[jderou]

What fly cutter tool geometry is required for a good surface finish on aluminum? I attempted to use one last night but the finish was quite poor, it was kinda like the surface of a file (raised ridges).
Any input?

[RomaxxCNC]

Fly tool cutter geometry is a craft within itself. For steels such as 1018 I usually use C-8 carbide bits with zero rake on the face and about 5 degrees relief. The point radius should be kept to less than .06". Larger radiuses will deflect the tool/holder and resist, resulting in chatter, squealing and poor finishes. This same tool can be used with aluminum however, aluminum requires extremely sharp tooling.

For aluminum such as 6061-T6, I usually use a High speed bit blank. Grind about 60 degrees of rake on the face 1/2 from the end. 5 degrees relief on the bottom. The radius is left large, As much as .25" Strange looking tool but, they leave a very good and more importantly, accurate surface. They can even be used to fly tool rubber without freezing it. Handlap the cutting edge on a whetstone for best results. This type of cutter actually cuts, zero rake cutters on aluminum merely smear the material away. The file surface experienced was probably caused by too small of a radius or no radius. A big no-no with flytools or any cutter for that matter is allowing it to dwell spinning in one spot against the stock, not cutting anything. It takes the edge off of it it immediately. Keep it moving. This same cutter geometry works for lathe tooling as well in soft materials.

Ron

[PROTOTRAKFAN]

Forget using high speed bits. I recommend that you use a small lathe insert tool with a carbide or, diamond insert.......
Patrick

[Konrad]

I would use carbide, allot of rake, allot speed, and a small radius on the cutting edge, use coolant is all you need most of the time, or brush on a bit of cutting oil or varsol, or WD 40, perhaps on your very last cut, otherwise you have too much smoke.

Konrad

[ViperTX]

I guess you could also use a face mill...I use a Lovejoy 205 and it cuts beautifully.

[Mcgyver]

I use HSS all the time – using carbide defeats the purpose – something cheap and easy to sharpen at home . A fly cutter bit is no different than other - they need rake and clearance of the appropriate amount in the appropriate place, I grind them like a face cutting tool for the lathe. if your mill is trammed properly, you'll get a great finish with a nice cross hatch pattern

You must use it at the right speed - here is where carbide might work - if your mill won't go slow enough.

the following would run counter clockwise in the position pictured. the radius as exaggerated, and is done on the edge of the grinding wheel.

[jderou]

Thanks guys, I have ground a radius on the tip of the tool and that made a big difference. Still not perfect but getting closer. I have wondered about using a face mill, what kind of finish does it leave?

[One of Many]

Thanks guys, I have ground a radius on the tip of the tool and that made a big difference. Still not perfect but getting closer. I have wondered about using a face mill, what kind of finish does it leave?

What is your feed rate and RPM.

Using a single tooth fly cutter with a .03R on a 3" flycutter turning 1200rpm at 2.5-5"/min, you should get a very nice finish. The smaller the tip radius, the slower the feed to keep the finish decent.

Too large of a radius increases tool cutting pressure and the tendency to chatter. That can also lead to greater warpage in the part. I don't know if that is from friction induced heat or odd stress relief over a larger area. Not much you can do if the radius is required. Lighter finish cuts and a very sharp edge should help.

No fancy cutter material is needed unless cutting steel. Interrupted cuts are not as kind to thin brittle cutting edges. Rake can help and hinder depending on the chip desired. Long stringy chips are not fun to deal with. I prefer to have a chip breaker as was presented, but not as thin at the cutting edge with relief on the bottom so only the radius portion is cutting. The basic positive rake left cutting lathe tool works in most instances. No need to complicate it with fancy grinds for the most part.

DC

[jderou]

It seems like I was running more like 1000 rpm at 15-20 ipm. I'll try a lower feed tonight.

[One of Many]

It seems like I was running more like 1000 rpm at 15-20 ipm. I'll try a lower feed tonight.

