywhere near as hard as most people do. I also avoid using cutters that are less than 5mm diameter unless I have to. Going more than say one cutter diameter deep is likely to make it difficult for the swarf to escape. It doesn't matter if chips stay in the cut and keep getting recut if it's a roughing pass. Any marks that might leave on the part are irrelevent since it's not a finishing pass. I leave it cutting completely covered in swarf, for hours at a time sometimes and it really doesn't matter in my opinion.
I clean off the swarf and take the last 0.2mm off, and that's usually all it takes to get a nice clean finish. I can't be doing with standing over something with an air gun. Life is too short.
Being in too much of a hurry is the number one cause of difficulties in my opinion. Cycle time is only important if you have to stand over it.

[David]

I don't use ramp cuts because most of my cutters are not center cutting so I figure a ramp is no better than a plunge. It's not much effort to make the entry holes so I prefer that if I can't get in from the edge. Same reason I don't like tabs much.

It's not the effect of the chips on the finish I care about, the finish is usually ruined by me afterwards trying to clean the cusps off. It's the flute clogging that causes me trouble. For some reason the chips get packed in the flutes so hard they take up all the clearance space in there and can't be got out without something like a scriber and a lot of force and luck. This really does happen a lot to me, and it happens on cutters from 6mm down. I'm guessing it is what caused the disaster with the mill table last year.

Less flutes probably makes them bigger which might help and that's why I bought the 3 flute ones recently.

[jasonb]

Less flutes does help and you can also use the ones designed specifically for aluminium on brass and bronze which have a steeper helix angle to get the swarf away faster.

I would not really want to be using a 4-flute on cuts like that anyway, keep them for contour work where you can get in from the edge or final finishing cuts where the swarf production is low. If you look at most of the makers feeds and speed data they don't even give speeds and feeds for 4+ flute cutters at full width only side cutting, although most of us can't manage their rates it's a good indication that the 4-flute are not the best choice for what is in effect a slot.

Provided the angle is low you should still be able to ramp down into the cut of bore your way in to a pocket with a non ctr cutting cutter 1-2 degrees should be OK

[Neale]

I use a mix of 3- and 4-flute cutters, recently in the 2-4mm range. The 3-flute are supposed to be centre-cutting, but in both cases I use ramping, usually with the default 2deg ramp that F360 gives me. It's much easier on the cutters than plunging, and saves at least one tool change compared to making entry holes - at least, if you are not doing any other drilling operations. I also use triangular tabs for the same reason, although it's noticeable that the down-cutting part of the ramp does seem a little harder on the cutter than the initial entry ramp.

I've been cutting out pieces from sheet and need the tabs to hold pieces in place as I prefer to keep a complete frame around the pieces for more rigidity. This is why I'm ramping rather than coming in from the outside - I agree with Jason that this is preferable when you can do it. Because I'm making profile cuts rather than clearing, I'm effectively slotting so can't use the more effective adaptive clearing strategies but I still cut slightly oversize then make a finishing/sizing pass. This is all in steel so chips clear easily with a suck from the shop vac at intervals.

Fortunately the loco I'm working on doesn't have many aluminium components so I don't have to struggle with that sticky stuff!

[Roger]

Jan 5, 2021 0:38:04 GMT David said:

I don't use ramp cuts because most of my cutters are not center cutting so I figure a ramp is no better than a plunge. It's not much effort to make the entry holes so I prefer that if I can't get in from the edge. Same reason I don't like tabs much.

It's not the effect of the chips on the finish I care about, the finish is usually ruined by me afterwards trying to clean the cusps off. It's the flute clogging that causes me trouble. For some reason the chips get packed in the flutes so hard they take up all the clearance space in there and can't be got out without something like a scriber and a lot of force and luck. This really does happen a lot to me, and it happens on cutters from 6mm down. I'm guessing it is what caused the disaster with the mill table last year.

Less flutes probably makes them bigger which might help and that's why I bought the 3 flute ones recently.

That doesn't make any sense to me. Personally I would avoid using non centre cutting tools altogether if you have to start a cut into the top face. The fact that there's no centre means that if you plunge straight into the work, you're leaving a lump of uncut material in the middle trying to stop the plunge. If you're successful in making the plunge, you then move sideways with the plug of material trying to snap off the cutter. If you really must use non centre cutting tools, I'd use 2-3 degrees of slope into the work so that the centre has the least amount of material left.

I'm not sure what you mean when you say "clean the cusps off"? You should end up with a finish without noticeable cusps if you use a fine finishing cut with conservative feeds and speeds. Are you using an adaptive cut and expecting to get a good finish? The finishing cut shouldn't be swooping in and out of the finish line, it should follow the exact contour you're trying to create.

Maybe you could post a video of a typical cut you're making? It sounds like you're trying to run miles too fast, generating way too much heat and overwhelming the flutes with too much material.

You'll find that Carbide cutters with a coating stops a lot of the sticking of material in the flutes. Are you using HSS tools? 3-flute cutters are good, they seem to give a sensible compromise. I use all types of cutters though, whatever is to hand.

[jasonb]

I thought I would post this for David regarding the recent mention of air to clear swarf. It's a flywheel cut from a slice of cast iron bar and you can see the swarf build up on the ledges during the adaptive cuts as I was not able to manually clear it while taking the various video clips. But if you can bring yourself to watch through to the 5min mark you will see I have finally rigged up some air which is just enough to clear the swarf ahead of the cutter. The first side I stood over the machine clearing swarf more so on the adaptive than the finish but decided I did not want to waste another 3hrs each side. The second side and second flywheel were left unattended except for doing the tool change trusting F360 to have spat out the right code as each side and each flywheel was slightly different and all went well.

Ketan at ARC suggested that I use an air tool lubricator as I did not want to soak the place in coolant as this is what John Stevenson had set up ARCs own machines and his four Sieg CNC mills with. I'll only be using liquid when cutting aluminium but it certainly worked well doing the CI dry. Only a small amount of air is needed - the regulator was almost turned off and the swarf does not get spread all over the place staying in the "trough" that the KX3 comes with. I'll make the fitting a bit more permanent once I have tried it with liquid and then look at getting a quieter compressor as my old Machine Mart one is louder than the mill. The LocLine is acting as a means to position the air only as I have run a 4mm OD PVC line inside that with a small brass outlet drilled 1.5mm to get the velocity up and it will save a build up of fluid in the LocLine before it comes out the end.

Speeds, feeds, cut and tool details are in the video

[uuu]

I prefer to do aluminium dry as well. I find that any lubricant makes the swarf more sticky, so needs a stronger air supply to clear away. The aluminium chips are hard, so if the cutter eats them it makes a crunching noise - and leaves marks in the finish.

Wilf