[kong]

Following on from my previous post regarding internal profiling of aluminium, I have got some new tools, and the special geometry ccgt/vcgt inserts. Now the biggest problem I have is the swarf in the hole! I have added a piccy of the part, and you can see the chatter marks on the inside rim. I am using a facing op with a boring bar, high spindle speed, low feed, and 0.4mm depth of cut (Yeah, my little lathe loses too much power at high speed). I tried boring rather than facing first, but the 2' curly swarf was just clogging in the inside and damaging the cutting tip eventually. So, how can I reduce the chips into, well, chips?! I am running out of materials and inserts here, so would like to get it right without another load of practice runs. Any advice would be appreciated.
Oh yeah, I am using flood cooling, would a switch to something else make a difference?

[kong]

The piccy needs to be uploaded (chair)

[WOLOG]

Hey Kong, Try increasing your feedrate and/or depth of cut to get it to chip better. It may also be the geometry of the insert. If I am correct, you should have a positive geometry insert to cut aluminum. How fast are you turning? You may want to try stick less of the boring bar out to reduce the chatter. You should only have about .100" or so longer than your longest "Z" depth. Anything longer is not good for anything.

Hope this helps.

[WOLOG]

Oh yeah, try blowing air in the hole to remove the chips if coolant is a problem.

[SMOA]

I agree with wolog, mabey shorten up your boring bar. How far is the boring bar hangin out, what is the dia of the bar, and what is the Dia of the hole? Also mabey less of a radius on the insert, and a little positive rake.

[cnctoolman]

Kong,
Also what type of aluminum are you using. I have found that 3003 is really stringy and doesn't want to chip off any way I have tried especially when doing a finishing cut. And as the others say the chatter looks like your feedrate is either too slow or your rpm is too fast. One other thing to double check is your tool height in relation to center.

On a side note you can also buy high speed steel inserts and they cut aluminum better sometimes than carbide will depending on the situation. I will post the link if I can find it again.

[cnctoolman]

Here is the link to the high speed steel inserts:

www.arwarnerco.com

[HuFlungDung]

My sympathies, Kong. I haven't found a way to make a finish cut in aluminum to break chip dependably, that's why I mill it as much as possible, particularly when working inside of a hole.

Are you roughing with this same tool, all the way to finish? What are you starting from, a drilled hole? How many cuts is this insert taking before the final finish? I'm just wondering how perfect the edge is before the final cut. If it is suffering built up edge, that can skuff up your surface, too.

The volume of metal you are removing still generates a fairly stiff chip. I would try a finish cut of .005" depth, in an attempt to keep the swarf building very slowly in volume, and being very lightweight. You might have to retract from the hole at a suitable position (say as the tool moves over a corner or something), to remove the swarfnest before continuing. Hopefully, you can then move right back in where you left without leaving a toolmark.

[kong]

Cheers guys, seems I am not alone here! The inserts are ccgt, sharp, positive rake, designed for aluminium. 0.4mm rad on the tip, I am using the same cutter for roughing and finnish, just reducing the feed speed.
Hu, I am fairly certain the chattering is caused by a damaged tip, which has suffered due to the swarf getting wrapped around it, then the cutter pushes it int othe side of the part. Although the facing op leaves an almost mirror finnish on the internal face of the part, it is just the sides that are screwed. Perhaps a different style of bar?
I am starting with an 18mm drilled hole, then facing around 2mm off of the piece before it gets to work inside. The bar is a 12mm diam, and is not suspended any further out than it needs to be. I guess I could switch to a larger bar, but that means using a boring motion, rather than facing, and there is where the problem is with the chips.
Perhaps I will take a smaller cut, and play with feed speeds to get those chips to form a little better. Thanks guys, I will let you know when I get it sussed out!

[HuFlungDung]

What bar number was it, Kong?

Is there any way that you can position the bar at an angle to the bore, in order to give it a little more clearance? This may help.

I was going to suggest that you face from the center outwards, but stop at the corner, then bring the tool out of the hole and bore the ID. If you get a really light chip going, you might be able to rig an air blast to try to blow the chip out, or at least farther up the bar, instead of bunching around the tip.

I would probably rough that part with a different bar than I was going to finish it with, just to keep that tool tip in perfect condition for as long as possible. Just keep throwing money at the problem until it works out right

[kong]

Lol, nice one Hu, I will have to get a sub off the missus!
Seriously though, the bar I am using is a standard SCLCR boring bar, but the other bar I bought is the kennametal A-SVMB which uses vcgt inserts with a 50^ angle to the flank. The problem is that I cannot rough with this bar since it has a tendancy to dig into the workpiece. I will have a go tomorrow with lighter cuts, and the air blast.

By the way, I got a nice Trico MD1200 unit winging it's way to me from the US, hope to get that delivered next week, thanks for the advice, albeit some time ago now!

