Need Help!- Countersink Problem on CNC

[Terry G]

I've been CNC machining for about 8 years on a Taig mill. I keep the mill tight and service it regularly and it has done great and continues to do so over the years.

I recently started making a part out of 6061 aluminum that requires 4 countersink holes and another part that requires two countersink holes and 2 countersink slots.

The holes and slots are for an M3x.5 screw. I am using 1/4" 6 flute 90deg countersinks. I'm running these bits at about 800 rpm and feeding it at 2 ipm, so I'm taking a very light cut. The material is 0.120" thick aluminum and I pilot drill an 1/8" hole before countersinking. I'm running the countersink .110" deep using mist coolant.

I started making these countersinks with a HSS 1/4" 6 flute countersink that I had laying around for quite a while. After about a dozen parts that came out great, it started to gum up on me and destroying the parts. It would just push away the aluminum instead of cut it.

Thinking my old bit was just old, I purchased a new HSS 1/4" 6 flute countersink and it worked excellent for about 20 to 30 parts (4 holes each and some slots). Then it also started to gum up on me and destroy parts.

I ordered some solid carbide 1/4" 6flt countersinks thinking those should last a long time. Well, first time I used it, it would not even countersink a single hole without 'smearing' the aluminum and destroying the part. I took the 2nd brand new carbide bit and it did the same thing. Basically leaving a large burr around the top edge of the hole, and closing the 1/8" hole on the bottom to about 1/2 the size.

Any suggestions to things I may be doing wrong? I don't understand why the HSS bits work great with these exact machining parameters, but wear out after 100 holes, and the new equivalent carbide bits don't work at all.

I also tried pecking at the countersink hole with .040" cuts, increasing my feed and decreasing my feed, but nothing seems to make a difference with the carbide bits. It continues to smear the aluminum.

I have my jig loaded waiting for this next step. I'll probably just go buy another HSS bit to get through these next dozen parts I need and hope it lasts. But I really wish I could figure out what I'm doing wrong.

If I left any important info out, please let me know.

Thank You.

Terry

[christinandavid]

Try a 2-fluter for better swarf evacuation, and mill in XY rather than peck in Z wherever you can.

DP

[Terry G]

Thanks, I'll try a 2 flute and see how it works.

I understand what you are saying about XY milling, but due to the backlash in my mill I would not get a nice even countersink with the pilot hole perfectly centered. So I have to plunge the whole cut.

I guess the biggest frustration is why these brand new carbide countersink bits won't even cut a single clean hole? At least the HSS one lasted 100 holes or so.

Another question, when determining the RPM, I have read that you should use the largest diam. of the countersink (.250") to calculate your feed, then cut the RPM by 1/3. The one thing I don't understand is how the number of flutes come into play? The 'Drill' formulas don't seem to take that into account like the 'Mill' formulas.

I'm using 150 SFM, .250" dia., and a feed (ipr) of .001" which gives me 2400rpm at 2.4ipm. I take one third the RPM and run the countersink at 800rpm and 2.4ipm to my depth. I'm taking light cuts due to my small mill not being so rigid.

This was at least a good starting point, and had been working great for me with the HSS bits so I stuck with it. Maybe I need to change some parameters with the solid carbide bits.

Thanks.

[juergenwt]

Terry- Just use a HSS drill sharpened at 90 deg. If you have a high spiral drill - even better.

[Geof]

1/4" 6flt countersinks

6flt, that is your basic problem; the space between the fluts is small so there is nowhere for the chips to go so they tend to pack up and fill the flutes.

You were lucky with the HSS which probably worked when they were new and very sharp because the chip peeled off as a nice clean thin wafer and could clear out of the flute. As the tool dulls the chip tends to get thicker because the metal is being pushed off rather than sheared off; the thicker chips simply jammed up.

Carbide tools do not have the nice sharp cutting edge that is possible with HSS so your new carbide cutter behaved simiular to a slightly dull HSS cutter.

A two or single flute countersink should see you fine.

One other thing: Are you using coolant/lubricant? You should be to allow the chips to flow freely across the cutting edge. Actually with good lubricant such as tapping lubricant even the six flute cutters may work okay.

[Terry G]

Never thought of that. I'll have to take one of my old 1/4" drill bits and do exactly that.

