CNC boring aluminum prob

I have to make a whole lot of 0.177" holes 0.6" into aluminum. I have a 2-fl 1/8" carbide endmill and a single-flute 1/8" carbide and a Taig mill, which I'm trying to use at 10K RPM although I did bump it down a speed which makes it maybe 7K or so. The bit has a cutting length of 0.375" (the actual flute length is a bit larger). I don't have coolant or an air blaster. I have reasons not to want to use a drill bit, partly because I'd just like to know how to do this with a mill for similar but noncylindrical bores which couldn't be done with a drill. The single flute so far has shown to be far superior, but still not successful.

I keep clogging the bit here once I exceed the cutting length, no matter which way I went. In some cases the aluminum welded itself into the carbide flutes and couldn't be removed, already destroyed a number of bits.
* CW or CCW helical bore, 0.1" steps. Since the width of the hole is less than 2x the bit diameter, it's possible to do this, except no, it clogs once it gets deep in past the cutting length. Also welds crud all over the walls.
* Step down in center, move to the side, do a flat circle- same problem basically.
* Peck the center all the way down, then go back to the top and helical down to enlarge it. The idea being that the prior helical boring attempt was just pushing chips around in the hole, but the peck gives no room for chips to avoid getting lifted out when it withdraws. It was a nice theory! But what was happening here is that as the pecks get deep, the chips tend to stick on the flutes and fail to throw off when the bit withdraws to the top, defeating the point of pecking. Still ended up with crud lightly welded to the walls of the hole, too.

Any ideas on how to run this operation with this bit?

can you back relieve the cutter

Yeah. #1 - Put an air blast on it (or mist coolant). #2 - Do not step down in cutting more than 3 degree angle or 1/2 of diameter. #3 - Once you reach full flute length, you will have to do full retract before next cutting to allow chips to escape hole. #4 - Full retract also helps allow time for tool and material to cool slightly before next cutting.

Quote:

---

Originally Posted by nash398

can you back relieve the cutter

---

I am unfamiliar with this term, plz explain.

Quote:

---

Originally Posted by txcncman

Yeah. #1 - Put an air blast on it (or mist coolant). #2 - Do not step down in cutting more than 3 degree angle or 1/2 of diameter. #3 - Once you reach full flute length, you will have to do full retract before next cutting to allow chips to escape hole. #4 - Full retract also helps allow time for tool and material to cool slightly before next cutting.

---

#2 I did limit the step quite a bit, but it didn't resolve the problem, even when less than 1/2D.
#3 That didn't work. Chips tended to stick in the flutes. I'm wondering if I should plunge FASTER not slower though, I think the slow plunge (3-5 ipm) at the end of the peck is grinding up aluminum into a powder that forms a concretion in the flutes too easily.
#4 Didn't seem to have a heat problem. After the cycle ended and it shut down, the bit and material in the flutes wasn't even warm.

Straight plunge? You need to ramp. I have a Taig too, and I do 3D aluminum work with it, but I am turning 27000 rpm, and using multiple nozzle flood oil lubricant/coolant.

(Not with the stock Taig spindle. LOL)

I struggled with dry cutting aluminum with my Taig and stock spindle. I could do a little better with some coated (ZRN or tialn), but if I got very aggressive at all it would still chip weld. I also got much better results with larger cutters. 1/4" and bigger coated seem to work pretty well within their speed feed range. An air blast will help, but its not as good as a flood coolant.

You also have to remember you have a skinny little V-belt and a limited horsepower motor. You can bog the motor. If you bog the motor the belt will just slip.

I'm currently running a 1 3/4 HP router as my spindle.

P.S. I may sell my Taig soon. I've got tens of thousands of hours on it, and I am ready for a real high speed spindle machine.

Quote:

---

Originally Posted by Bob La Londe

Straight plunge? You need to ramp. I have a Taig too, and I do 3D aluminum work with it, but I am turning 27000 rpm, and using multiple nozzle flood oil lubricant/coolant.

(Not with the stock Taig spindle. LOL)

I struggled with dry cutting aluminum with my Taig and stock spindle. I could do a little better with some coated (ZRN or tialn), but if I got very aggressive at all it would still chip weld. I also got much better results with larger cutters. 1/4" and bigger coated seem to work pretty well within their speed feed range. An air blast will help, but its not as good as a flood coolant.

You also have to remember you have a skinny little V-belt and a limited horsepower motor. You can bog the motor. If you bog the motor the belt will just slip.

I'm currently running a 1 3/4 HP router as my spindle.

P.S. I may sell my Taig soon. I've got tens of thousands of hours on it, and I am ready for a real high speed spindle machine.

---

Good lord, how did you get a Taig to 27,000 RPM?? Got docs on what you did?

I thought of speeding up the spindle, but then investigating the bearings and found I really couldn't get bearings rated for much high speeds in that size. Even ceramic was limited to 12,000 RPM IIRC. So yeah, if it were to need to go faster, the spindle would have to be modified or replaced.