Yikes!, that is .015-.020/rev with a single tooth fly cutter? Not surprising it was groovey! LOL!

Getting the feed rate down to .003/rev is going to be a big improvement. At least below 5"per min.

1000/3"per min=.003

If you see a nice cross hatch pattern develop, it means the head is trammed properly. If you see any steps for successive passes in either the x or y directions, this will indicate the head is out some or wear in the ways.

Be very aware if you have an automatic oiler on your ways. The oil can lift the bed floating on the oil during a cut when least expected at the worst possible moment.

DC

[jderou]

wow, I never thought about the automatic oiler thing, I'll have to watch for that. I do get some small steps between passes, but I have a Boss rigid ram, so I pretty much am going to have to settle for it. It may be possible to do some shimming, but it sure doesn't look like fun.

Joe

[One of Many]

I do get some small steps between passes, but I have a Boss rigid ram, so I pretty much am going to have to settle for it. It may be possible to do some shimming, but it sure doesn't look like fun.

Joe

This would be worth investigating. Point being if you see steps why fly cutting, the alignment for tool lengths will be compounded. Lets say you use a 1" long center drill and change to a 6" long drill bit. The place where the 2 tools actually position at there ends will have an exponential offset in whatever direction the spindle is oriented not perpendicular to the work. It is more noticeable when using long and short endmills and discovering a "mystery" shift in the "as cut" geometry.

DC

[jderou]

I tried running at .010 deep 1200 rpm and 5 ipm, results; Beautiful finish! and no step between passes. Head seems to be trammed in pretty good, my only complaint was that the cutter started squealing once it was fully engaged in the part. I reached for some undiluted cutting oil (only thing that was handy) but it didn't seem to help, i'm sure that vibration doesn't help the finish.
I have a job starting tonight that I will have to take .090 off a bunch of 3" wide peices. The finish on one side really doesn't matter so I'm thinking I will face the visible side as done last night, turn it over and then do the major metal moving. How much is safe to take off in one pass?

[jderou]

Trying to draw the appropriate cutter geometry, the cutter I am using right now is carbide so I can't do much modifying to it. I wan't to grind one out of HSS today. The attached is 30 degree rake, 5 degree relief and .062 radius. I am not sure how to incorporate the chip breaker, it seems like it would go right through the cutting edge.
When grinding, do you grind the radius first then the relief and rake?

[Mcgyver]

Joe, I've added some arrows to your image. This will remove metal on a light cut, but not as nicely as it could and not on heavier cuts. Assuming it's oriented in the image as it would be in the mill, the top rake is ground as if you want to plunge into the material in the direction of the green arrow. Think of this bit mounted in a lathe, a nice knife tool. It will cut well going from left to right. But take this tool this to the end of your work and try a plunging facing cut and you'd have problems. That’s what's happening when you fly cut - its cutting in the direction of the red arrow, not the green.

If you study the image I posted a few posts above, you'll see there is a crescent shape ground out of the end - the is what gives the tool the top rake for cutting in the direction of the red arrow, its not a chip breaker (well it is, but that’s just an added bonus). When using a fly cutter, its usually an interrupted cut so long chips aren't an issue anyway imo

This radius is exaggerated in the image I made - grind it on the corner of the wheel, its nothing fancy it doesn't have to be exact - anything that'll give you 10-15 top rake (30 is too much, does hurt the action of cutting but it does weaken the cutting edge). Btw, this is a standard (and the best imo) grind for facing tools for lathe work.

Also, don't forget clearance – It looks like you have no front clearance - the front of the tool (as per the red arrow) needs to be angled away from the cutting edge. If used as drawn, the edge after the cutting edge leading up the blue arrow will hit/rub, preventing the cutting edge from engaging properly

After grinding, stone the tool a little, sharpness does count, and put a small radius on corner. no need to grind the radius, doesn’t have to be big, just do it with a stone. This will give both a great finish and allow fairly high removal rates. As always, work out your feeds and speeds!