I also stopped by my friends machine shop and he gave me a solid carbide 2 flute countersink cutter to try. I guess it is not technically a countersink, but he said it should work.

I showed him the 6 flute carbide cutters I just bought and he said he has never had any luck using that style cutter on aluminum. I guess that answers my question.

Thanks.

Terry

[Terry G]

Originally Posted by Geof 1/4" 6flt countersinks 6flt, that is your basic problem; the space between the fluts is small so there is nowhere for the chips to go so they tend to pack up and fill the flutes. You were lucky with the HSS which probably worked when they were new and very sharp because the chip peeled off as a nice clean thin wafer and could clear out of the flute. As the tool dulls the chip tends to get thicker because the metal is being pushed off rather than sheared off; the thicker chips simply jammed up. Carbide tools do not have the nice sharp cutting edge that is possible with HSS so your new carbide cutter behaved simiular to a slightly dull HSS cutter. A two or single flute countersink should see you fine. One other thing: Are you using coolant/lubricant? You should be to allow the chips to flow freely across the cutting edge. Actually with good lubricant such as tapping lubricant even the six flute cutters may work okay.

Thanks, this is a great explanation and is exactly what I am seeing. I did not know that about carbide bits.

I am using mist coolant. Basically when the cutter hits the material, it is pretty much flooded since I am countersinking into somewhat of a pocket. The tool stays very cool with the strong mist.

I do use cutting fluid occasionally on holes through thin material. Would it be enough to just fill the hole with a few drops of cutting fluid and let the cutter plunge?

I'll try all these great ideas.

Thanks,

Terry

[keebler303]

If it's more about the finish than the speed, I have the best luck using "zero" flute countersinks at 1-200 RPM. Just be careful not to feed it too fast as they don't have too much clearance.

Matt

[Geof]

Originally Posted by Terry G Never thought of that. I'll have to take one of my old 1/4" drill bits and do exactly that.... Terry

Try it on some scrap first, it will almost certainly chatter and grab and make a mess.

Countersinks have very little clearance back from the cutting edge and they have little, if any rake, so they tend to rub and stabilize so they do not chatter or grab into the metal.

A drill sharpened to act as a countersink does have significake on the cutting edge because of the helix, also it is difficult to sharpen them with minimal clearance so they tend to chatter and grab.

[Terry G]

Thank you everyone for the great tips. I drilled about 20 holes in the same material I'm working with a did a bunch of testing. I found that the old worn out 2 flute carbide bit that my buddy gave me today worked excellent!

I guess it was the number of flutes I was using, and getting lucky with the new HSS bits for the first 100 holes or so.

I just ran the 2 flute 90 deg chamfer bit at about 2000rpm, and fit it really slow and it came out real nice. No burr, and the aluminum was actually being cut. Finish was better than I expected for the beat up bit.

I'll be purchasing a new 2 flute actual countersink bit now and should have even better results based on my testing.

Thanks again, it is really great to have support on here. I've been fighting this for a few weeks now and I hope it is over with!

Terry

[juergenwt]

Terry - Geof is right when he tells you to try it on a scrap part first. If sharpened correctly you should not have a problem. In my life time I have hand sharpened hundreds of drills for 90 deg or 82 deg. c'sink and done thousands of holes in all kinds of materials. It does not take very long to get the drill to cut right and most of all it does not cost you anything.
But one thing I always do is use a drill approx. 0.1 mm larger than the top of the screw and than go with the full dia. just about 0.1mm below the surface. Makes for nice just below the surface fit. Also-unless you have a print that gives you the dia. for the c.sink make sure you know the type of screw that is being used. It would help if you can get a DIN or ISO number. Standard M3 Hexagon Socket Countersunk Head Screw will use a 6mm c'sink (5.3/5.6) for DIN 7991. But there are some others on the market and if you are making a lot of parts - double check.

[Terry G]

Thanks for the tips on the drill bits. I will be using the 2 flt chamfer bits for now since it seems to be working great.

I'm specifically doing 3mm 90deg machine screws right now. I don't have much experience hand sharpening drill bits, but do use a drill doctor to keep all my bits sharp.

Have done some grinding on HSS for the lathe and made a nice puckered, but that's about it for now.

Thanks again for all the great info. I will always remember these tips to get me going next time I get stuck.

Terry