PDA

View Full Version : Burrs after side milling.



Black_Moons
11-15-2009, 07:38 AM
Hi, im side milling the ends of some cold rolled bar (5/16") with a 3/4" 4 flute TiN coated endmill at 500rpm with cutting lube at 6IPM, 0.05 or so width of cut, and wondering why I often get a giant burr on the end of my cut? Any way to minimize that? Should I be using a smaller endmill? A better non chinese endmill?

The bar is supported within 1/4" of the cut by a custom made split collar block in my vise, so I suspect its supported well enough for the cut.

brian Rupnow
11-15-2009, 09:43 AM
The man who sharpens my end mills told me that many Chinese endmills are not sharpened properly (when they are made) to cut on the sides---Only on the ends. Odds are pretty good that you have an endmill thats ONLY good for end milling.----Brian

JMS6449
11-15-2009, 10:00 AM
Think If you are convential milling it is the last of the material and there is no support and it is pushed over. Climb mill and it will be much less. There are always burrs when cutting.

Mcgyver
11-15-2009, 10:06 AM
The man who sharpens my end mills told me that many Chinese endmills are not sharpened properly (when they are made) to cut on the sides---Only on the ends. Odds are pretty good that you have an endmill thats ONLY good for end milling.----Brian

huh? then they'd only be good for plunging straight down, like a drill.....any other action IS cutting on the side See if you can plug him for more details on what he thinks is wrong with them. It may be there's something or maybe a tool grinder has a vested interest in trashing cheap throw away imports....seems a stretch that the entire chinese end mill industry has got it wrong and makes stuff that doesn't cut well on the sides; what use would they be?

Black_Moons
11-15-2009, 10:32 AM
Iv tryed climb milling and it does help somewhat, my endmills do wonders on aluminum so I doubt its that they 'can't cut sideways', just this little bar makes like 1~2mm burrs at times conventional milling.. little excessive..

BobWarfield
11-15-2009, 11:01 AM
Try picking up the rpms and the feedrate.

First, the shallow cut relative to the end mill's diameter is causing some chip thinning. So you chipload is less than you'd think.

Even if we ignore the chip thinning, G-Wizard would call for more like 900 rpm and 19 IPM.

Cheers,

BW

Evan
11-15-2009, 11:35 AM
What does it sound like when it is cutting? If it is cutting properly it should make a smooth purring sound. If it is pushing the metal it will make a louder almost clattering sound.

Another indication is to make a second pass without changing the depth of cut. Does it cut some more? If it does it isn't cutting well.

brian Rupnow
11-15-2009, 11:41 AM
huh? then they'd only be good for plunging straight down, like a drill.....any other action IS cutting on the side See if you can plug him for more details on what he thinks is wrong with them. It may be there's something or maybe a tool grinder has a vested interest in trashing cheap throw away imports....seems a stretch that the entire chinese end mill industry has got it wrong and makes stuff that doesn't cut well on the sides; what use would they be?
Really--and I have found no reason to not believe him. The Chinese end mills I took to be sharpened were what initiated his statement, but when he examined them he said that they had been sharpened correctly from the factory. He did say that he has had many Chinese end mills brought to him that never cut properly on the sides, and that a close visual inspection showed that one of the critical angles which make them cut on the sides correctly had never been ground on the mills, ever.

Mcgyver
11-15-2009, 11:48 AM
Try picking up the rpms and the feedrate.

First, the shallow cut relative to the end mill's diameter is causing some chip thinning. So you chipload is less than you'd think.

Even if we ignore the chip thinning, G-Wizard would call for more like 900 rpm and 19 IPM.

Cheers,

BW

wtf is a G wizard?

here's the M Wizard; rpm = CS * 4/ Dia = 100 * 4 / .75 = 500 rpm. you're fine where you are, faster will just wear the cutter out sooner.

19 ipm? in steel? my full sized XLO doesn't have a feed even half of that....feed rate has to take into account the machines removal rate capabilities. that's over 006 chip load - i thought 6 ipm was aggressive.

a chip is formed along a shear plane ahead of the tool. There's a fair bit of metal deformation happening at that point - when it gets to the edge some of this deformation happens below the plane of the cut which creates the burr. To reduce/eliminate, you've need to reduce the extent of the deformation of the metal - lighter cut or sharper tool for example.

Mills throw up burrs, knock them off with a file.

Carld
11-15-2009, 11:49 AM
Good post Mcgyver.

Think about what your asking the endmill to do. The helix action of the mill pulls the metal up as it cuts so just where do you think the burr will be? There will be a burr on the bottom of the work as well, just not as much. When the mill reaches the end of the work the metal that was leading the cut will remain on the surface of the corner. It always happens that way, sometimes more, sometimes less.

Anytime you cut metal your going to get a burr, sometimes big and sometimes small. Even if the endmill did not have a helix and was straight fluted it would still leave a burr.

If your going to do machine work your going to have to do some hand work and learn how to deburr the work.

Your expectations are to high as to burrs on the work.

Mcgyver
11-15-2009, 11:57 AM
Really--and I have found no reason to not believe him. The Chinese end mills I took to be sharpened were what initiated his statement, but when he examined them he said that they had been sharpened correctly from the factory. He did say that he has had many Chinese end mills brought to him that never cut properly on the sides, and that a close visual inspection showed that one of the critical angles which make them cut on the sides correctly had never been ground on the mills, ever.

The point was Brian that if they didn't cut on the side they'd be useless and returned to the store en-mass....except for the odd plunging job, that's all and endmill does is cut on the side.....the way you describe above makes sense, that there could be a lot variance to the quality of the grind and a poor grind would create more deformation and hence more burrs

BobWarfield
11-15-2009, 01:37 PM
wtf is a G wizard?

here's the M Wizard; rpm = CS * 4/ Dia = 100 * 4 / .75 = 500 rpm. you're fine where you are, faster will just wear the cutter out sooner.

19 ipm? in steel? my full sized XLO doesn't have a feed even half of that....feed rate has to take into account the machines removal rate capabilities. that's over 006 chip load - i thought 6 ipm was aggressive.

a chip is formed along a shear plane ahead of the tool. There's a fair bit of metal deformation happening at that point - when it gets to the edge some of this deformation happens below the plane of the cut which creates the burr. To reduce/eliminate, you've need to reduce the extent of the deformation of the metal - lighter cut or sharper tool for example.

Mills throw up burrs, knock them off with a file.

And WTF is an M-Wizard? LOL

100 SFM is slow for HSS, slower still for a coated cutter and a very light cut. Don't take my word for it, check Niagara's recommendations:

http://www.niagaracutter.com/techinfo/common_mat/1020.html

OSG and many others will give you similar numbers.

G-Wizard likes 176 SFM.

Your M-Wizard's chipload numbers are wrong, because you're chip thinning. Any time you cut less than 1/2 your cutter's diameter, the chipload is less. There are formulas that determine all that, and they will tell you that to actually produce the recommended chipload at a lighter cut you have to feed faster. In this case, yes I have cut steel at such feedrates. It works great, and is very quiet. In fact, I've cut steel at over 30 IPM without even making the cutter hot and without flood coolant.

It didn't leave a noticeable burr either, when I was doing it. Surface finish was great and the mill was quiet and nearly vibration free. Ah, the wonders of chip thinning. It's a concept invented for high speed machining that works great at the low speeds even small mills are capable of. I'll try to take a video next time I'm making such a run.

Here's another interesting factoid that you can easily discover with a little research: ignoring chip thinning and cutting too fine a chip will shorten cutter life just as surely as too many SFM. Why? Because when everything is working right, the chip carries away most of the heat. Too light a chip and it can't carry away the heat.

Now you can ignore all of that, a lot of folks do, I'm guessing you're one of those folks McGyver. Good for you, you have many fine projects to show for it, so stick with your M-Wizard.

Or, you can try to calculate all that stuff for yourself. By the time you add in all the various kinds of compensation that are even shown on that Niagara page, and then add chip thinning, compensation for lead angle, ballnose comp, and so on, it gets pretty crazy.

Hence a piece of software can keep up with it all instead. So in answer to your first question, G-Wizard is that piece of software that I've written.

Cheers,

BW

Mcgyver
11-15-2009, 02:05 PM
the M wizard was joke, intent on drawing your attention to how someone with a bit of machining experience approaches a simple situation. I get it that beginners tend to rely too much on G- Izmos but with some experience comes the the sense of when to move forward and when to get the calculator out....hardly an observation that categorizes me as being ignorant or ignoring of theory.

The OP's talking about facing some 5/16 mild steel ends...you're going to start calculating feeds to deal with chip thinning? whatever.


G-Wizard likes 176 SFM.


G wizard knows not of which it speaks. Not what I'd recommend for home shop guy who wants to maximize tool life and probably isn't running a 100k new mill, buy hey maybe you're used to advising professional machinists and such.....btw how does your feed/speed recommendation reduce burrs?

BobWarfield
11-15-2009, 03:36 PM
Well McGyver, with due respect, we'll have to agree to disagree. G-Wizard does know whereof it speaks as do the various manufacturer's whose recommendations are incorporated into its workings.

As for getting the calculator out, its more trivial than running your "M-Wizard". It's whole point is I no longer have to worry about all the calculations, I can just punch it up in the software and it gives me the right numbers.

You can see how that works on this page:

http://www.cnccookbook.com/CCGWizard.html

Or not. Far be it from me to push anything on anyone who is not interested!

Here is the aforementioned video of steel being cut at 30 IPM/800 rpm spindle speed:

http://www.youtube.com/watch?v=EFUnV_MCV7o

Now that's not on a $100K mill, that's on an RF-45 bench mill. It's actually a very easy cut for a light machine to make, about 0.16 HP (again calculated by G-Wizard). HP is not a bad way to evaluate whether you're getting too carried away for what your mill can take (or you setup at some point!).

The gearhead makes more noise than the cut. When it was done, the workpiece and the cutter were cool to touch. The smoke you see is heat from chips burning off a little WD-40 I sprayed on before I started the run. Radial depth of cut is 30 thou. Axial DOC is one tool diameter = 0.5" Tool life is great, hours and hours on cuts like this.

BTW, this was half the max chipload, so I could have fed it quite a bit faster still.

RE the burrs, do you see a 1-2mm burr like the OP is trying to get rid of anywhere in sight in that video? The edges on the workpiece were sharp and need a light file touch (or a chamfer run with the CNC), but the burrs were minimal.

Nothing special about the endmill. It's not even coated, just a vanilla US-Made HSS 4 flute. It's not even recently sharpened.

Proper feeds and speeds make for better surface finish and tool life. It's harder to get them just right than you'd think, and it also makes more of a difference than you'd think.

It's also nice when things go a little faster to boot.

Cheers,

BW

Carld
11-15-2009, 03:49 PM
I doubt Black Moons is using a CNC mill.

In his hand he held the smitlet with which he gaunted his antagonizer :eek: , or something like that. Anyway the war is on.

I have popcorn and a highball of Vodka and Coke. Carry on fella's. ;)

Mcgyver
11-15-2009, 04:02 PM
I have popcorn and a highball of Vodka and Coke. Carry on fella's. ;)

haha, i'm done, I've got 3 teenagers so I know when to walk away :D

beanbag
11-15-2009, 05:13 PM
I made a very similar cut a few days ago, using 13/32 4 flute HSS TiN coated end mill on 1/2" hot rolled, flood coolant. No burrs.

I suspect three problems in your case:
1) That end mill is dull
2) Even if it weren't, your ipm is a bit on the low side
3) Even if it weren't, you are using a really big end mill, which "wants" larger chip load, but large chip loads generate large forces, which might bend your setup a bit anyway. Try a smaller end mill.

lane
11-15-2009, 05:42 PM
Well I have never cut any thing with out some kind of a bur .Large are small . I just grab a file and off it goes.

Carld
11-15-2009, 07:37 PM
Well, I don't really want to call those that say they can use an endmill to face the end of a flat bar and not have burrs a liar but----I DON'T BELIEVE YOU. Any time you make a cut with a cutting tool or drill a hole or tap a hole there will be burrs. I started doing machine work about 1962 and I have never seen a machined edge that did not need to be deburred. In fact most professional drawings that I have worked from have a notation, "Break all edges" and that means, remove the burrs.

I have gotten a lot of cuts from those non existent burrs of which you talk. Even if you can't see the burr it exists.

Black_Moons
11-15-2009, 07:42 PM
beanbag wins, I'll try a smaller/fresh endmill, maybe at higher IPM.

Blah blah 'no burrs', we all (hopefuly) know he means blatently visable burrs. on aluminum most of my cuts leave such fine burrs that a normal sheet of paper can be used to brake them, thats what id love to see on my mild steel, insted of 1~2mm burrs that look like it came outta my abrasive chop saw.

tattoomike68
11-15-2009, 08:22 PM
Hi, im side milling the ends of some cold rolled bar (5/16") with a 3/4" 4 flute TiN coated endmill at 500rpm with cutting lube at 6IPM, 0.05 or so width of cut, and wondering why I often get a giant burr on the end of my cut? Any way to minimize that? Should I be using a smaller endmill? A better non chinese endmill?

The bar is supported within 1/4" of the cut by a custom made split collar block in my vise, so I suspect its supported well enough for the cut.

buy a nice belt sander. its like owning a truck once you have one you dont want to be without one.

Any excuse to buy a new tool.:D

J Tiers
11-15-2009, 10:00 PM
It's really downright SIMPLE.....

Up until you get to the end of the cut, the metal is backed up by MORE metal. You push on it as you cut, and it is rigid.

When you get to the end of the cut, there IS no more metal, so for the last bit the cutting force stresses it more than its yield point, and it bends over as a burr.

I think it is impossible to have no burrs.

I think it IS possible to have very small burrs.

if you spin the cutter very fast, the mass of the last bit holds it in position long enough to get cut fairly clean, so the yield strength never comes up. better have some HP behind it, because that might be REALLY fast.

Kinda like slowing the feed / lessening the feed pressure when the drill is about ready to break through.... that minimizes burrs also.

A sharp cutter has less force in cutting, so it forms less of a burr. That works with drills just like the feed trick.

Black_Moons
11-15-2009, 10:28 PM
a smaller (fresh) cutter helped somewhat, as does climb cutting, but the burr is still there, I think the main problem is that its a small diamiter round object, so when it gets to the end theres just a little point of material, not even a flat edge like milling a block, also this is mild steel so...

IPM did'nt seem to make that big of a diffrence, other then at high IPM the cutting fluid would start smoking.

Deburring it with my handheld air belt sander is easy even though the part is barly big enough to hold with my fingers (little belt sander with 180+ grit belts hardly even affects the fingers if I slip), I was just wondering if there where ways to minimize it.

tattoomike68
11-15-2009, 11:07 PM
a smaller (fresh) cutter helped somewhat, as does climb cutting, but the burr is still there, I think the main problem is that its a small diamiter round object, so when it gets to the end theres just a little point of material, not even a flat edge like milling a block, also this is mild steel so...

IPM did'nt seem to make that big of a diffrence, other then at high IPM the cutting fluid would start smoking.

Deburring it with my handheld air belt sander is easy even though the part is barly big enough to hold with my fingers (little belt sander with 180+ grit belts hardly even affects the fingers if I slip), I was just wondering if there where ways to minimize it.

then make a milling fixture so the part is held in a way so the bur goes over the fixture and has no place to go but eaten by the cutter. Just like drilling a hole through 6 parts, just the last one gets a burr.

try ganging up the parts as many as you can and just the last one will have a big burr.

