What should my aluminum swarf look like?

[guru_florida]

Wowee, another discussion of speeds and feeds!

The numbers are killing me. lol. I've already cut aluminum by playing with different speeds and feeds empirically. Now I am trying to nail down the formulas. The formulas aren't difficult but choosing the right numb3rs are, when considering the rigidity of the machine, cutter, material, etc.

Currently, my swarf is pretty small. I know this isn't ideal and my RPM is probably way to high and feed rate too low! (6500RPM)

I am using TAPMATIC Plus #2 (For Al), this stuff really helps cutting. I have an air swarf blower.

My spindle is a TAIG spindle, with a Rick Lane motor and speed controller. My machine is home made using ground ballscrews, NSK rails and 8020, it's pretty rigid/solid. Stepper amps are gecko G203Vs.

In the picture I used a 1/4" Cobalt Rough End Mill, 3 flute, TiN coated. Mat. Grade M42. This had the best material removal rate of the endmills I've used so far. Of course, a finish pass is required with a standard End Mill. I used a 12IPM feed rate and 5000RPM. It cut very smoothly and quietly, my wife didn't even hear it! I am sure I could increase the feed.

I would like to get comments on my swarf and your speed and feed numbers , machine details, etc.

[DeusExMachina]

Your swarf looks pretty good, but maybe a little small. I have a 3 flute carbide 1/4" end mill from SGS. Their recommended chipload/tooth is 0.0012 - 0.002 feed/tooth. I typically run my machine at 4300 rpm, and my feed at 22 ipm so thats a chipload of about 0.0016" per tooth and a DOC of about 0.025"-0.035", it cuts great and finish is extremely smooth.

Try to keep your chipload, close to your manufacturer's specifications and your tools will last sometime. I managed to burn up a niagra 3-flute 1/4" HSS roughing end mill because I was running it at 4300 rpm and about 8-12ipm, it only had about 40-60 hours cutting time on it before welding to a part -- afterwards I looked up the feed/speed from the manufacturer and realized what I had done to the poor thing heh.

[guru_florida]

I tried cutting a part today without any luck what-so-ever. I am starting to understand the speeds and feeds formulas. I am using a 0.002 in/tooth (0.006 in/rev) feed with a 270 SFM speed. This equals 4125 RPM and ~24 in/min feed rate. I started with a 0.2in DOC and moved down to 0.125 DOC. This is for a 3 flute rougher.

I couldn't come close to this feed. I started at 50% feed (so ~12 in/min) and it couldn't reach this before getting melted aluminum in the teeth. I think part of this is the lack of horsepower in my TAIG spindle and motor, I could see the bit complete stop occasionally.

Secondly, I think my rougher might be too dull from the last part but I am no where near an hour of cutting use. At 25$ a pop I would think the rougher would last longer!

I have included a pic of the rougher with the aluminum *jam* still on it. What causes this buildup to occur exactly? Of course, once this happens it no longer cuts so how do people setup a machine and walk away from it?

I also tried a 4 flute standard end mill, 0.07 in DOC with 11 in/min and 4200RPM with similar results, hardly get started before it's jamming.

Finally, the last thing I noticed is the part is deformed surely due to missed steps. I have 170oz.in. steppers on the X/Y axis, they are unipolar running half coil. Is this enough power?

I am a little suprised at todays efforts. The last part, pretty much the same. Ran at 12IPM, 5000RPM, .125 DOC and came out correct and without a problem....it almost seemed effortless to the machine.

Thanks,
C

[Hirudin]

For the most part, I've been following this feed and speed formula...
RPM = SFM × 12 ÷ π ÷ D
IPM = RPM × F × CL

D = tool diameter
π = pi (although it doesn't really look like it)
F = number of flutes
CL = chip load

It looks like this is the same formula you're using (that must be a 0.25" rougher right?)


If I find that the machine stalls (or something else bad happens) I will reduce the DOC. I usually keep my DOC at or under 0.040" (but I haven't really experimented with 0.25" end mills much, maybe they could go deeper than the 0.1875 cutters I've been using).

Based on my experience, 0.125 DOC is prolly too high (or "low" depending on how you look at it).

If 12 IPM with 0.125 DOC works fine maybe 24 IPM with 0.0625 DOC would work fine too. With twice the speed but half the DOC it would probably take the same amount of time, but you would be following the correct speeds and feeds.