[metlmunchr]

Kong, I use a lot of ccgt aluminum specific inserts for aluminum, and, unless something is happening to the corner of the insert, your problem lies somewhere other than with the insert. I'm speaking strictly about the chatter now. Once chatter is established, it's real difficult to cut it back out of the part, as the frequency of the previous bumps excites the tool at exactly the right frequency to produce more chatter. Overall, the cardinal rule when a turning operation starts chattering, is to reduce the speed and increase the feed. As Hu pointed out, the ideal situation is to leave just a few thou for the final pass. The fact that this wispy string wont break doesn't matter, because its not strong enough to hurt anything. When you describe the operation, it sounds as if you're making the hole via a succession of facing cuts deeper and deeper into the part instead of a normal boring operation. If my reading of this is correct, then you're putting additional forces on the bar as opposed to a z direction boring op. Moving in z, the bar will be deflected by the force of the cut, but the force it takes to push the bar into the cut is largely reacted straight back up the bar to the holder. In a facing cut, the same cut force deflects the bar downward as before, but the sidewise force required to push the bar into the cut is now pushing the bar sidewise instead of axially. Within the limits of your lathe, I'd try to slow the spindle and increase feed in an attempt to break chips. Coolant is good because you want the aluminum to stay as cool, and therefore as hard, as possible. If you can tell me the rpm limits of your lathe, and where you've been running as far as speeds and feeds, I've got one turning center that stays set up for aluminum with _cgt insert tooling. I can stick a chunk of bar in the lathe and diddle with the parameters and pretty quickly determine what you might run to break chips on the roughing passes. Because these are micrograin inserts, they are surprisingly tough. Using the right numbers, I think you can still rough and finish with the same tool.

[kong]

Thanks metlmuncher, I am running between 1350 and 800 rpm for my cuts, the lathe has speeds from 150 - 1800 rpm. My feed speed is around 100 - 150 mm/min, although I can go faster, off the top of my head, to around 1000mm/min. The reason I switched from a boring motion to facing was due to the incredible amount of swarf wrapping around the bar inside the hole - which prevented a clean cut, and stopped the coolant reaching the tip. I figured the facing motion would allow the swarf to clear itself, without a lot of thought (and experience) to the stresses on the bar itself.
I would appreciate some pointers as to feeds and spindle speeds, but like I said, I will also try some air blasts to clear the chips.

[Zep]

blind hole boring can always be a problem. Looking at your part I'd figure the biggest hurdle would be to rough it out. In that case I would step it out working in from the face. high rpm high feed (assuming setup is rigid) to break chips , lots of coolant to flush. Finishing high rpm again light cut .02 on dia .005 to .01 on face. insert style i would use a vnmg stle profiling insert with a large lead angle. Reason for this is, smearing is caused by chips being trapped between bar and work damaging surface. try to keep area directly around the bar clear of pinch points. This style insert works well for finishing with a small toolnose rad (.015); less prone to chatter . keep bars short as others have suggested .I have had good results using VNMG style inserts for finishing. Most suppliers will reccomend a grade/geometry to suit your needs
good luck

[RotarySMP]

How many of these do you need to make? The easiest solution might be to put a dwell on each retract and remove the swarf from the tool tip with a hook.

[kong]

I have loads to make unfortunately, like a hundred or so. I have just got my car fixed (damn stupid thing) so I will have a go this afternoon, after a nice coffee

[RotarySMP]

Is the alloy critical? How about changing to a leaded free machining Alloy?

[kong]

Fairly critical, these will eventually become alloy wheels for small rc-cars, so I am using 6082 for it's strength, corrosion resistance and ability to be pollished easily. Also, there is not the range available in the UK as in the states, so I think I have a choice of about 3 alloys which are readily available! Anyhow, I have jusu re-programmed the part to use a higher feed, and a boring motion. Just gotta drink the coffee now!

[RotarySMP]

I have been doing a lot of boring on my little cnc converted mini-lathe and tried a carbide insert bar with a thin carbide shaft, a larger diameter steel bar with a sharp HSS bit and a well used brazed carbide bar. I was really suprised that the brazed carbide bar gave by far the best surface finish and chatter resistance.

In your position I would try the variety of bars you have on hand. Not very scientific, but easier faster and cheaper than ordering new ones

[kong]

HA! Got it.
I ran a faster feed, lowered the spindle speed, and took a shallower cut so as not to stall the lathe. Unfortunately, I never left enough of material for a decent finnish pass, so some of the roughing marks are still visible. There is also a tiny bit of chatter on the inner most radius, you can just make it out in the second picture.
I ran
Spindle - 550
Feed - 300mm/min
DOC - 0.25mm
Hopefully I can take a bigger cut, and up the feed a bit more, since the motor wasn't struggling at all (stop laughing all you guys with 20HP lathes :boxing: ).
The chips were different altogether. Some breaking up, and some a tighter curl, a bit thicker than the last lot. So a big thankyou to you guys :cheers: