On Small chamfering... Try a SK1S carbide burr...

snowshooze · Sep 30, 2020

Hi guys,
I do a lot of small chamfers, and often it is the slowest operation as I am limited to 4 flutes on these 1/4" chamfer mills.
So, I tried a SK1S carbide burr.
It has 16 teeth, and the 45 degree chamfers I am layng down are usually .005 to .010 depth.
I was programming .0015 IPT and just a bit rough, but ok.
With these, a comparable finish is .0007 IPT, BUT there are 16 teeth... so I have doubled my travel speed.
The carbide burrs aren't ground as well as our stuff is, but they are dirt cheap, this one I allowed about a .005" flat nose accounting for grind... seems about right.

Try it.

DanielG · Sep 30, 2020

A few manufacturers make higher flute count chamfer mills. I don't recall seeing eight flute, but Helical and Guhring make 5 and 6 flute options (respectively).

Delw · Sep 30, 2020

Ive tried burrs but they dont repeat and tended to run out a few thou. I use 6 flutter pointed solid carbide in 1/8" -1/4" shanks
also I havent had success with them cutting clean like and chamfer endmill

snowshooze · Sep 30, 2020

DanielG said:
A few manufacturers make higher flute count chamfer mills. I don't recall seeing eight flute, but Helical and Guhring make 5 and 6 flute options (respectively).

That helical looks good, I will try them.
But I have been trying to find as many flutes as I can, this burr gets me up to 90" per min, big help, but that Helical may do better.
Thanks!
Mark

Delw · Oct 1, 2020

snowshooze said:
That helical looks good, I will try them.
But I have been trying to find as many flutes as I can, this burr gets me up to 90" per min, big help, but that Helical may do better.
Thanks!
Mark

Mark does it give you a clean cut? with a 4-6 flute and 10k-12k I can go about 50 IPM on .050 dia(using a 1/8) and get a clean cut, granted I tumble the parts so I dont see any feed lines, at the same time I am only going .001-.002 deep so its mainly just rubbing the hard part of burr off in alum and tumbler doing the rest. 90+ inchs a min I would be really happy with.
I got mine through mc master to try there kyocera 6 flute points, make sure you look for the point ones as the others have a small flat on them.

wmpy · Oct 1, 2020

Harvey makes CNC burrs...

Deburring

Mike1974 · Oct 1, 2020

Delw said:
Mark does it give you a clean cut? with a 4-6 flute and 10k-12k I can go about 50 IPM on .050 dia(using a 1/8) and get a clean cut, granted I tumble the parts so I dont see any feed lines, at the same time I am only going .001-.002 deep so its mainly just rubbing the hard part of burr off in alum and tumbler doing the rest. 90+ inchs a min I would be really happy with.
I got mine through mc master to try there kyocera 6 flute points, make sure you look for the point ones as the others have a small flat on them.

Depending on your parts and/or any clearance issues, the flat shouldn't cause any problems if you have a good way to measure it. I check them on the microvu then alter the tool profile in Mastercam so it cuts the right size chamfer I programmed.

Finegrain · Oct 1, 2020

DanielG said:
A few manufacturers make higher flute count chamfer mills. I don't recall seeing eight flute, but Helical and Guhring make 5 and 6 flute options (respectively).

Harvey makes an 8-flute 3/8" 90* double-angle cutter (PN 838824) which is what I use whenever part geometry allows.

Regards.

Mike

Delw · Oct 1, 2020

Mike1974 said:
Depending on your parts and/or any clearance issues, the flat shouldn't cause any problems if you have a good way to measure it. I check them on the microvu then alter the tool profile in Mastercam so it cuts the right size chamfer I programmed.

Mike some of the flats are bigger than the width of the slots usually its the reason I need the pointy ones.

but sometimes you have a shallow depth where you need a flat so it doesnt hit the bottom we just grind those on the surface grinder.

snowshooze · Oct 2, 2020

Delw said:
Mark does it give you a clean cut? with a 4-6 flute and 10k-12k I can go about 50 IPM on .050 dia(using a 1/8) and get a clean cut, granted I tumble the parts so I dont see any feed lines, at the same time I am only going .001-.002 deep so its mainly just rubbing the hard part of burr off in alum and tumbler doing the rest. 90+ inchs a min I would be really happy with.
I got mine through mc master to try there kyocera 6 flute points, make sure you look for the point ones as the others have a small flat on them.

Well, smooth with a slight ripple. I am going ahead with it for now.
I had hoped for better feed rates, but the grind isn't up to snuff.
Still, looks pretty good and the speed is doubled.

For the point flat, I gauged off a 3/16 diameter bushing and found the height difference between a true sharp tip as opposed to the burr.

Mike1974 · Oct 2, 2020

It's alot more programming work, but you can deburr with small ball endmills as well (providing not trying to hit a chamfer number form print). Certainly doesn't make sense for small volume, but on repeat jobs with small features....

Delw · Oct 2, 2020

Mike1974 said:
It's alot more programming work, but you can deburr with small ball endmills as well (providing not trying to hit a chamfer number form print). Certainly doesn't make sense for small volume, but on repeat jobs with small features....

Mike
Can you explain this better. I was always curious on how. I have the idea what its doing but never tried it. on small .005 max rads we just need to knock burrs off . The tumbler makes it an even finish

I am guessing you just touch the edge in one straight line?

Mtndew · Oct 2, 2020

Delw said:
Mike
Can you explain this better. I was always curious on how. I have the idea what its doing but never tried it. on small .005 max rads we just need to knock burrs off . The tumbler makes it an even finish

I am guessing you just touch the edge in one straight line?

A good example is Mastercam's Deburr toolpath, it's super simple and quick.

Signature Part- Optical Mount Deburr - YouTube

Mike1974 · Oct 2, 2020

Delw said:
Mike
Can you explain this better. I was always curious on how. I have the idea what its doing but never tried it. on small .005 max rads we just need to knock burrs off . The tumbler makes it an even finish

I am guessing you just touch the edge in one straight line?

What I did was "lie" to the toolpath and tell it to leave negative stock in XY and Z. You have to fiddle with it depending on size of the ball endmill, and the features, and how close they are. Really lets you get in tight corners that you may not be able to reach with a traditional chamfer mill. The side/tangent of the ball then just touches, and actually creates a concave deburr profile, but we are talking teeny tiny, like .001-.002" *edge break*. I use contour toolpath in MCX, then adjust XYZ accordingly, and use the lead in/out to stretch or shrink the start/exit moves.

Mike1974 · Oct 2, 2020

Mtndew said:
A good example is Mastercam's Deburr toolpath, it's super simple and quick.

Signature Part- Optical Mount Deburr - YouTube

Holy crap!!! Badass! I have to do it the hard way.

Delw · Oct 2, 2020

Mtndew said:
A good example is Mastercam's Deburr toolpath, it's super simple and quick.

Signature Part- Optical Mount Deburr - YouTube

Mtndew
Thanks for that vid, that is as mike said BADASS its almost worth buying mastercam just for that feature. we spends tons of time deburing parts.

Mike1974 said:
What I did was "lie" to the toolpath and tell it to leave negative stock in XY and Z. You have to fiddle with it depending on size of the ball endmill, and the features, and how close they are. Really lets you get in tight corners that you may not be able to reach with a traditional chamfer mill. The side/tangent of the ball then just touches, and actually creates a concave deburr profile, but we are talking teeny tiny, like .001-.002" *edge break*. I use contour toolpath in MCX, then adjust XYZ accordingly, and use the lead in/out to stretch or shrink the start/exit moves.

Mike, Thanks Thats what I was thinking concaved. I'll have to give it a try and see how that works for us. I have an old cam system so its going to be that hard way like your doing I am guessing.
I got another batch of parts coming with the key holes/slots monday that ball would make it super nice. 60 parts take damn near 2.5 days and alot of cussing to deburr complete (tons of fins in them)

snowshooze · Oct 2, 2020

Mike1974 said:
It's alot more programming work, but you can deburr with small ball endmills as well (providing not trying to hit a chamfer number form print). Certainly doesn't make sense for small volume, but on repeat jobs with small features....

Awesome solution!
I love it. Ball or lollipop.
Just so easy.
Thank You!!!
Mark

Still having a problem getting enough teeth at Harvey tool. They have a 270 degree undercutting style, but the deburr is a diamond cut.
If they had left out all the left-hand cuts there would have been 15 remaining rights..
Still digging.

Mtndew · Oct 5, 2020

Mike1974 said:
Holy crap!!! Badass! I have to do it the hard way.

It really is badass. No guessing, no changing lead ins/outs etc... click the things you want deburred and you're done.

Mike1974 · Oct 5, 2020

Delw said:
Mtndew
Thanks for that vid, that is as mike said BADASS its almost worth buying mastercam just for that feature. we spends tons of time deburing parts.

Mike, Thanks Thats what I was thinking concaved. I'll have to give it a try and see how that works for us. I have an old cam system so its going to be that hard way like your doing I am guessing.
I got another batch of parts coming with the key holes/slots monday that ball would make it super nice. 60 parts take damn near 2.5 days and alot of cussing to deburr complete (tons of fins in them)

Yep! Exactly why I chased this down to "perfect" it. Did a part where one side had tons of ribs and such, the opposite side/op cut out cooling vents, like 20-30 on each end. No way I wanted to do all of that by hand! Still left with a chunk of hand deburring because the slots cut through a radius, but cut it down tremendously using the ball end mill.

D Dubeau · Oct 6, 2020

I've done deburring with a ball and lolipop a few times. Edgecam has a "slot" cycle that will drive a cutter from it's tip along any 3d path you create. A little bit of cad work provides me with the 3d path, and it runs a very efficient cycle. More work on my end, but I know that tool is going to follow that path exactly how I intended it. Pretty easy to make it stay down in pockets and move around without adding a hundred retracts too. Sucks if you want to change chamfer size though.... But it does work.

That Mastercam cycle looks pretty slick and would be WAY easier. Thankfully I don't do much production and only have to do my way maybe a few times a year. Wish I had Mastercam to play with instead though. Haven't used it since V9... A few days ago....

On Small chamfering... Try a SK1S carbide burr...

Stainless

Stainless

Stainless

Stainless

Stainless

Hot Rolled

Diamond

Diamond

Stainless

Stainless

Diamond

Stainless

Diamond

Diamond

Diamond

Stainless

Stainless

Diamond

Diamond

Hot Rolled

Similar threads