The grind you drew would be perfect for fly cutting if the tool was held vertically. Build a fly cutter of that type to use the brazed carbide tools if you don't to modify them. the type of fly cutter that has the tool more oriented as in your image, is better off with hss ground as per above

[jderou]

Is this what you are talking about? It just seems weird that that radius is going through the cutting edge, but I guess I am looking at it wrong. I have 5 deg relief on the bottom and on the side now.

[Mcgyver]

I think the confusion is over what exactly is the cutting edge - the thick red line is the cutting edge - this is a what traverses the work forming a a chip. we are used to, because of lathe work, thinking of the cutting edge as being along the side of the hss bit. in this case its on the end - its the same principal as any other cutting tool but you have to turn your head sideways to see it

btw, if you don't grind your lathe facing tools like this, give it a try - it will be your new defacto.

check out http://easyweb.easynet.co.uk/~chrish/tl-tools.htm. There’s a diagram half way down showing rake/clearance angles etc. every cutter, from simple lathe bit, to drills to shell mills has them, you've got to orient yourself to what the cutting edge is then where the rake and clearance has to be. Its good to learn this as the angles change substantially for different materials – knowing how to grind a bit or drill for different tasks is fundamental to good workmanship. Next you’ll be making your own specialty cutters from drill rod .

my comment in blue - you don't need this angle.
purple- shows how the top rake is formed by the crescent shaped grind.
front clearance, yours doesn't yet have any, i've shown it on the side view in orange.

does this clarify?

[jderou]

Let me try again. I guess I am looking at it as if the bottom were cutting when it isn't because you would never plunge and fly cutter. I think it makes sense now, can't wait to try it.
Is this better?

[One of Many]

I tried running at .010 deep 1200 rpm and 5 ipm, results; Beautiful finish! and no step between passes. Head seems to be trammed in pretty good, my only complaint was that the cutter started squealing once it was fully engaged in the part. I reached for some undiluted cutting oil (only thing that was handy) but it didn't seem to help, i'm sure that vibration doesn't help the finish.
I have a job starting tonight that I will have to take .090 off a bunch of 3" wide peices. The finish on one side really doesn't matter so I'm thinking I will face the visible side as done last night, turn it over and then do the major metal moving. How much is safe to take off in one pass?

Nothing like progress huh?

The chatter can be a result of excess radius, cutter angles, RPM, or thin material to begin with. Thin material should be fully supported, not just on parallels in a vise. Reading the material, cutter or reaction to changes can help pinpoint what is contributing to the chatter.

The cutter you have posted with the chip breaker is pretty close. I would not cut the groove that large or deep and if I did, I would reduce the hook at the cutting edge some. The idea is to get the chip to curl against itself so it will break off or at least be compact. I would also cut it at an angle behind the radius tip and not directly parallel with the front edge. Application dependent again.

As a side note.....on thin materials in taking more material off of one side verses the other. That can set up differing stress relief, which will spring the parts toward the side with greater material removal when released from workholding.

With a single tooth cutter, you could cut .125, but realistically around .06-.09 is not uncommon with a smaller tip radius. I have taken .375-.5 with a 4 stepped 4" flycutter. Just try to avoid taking a heavy pass that envelopes the full cutting radius of any fly cutter. Wiser to step over one half its diameter or use a larger fly cutter.

DC

[One of Many]

Let me try again. I guess I am looking at it as if the bottom were cutting when it isn't because you would never plunge and fly cutter. I think it makes sense now, can't wait to try it.
Is this better?

If you let the chip breaker groove run out slightly(shallower) before the radius at the tip, instead of all the way through as drawn. You will retain the tangent point of the tip radius that cuts the finish in contact with the face of the part. As drawn the tip radius will become ineffective.

I have not figured out how to post images as of yet.

DC