I hope that gives you an idea that helps.

J Tiers
11-16-2009, 12:10 AM
then make a milling fixture so the part is held in a way so the bur goes over the fixture and has no place to go but eaten by the cutter. Just like drilling a hole through 6 parts, just the last one gets a burr.


That's an interesting idea.

Would you make the fixture with a sacrificial edge so that the first set would include a trim-down of the fixture? Seems like that might be a plan.

Would be easier than trying to set it perfectly....

Black_Moons
11-16-2009, 03:00 AM
actualy I was using a fixture but protrudeing it, Would I have to cut the fixture every time or just skim it?

beanbag
11-16-2009, 03:53 AM
Here's another idea: Is your rod sticking out too much and vibrating? (har har) What I would use as a fixture is to take a 1/2" square of Al, and drill a 5/16 hole in it. Then cut a slit from the side into the hole, and now you can clamp the rod from all sides.

I try to use climb milling as much as possible.

If the rod is not securely fastened, the cutting forces will tend the pull the rod up. When that happens, it bends away from the cutter, creating a larger burr.

One other thing you can try is to not do a full DOC, but rather 2/3 or 1/2 of the way. That way, you have a little ledge below the end mill that prevents the work from being pulled up. For the second full depth pass, there's no chance for a burr to form.

Carld
11-16-2009, 10:52 AM
Any time you machine a material there will be a burr. It is a given, there is no way to get around it. You can diminish a burr but you can't eliminate them.

While you may not see the burr it is there, go look at it under a magnifying glass. There is a reason why prints will say break all edges and sometimes they may say remove burrs and leave square edge. It all depends on the use of the work.

A good machinist will use a file or stone to remove the burrs. The rest will turn out work with the burrs still on the work. It is the difference between a professional and an amateur. A professional machinist doesn't complain about a burr on his work, he removes it and carries on.

I have long wondered how many CNC operators remove burrs or just toss the part in the finished bin.

To me it's a quality of workmanship to clean the parts before shipment. If there is a burr the work is not finished.

When you sharpen your knife on a stone there is a burr on the edge of the blade and for that reason the blade is stropped to remove the burr.

All machining operations produce a burr, just remove it.

Evan
11-16-2009, 02:37 PM
Any time you machine a material there will be a burr.

Not so Carl, at least not one that is significant.

For example, and there is no difference between this and side milling:

http://metalshopborealis.ca/pics3/hmillcut1.jpg

I have some cheap Chinese endmills that do leave a burr. I have some high quality solid carbide cutters that never leave a burr. Machine rigidity also plays a part but burrs, especially "a giant burr" are not inevitable and I don't expect to have to do a lot of deburring. Break the edge, yes. If I see a significant burr I know something is wrong, usually with the cutter.

Mcgyver
11-16-2009, 03:09 PM
Not so Carl, at least not one that is significant.



Oh come on.... you quote only the the first half of his line, tell him he's wrong yet proceed to say essentially the same thing.... he said



Any time you machine a material there will be a burr. It is a given, there is no way to get around it. You can diminish a burr but you can't eliminate them.

he didn't say a burr had to be significant, he said there will be one. How is his statement I correctly quoted above "not so" What, it's only "so" if you state it?

Evan
11-16-2009, 03:24 PM
There is no visible burr on the image above. That is what I mean by significant, visible. I used the qualifier because I knew somebody would try to pick a nit. The OP is talking about a "Giant burr".

Everyone is telling him to expect burrs. I don't expect burrs like that and neither should he. [added] I will also point out that there isn't necessarily an invisible burr either. The material will shear cleanly with a sharp edge.

Mcgyver
11-16-2009, 03:35 PM
There is no visible burr on the image above. That is what I mean by significant, visible. I used the qualifier because I knew somebody would try to pick a nit. The OP is talking about a "Giant burr".

