[popspipes]

I have had problems with chamfer mills and engravers leaving a wire edge on the top of the part, this isnt a real problem as long as the tool is very sharp it will remove easily, as the cutting edge deteriorates it gets progressively harder to remove. I hand ground a 2 flute .250 endmill to approximate a 45 degree chamfer on the corners of the mill, this seems to work very well using the flute geometry of the cutter (no 90 degree rake angle at the cutting edge), no detectable wire edge is left on the top of the part at least in this trial.

I always used a file or other means when manual machining to remove the edges, with cnc its a time consuming problem for me.

Most chamfer mills comercially available that I have seen have the 90 degree rake angle ground on the cutting edge, this makes the edge more durable but it doesnt cut quite as well and leaves a small burr on top of the part.

The question is, is there a chamfer mill available that addresses this problem?

Thanks

[SCzEngrgGroup]

I do all my chamfers with carbide 90-degree 2-flute spotting drills. They leave a perfectly sharp, clean edge, and seem to last forever - I've got one I've been using for years.

Regards,
Ray L.

[R.DesJardin]

I use carbide 2 and 4 flute chamfer mills quite a bit. I have never had the issue with a bur on the part edge in aluminum of steel. This may just be a feed and speed issue and could be resolved with some playing around.

[popspipes]

I use carbide 2 and 4 flute chamfer mills quite a bit. I have never had the issue with a bur on the part edge in aluminum of steel. This may just be a feed and speed issue and could be resolved with some playing around.

Thanks for the input, I think I am too picky, the burr isnt really visible in most cases but it isnt as smooth an edge as the lower one.

The engravers are one flute and work better at 5 ipm 5140 rpm they are .125 diameter. I am limited in rpm to the Tormach spindle, at least for now.
You are correct as the feedrate increases the burr does become larger.

I am having the burr problem on steel as well with the engravers. They are cheap and questionable origin, that may be the problem there......

thanks

[Hirudin]

What feed and speed are you guys using? Also, at what effective diameter are you entering the material?

I use a 1/4" 4-flute chamfer mill as well*. 6000 RPM at 457.2 mm/m (18 IPM) and I usually put the chamfer mill down as deep as possible (~6 mm effective diameter). These chamfers come out looking good in my opinion. I'm assuming 5000 RPM at 15 IPM would work just as well.

* this one: 1/4" Drill Mill 4 Flute 90 Deg.

[AUSTINMACHINING]

I do a lot of 82 degree flat head fastener holes. I use the same tool for debur/chamfer. I've been using a Lakeshore Carbide 82 Deg. spot drill 20 IPM @6000 rpm with good results. Very sharp and seems to stay sharp. Might be my oldest tool. All the tools I've used from them have been very nice, especially the 3flute ZRN coated tools in aluminum. They are expensive and hard to justify in most cases, but they leave an incredible finish IF you need it (like an air tight gasket seal).

[SCzEngrgGroup]

The engravers are one flute and work better at 5 ipm 5140 rpm they are .125 diameter. I am limited in rpm to the Tormach spindle, at least for now.
You are correct as the feedrate increases the burr does become larger.

Those MUST be very poor quality tools. When you get some good ones, run them MUCH faster. On aluminum, you should be up around 20-30 IPM at 5000 RPM. At 5 IPM, I would not expect a good result with any tool The fact that going faster gives you a worse result says loud and clear those things are NOT sharp.

Regards,
Ray L.

[popspipes]

I do a lot of 82 degree flat head fastener holes. I use the same tool for debur/chamfer. I've been using a Lakeshore Carbide 82 Deg. spot drill 20 IPM @6000 rpm with good results. Very sharp and seems to stay sharp. Might be my oldest tool. All the tools I've used from them have been very nice, especially the 3flute ZRN coated tools in aluminum. They are expensive and hard to justify in most cases, but they leave an incredible finish IF you need it (like an air tight gasket seal).

I tried the spotting drills, they work fine, the angle of the grind is 60 degrees but for a small chamfer that is OK.

[SCzEngrgGroup]

You can get 90-degree spotting drills as well. That's what I use.

Regards,
Ray L.

[BIG IGG]

I use a 90 deg spotting drill as well. Works pretty good

[CadRhino]

My spotting drills are all 120 degree but my countersink tools are 82 deg and my chamfering tools are 90 deg so I might try those. Thanks for the suggestions.

[cobrakai]

I am using a tiny little 1/4" carbide 2ftl chamfer tool. Doesn't leave a burr at all. I think I was running it at 5000RPM 15ipm. The thing you have to factor in is that the effective diameter is maybe 1/16" at the bottom and 1/8 at the top due to the angle. Calculate your feedrates based on the contact height of your tool. I usually shoot for the maximum but due to clearance sometimes only get .025" of height. This means the tool has to move somewhat slowly.

But yeah... if you're getting burrs, get a new tool.

[popspipes]

I am thinking that a spotting drill as suggested above as it has a shallower rake angle at the cuttig edge and should cut a bit smoother.

[mountaindew]

The thing you have to factor in is that the effective diameter. Calculate your feedrates based on the contact height of your tool.

Good point!
Added this to my notes and edited my master tool crib defaults.


I also use a 1/4" carbide 2flt chamfer tool at around 4500rpm 12imp " one of the most used tools in the crib"
I tend to design and mill a .02 chamfer on every edge I can. "looks good on paper at mill and finished part"
Most the time I get good results and end up with nice clean parts.