[escott76]

I tried cutting a part today without any luck what-so-ever. I am starting to understand the speeds and feeds formulas. I am using a 0.002 in/tooth (0.006 in/rev) feed with a 270 SFM speed. This equals 4125 RPM and ~24 in/min feed rate. I started with a 0.2in DOC and moved down to 0.125 DOC. This is for a 3 flute rougher.

I couldn't come close to this feed. I started at 50% feed (so ~12 in/min) and it couldn't reach this before getting melted aluminum in the teeth. I think part of this is the lack of horsepower in my TAIG spindle and motor, I could see the bit complete stop occasionally.

Secondly, I think my rougher might be too dull from the last part but I am no where near an hour of cutting use. At 25$ a pop I would think the rougher would last longer!

I have included a pic of the rougher with the aluminum *jam* still on it. What causes this buildup to occur exactly? Of course, once this happens it no longer cuts so how do people setup a machine and walk away from it?

I also tried a 4 flute standard end mill, 0.07 in DOC with 11 in/min and 4200RPM with similar results, hardly get started before it's jamming.

Finally, the last thing I noticed is the part is deformed surely due to missed steps. I have 170oz.in. steppers on the X/Y axis, they are unipolar running half coil. Is this enough power?

I am a little suprised at todays efforts. The last part, pretty much the same. Ran at 12IPM, 5000RPM, .125 DOC and came out correct and without a problem....it almost seemed effortless to the machine.

Thanks,
C

You weren't using any sort of coolant were you? To get anywhere near advertised speeds and feeds of end mills you will need to use coolant. That's not to say you can't run without coolant, but you won't get to the feeds and speeds the maker advertises.
Aluminum building up on the edge like you show is not at all uncommon, and you will have to decrease the amount of of material you try and remove in a pass, apply some sort of coolant/cutting fluid to help with the buildup. More flutes also contribute to this problem as there is less space for chip evacuation. 2 Flute will get the chips out faster, and may work better.
If the bit is "stalling" it's not much surprise you are having trouble with missed steps. Your machine is limited in terms of horsepower and rigidity. You may simply be asking for more than it can deliver. I am not saying you can't cut aluminum, or anything else for that matter. But the amount of material you are trying to remove is too much for the conditions. Like has been said I would lower the DOC, and brush on something, WD40, tapping fluid, I suppose oil would work as well. It will make a difference. Chances are you can pop the chips off the edge with a sharp object like an awl or a machinist scribe. Personally I don't like TiN coated tools with aluminum. I prefer the "aluminum cutting" 2 or 3 flute bright finish HSS end mills for aluminum. They have flute geometries and helix angles optimized for chip evacuation. I have found that I get a lot more edge welding with TiN and aluminum, but I know others have had a lot of luck with it. Within the range of speeds and feeds that smaller machines use tool coatings are of limited use. They really come into play on larger production machines.

[DeusExMachina]

I started with a 0.2in DOC and moved down to 0.125 DOC. This is for a 3 flute rougher.

... 0.2, as in Almost 1/4"? Thats an insanely deep depth of cut for a benchtop mill. Depending on the HPs behind you spindle, 1/4 - 1/8 your cutter's diameter is all the deeper you want to go. On my Taig I have a 3 flute carbide cutter that I've tested up to 0.1" but I can only do that at low feeds and its rough on the cutter.

[guru_florida]

... 0.2, as in Almost 1/4"?

oh, yeah! I have been going about 40-50mils DOC up until the last part to go easy on the machine. I did the last part at 80mils and as I said it was quiet and smooth. I wanted to push the DOC so that I am using more of the tool instead of the first 50-80mils and the rest of the tool is primarily unused. It makes sense to, but I don't really know the limits of my own machine yet.

Why is 0.1" on your taig pushing it? Does it start to chatter, or is it the HP of the motor? I have the taig spindle but a different motor rated at 1/5 HP at 2.12 down-ratio.

Any word on the aluminum stuck in the tool? Is it just too high a removal rate for my machine?

Do you keep your dull tools and send them away to resharpen? They will get expensive at 0.1" DOC and the resulting longer cutting time.

C

[escott76]

oh, yeah! I have been going about 40-50mils DOC up until the last part to go easy on the machine. I did the last part at 80mils and as I said it was quiet and smooth. I wanted to push the DOC so that I am using more of the tool instead of the first 50-80mils and the rest of the tool is primarily unused. It makes sense to, but I don't really know the limits of my own machine yet.

Why is 0.1" on your taig pushing it? Does it start to chatter, or is it the HP of the motor? I have the taig spindle but a different motor rated at 1/5 HP at 2.12 down-ratio.

Any word on the aluminum stuck in the tool? Is it just too high a removal rate for my machine?

Do you keep your dull tools and send them away to resharpen? They will get expensive at 0.1" DOC and the resulting longer cutting time.

C

You don't have the rigidity or horsepower to take the kinds of cuts you are describing. When you can "see the spindle stop" it is a BAD THING. It means you are pushing too hard.
One of the ultimate limits of tools these size is the speed that the can remove metal. Go back to where it was smooth, as trying to use that much of the tool isn't going to do well on a machine this size.

[doanwannapickle]

For the most part, I've been following this feed and speed formula...
RPM = SFM × 12 ÷ π ÷ D
IPM = RPM × F × CL

D = tool diameter
π = pi (although it doesn't really look like it)
F = number of flutes
CL = chip load

Since cutting speed is approximate, this formula reduces to:
RPM = 4*CS/D
This makes it simple enough that you can usually do the math in your head.

WD40 makes an excellent cutting fluid for aluminum. At $15 bucks a gallon, it's very cost effective. It takes very little so I usually apply it with a brush. This also keeps the mist out of the air. If you buy a gallon, shake it before transferring to a smaller container. Some of the waxes tend to settle to the bottom.

Cheers,
Walt

[guru_florida]

You weren't using any sort of coolant were you? [snip] More flutes also contribute to this problem as there is less space for chip evacuation. 2 Flute will get the chips out faster, and may work better.
[snip] Personally I don't like TiN coated tools with aluminum. I prefer the "aluminum cutting" 2 or 3 flute bright finish HSS end mills for aluminum.

Thanks for the info. I am using a petroleum based lubricant that is made specifically for cutting Aluminum. It makes a real noticeable difference. There is a picture of the stuff in one of my first posts. I have also used tapping/drilling fluid that smells like bacon fat. It works good too, but I think the petro stuff works better. I also have a blower to blow the swarf away.

I am thinking the material getting stuck in the tool is a HP/DOC problem as you say, and maybe the tool is getting dull too.

My cutter was a 3 flute rougher that was made for roughing Aluminum. I noticed myself that the fewer flutes seem to cut better without welding but fewer than 3 flutes also means there is not always a flute in contact with the cutting surface and that leads to vibration so I am liking the 3 flute. (also poor surface finish, but I'm roughing anyway.)

[fatal-exception]

Even if you mill can cut up to .2" DOC, you will stress and wear it out much faster. .2" DOC at 12"/min in aluminum = .35 horsepower at the tool, so it looks like you do have the power, but barely.

Lots of coolant will stop the chip welding.

Hard to believe that the tool is still in one piece. Anytime that's happened to me, the tool has always broke.

BTW, nice job milling the dime!

Paul

[guru_florida]

BTW, nice job milling the dime!
Paul

What dime? That thing just popped out of my swarf?

What formula did you calculate that HP value from?

The aluminum didnt really weld to the tool. I popped it out very easily with a pointed edged tool and used the tool tonight to make another part no problem with a 50mil DOC. I just wanted to show a picture before I did so, so I can get an opinion on the reason.

I made my own CNC machine, but I still have little idea how to use it. lol! So I need people's experience here to guide me and pics are worth a 1000 words, right. An experienced machinist could see/hear my machine cutting and say, "speed/feed to fast", "to much DOC", blah blah blah...but I don't have that emperical knowledge yet. For now, I cut with one finger on the ESTOP just waiting for a "...mmmbrrrrrruuugghg!@#$%@%!@!%..."!

I think I can dial in the DOC, feed and speed now. The part I cut tonight turned out well. I included a pic of the two pieces. Both were cut with the rougher so I smoothed it as best I can with a metal brush but it's still rough. I keep misjudging my Z distance and the part releases during the roughing stage before I can do a finishing pass. The first pic is a robot I am building. And as you can see, I haven't modeled the body of the robot yet! hehe