Everyone is telling him to expect burrs. I don't expect burrs like that and neither should he.

...and that's fine, you have the worlds hardest floor and your cutters don't leave burrs.....my objection was to you telling someone they were wrong when you misquoted them and in fact your statement didn't contradict theirs.

and what is giant burr? height or width of where attaches? I'll often get a bur 1/2" or more high but it'll break off with finger pressure....otoh, if you've ploughed up a furrow over the edge that only an angle grinder will remove, well, something is wrong. I don't consider the former much of a burr or a problem, the latter, yes it is a cutter problem.

bottom line, Carl is right, there will be a burr. even if there was no discernable burr, its still proper practice to break a sharp edge. Using a sharp tool they'll be minimal, but the edge should still be cleaned (minuscule chamfer) with a file

Evan
11-16-2009, 03:40 PM
I believe I did mention breaking the edge.

I apologize to Carl, he isn't wrong. The impression he gives is misleading though. One should not always expect burrs that are a problem and in fact when they occur they signify that something isn't right in most cases.

Carld
11-16-2009, 04:10 PM
All I was saying was that you can expect some big burrs and always a razor edged burr that will cut you if not removed. It's just the nature of the machining process.

beanbag
11-17-2009, 04:57 AM
Here's a picture of the cut I was talking about. Inside the rectangle is a very very small burr. To the right of that there pretty much is no burr.

http://i139.photobucket.com/albums/q286/beanbag137/IMG_0276.jpg

I wouldn't be surprised if in some materials, under the right condition of sfm and chip load, the chip snaps off and doesn't leave any kind of burr at all.

Macor leaves no burrs, not even microscopic. ;)

BobWarfield
11-17-2009, 11:34 AM
ROFL.

And I used the term "noticeable" in my description as well, but it didn't stop Carl from calling me a liar.

Honestly, if you're going to conduct these threads at that level, Evan is entirely justified in exactly what he is saying and shouldn't be nitpicked. You've now got a video and Evan's photo with "no noticeable burrs."

Personally, I think Tatoomike had the best and most constructive answer yet, but of course he does this stuff for a living.

There are, BTW, ways of setting up the machines to eliminate the burrs. Go research it. It can't be done in all cases, but you can certainly minimize the burrs in all sorts of ways. Lots of the CNC intentionally program various moves of their machines exactly for that purpose.

If you do have a CNC, it's also very easy to make a chamfering pass to eliminate the burrs.

Now here comes the HSM nitpicking gang to complain that this isn't CNC, the burrs are still there, yada yada.

Whatever.

Cheers,

BW

Black_Moons
11-17-2009, 12:16 PM
Actualy I did exactly this, but used a 1"~ square block that I had cutoff from some scrap in my bin. I use a 0.01" feeler gage on the side with the slit to insure its clamped correctly to 'close' on the work peice (ie so the part isent clamped parallel but at a tiny angle to close the gap)


Here's another idea: Is your rod sticking out too much and vibrating? (har har) What I would use as a fixture is to take a 1/2" square of Al, and drill a 5/16 hole in it. Then cut a slit from the side into the hole, and now you can clamp the rod from all sides.

Carld
11-17-2009, 01:20 PM
:eek: Liar, Bob that Carld should be ashamed of himself. Uh, wait, that's me :o . Well I'm sorry if I missed the "noticeable" part.

In a mill the burr is relative to the action of the endmill. Many times there will be little if any burr on the underside of the work when undercutting because the helix will pull the material up. If climb cutting the burr may be on the bottom of the work. There will be a fine burr on the start of a cut when climb or undercutting. Likewise, an under cut will end with a burr and a climb cut may end with little or no burr.

A lot depends on the sharpness of the cutter and the material and the speed and feed. The reason I see this is I deburr all my work so I see where the burrs occur. Others observations may be different but that is what I see.

I don't fret over it, I just deburr the work as needed, it's part of the job.