Yeah the belt slippage has come up, but in this case, the slippage seems to always be an effect of the bit getting clogged to begin with and unable to cut. It's not a cause and if anything, it is saving me.

The helical motion IS a ramp. Tried CW and CCW. At first it chews right in, but once it gets deep enough that we exceed the cutting length of the bit, things gum up the bit easily, and withdrawing doesn't seem to be of great help.

It probably wouldn't be a big deal if it were a LARGER hole, and give the chips more room to move away from the bit. But the current job is, it's a .125 bit in a .177 hole.

This one is a .125 ball nose doing mixed 3D carving at 34,000 rpm with a 1hp router.
[ame="http://www.youtube.com/watch?v=AuzzRYRdTV8"]The Square Back Minnow's Humble Beginnings - YouTube[/ame]

If I recall step over is about .003. Might be more as I was going to a lined or ridged look. My Taig spindle sits up on the shelf. I planned to turn it nto a 4 axis for lathe like operations one day. I just realize I haven't shot any video with the new bigger router.

Well, it is running better with the feedrate bumped up and the depth dropped down, but clogging is still a problem.

LOL more Mach3 number-bugging. I tried to adopt another helical path strategy and suddenly the Z-axis stalled, and it's limited to 30 ipm. I changed the feedrate for that operation to F15, it slowed down enough it didn't stall but it was clearly ignoring the axis limits and moving the Z WAY faster than the 30 ipm. The display read 70 ipm, and that lifting pass is mostly vertical. Then it showed toolpaths that weren't even in the run and not depicted via Regen Toolpath or Simulate Toolpath so basically it's hosed.

Mach3 is good with numbers MOST of the time. But there's certain things that irregularly cause major divide-by-zero sort of errors that you just hit at random that make it go berzerk. Playing with the A-axis can do it too.

You might consider pecking the end mill down, just like a deep hole drilling cycle. I usually start with 1st peck = diameter then reduce following pecks by 1/2 until I get to 1/8 diameter. No matter how you approach this, you have a chip removal problem. You are making more/large chips than you can get out of the hole fast enough. And you have a flute length problem that is making it worse. I am not going to tell you to switch to the correct hole making tool because you have already said you won't. There are just some laws of physics that stubbornness will not over come.

I run my router at 30000 rpm. I use 2 flute, 1/8 to smaller bits all the time.

I cut 6061 and some softer aluminum.

Things I've learned.

4 flutes, stay away for aluminum.
3 flutes, stay away from. They still gum up.

I blast air on my aluminum cutting and mist fluid when it's not clogged. Point is, if I don't run air to evacuate the chips, I'm gonna gum a bit, and if the bit don't break in time, the material is going to move.

If my material moves, then I'm screwed and won't get a good "do over". Hence, time wasted along with scrap material.

Even an air brush compressor can produce enough air to evacuate chips.

For that matter, try a spray bottle or even wd40. It's a whole lot cheaper then gumming up bits, scrapping material and just plain wasting time and electricity.

There you go. Clear the chips. Everybody agrees.

As to air compressers... I have seen what a $69 box autoparts store compressor can do. I think you need a "little" step up if you are going to use it as a continuous air supply for blowing chips. I have a roll around 20 gallon Cambell Hausfeld I bought 18 years ago that does ok though. Its about the smallest compressor I would use for doing real work, and it is more than upto the task of keeping a continuous air blast strong enough to blow chips clear.

If you get wind up with aluminum "welded" to the cutter, don't throw it out. Throw it my way. :-)

I'll just soak it in a lye solution (drano and water) for a day, and the aluminum will be gone.

Ken

I just drilled 32 .156" holes, using a .125" 2-flute endmill, to about .32" though mic-6 with no problems. A lot of it has to do with CAM. I used one of OneCNCs drill strategies, clean circle with zig-zag ramp in, going .04" per pass at 25IPM feed/13IPM plunge. Climb cut! And run a finish pass each rough depth, this will help the tool from deflecting toward the center as you go deeper.

Check here, post 104:
http://www.cnczone.com/forums/diy-cn..._router-4.html

After this was done, I decided to drill through the plate for more thread engagement. I used a 5/32" drill bit, and the milled hole guides the bit the rest of the way. Done on a drill press, peck drilling, with WD-40 lubricant. Lube tehe bit, not the hole. To attest to the accuracy of this method, I was able to attach the LM rails on the THROUGH side with the holes still lining up, so I know it's good to at least .005"...

You shoud use lubricant with aluminum. Not only will you prevent chip welding, but your endmills will last longer. In fact for these holes I do no chip clearing, but make sure I get lubricant on the bit during retract. Right now using Ashburn TD Foamy with success, but Pam High Heat works well!

... and I thought I was the only one silly enough to try cooking spray in a pinch. LOL.

Quote:

---

Originally Posted by Bob La Londe

... and I thought I was the only one silly enough to try cooking spray in a pinch. LOL.

---

Better still, it smells like breakfast!