# Slot milling in 6061-o Aluminum 0.04 thick help



## Pumper (Apr 29, 2022)

I am trying to mill some slots in the aluminum to shape it.
I had a suggestion to run it at 4000 RPM and a feed rate of 8 inches/min at full depth of the part.  I do not have the way to add coolant so you can imagine what happened.

I have no ides on how to do this so I need help with the speeds and feeds etc.
I have attached a picture of my set up and the results of my first try.
I am feeding left to right so it is climb milling at full part depth of 0.04.


----------



## markba633csi (Apr 29, 2022)

So you're getting chatter?  Mostly I think it's due to your setup/fixturing- too precarious
I would fasten the wooden back board directly to the table for starters; eliminate the vise.  As rigid as possible is best.
Secondly, I see a problem with the screws- the three at the rear are not allowing the small piece to fall away from the main workpiece
I would remove those and use the three unused holes in the main workpiece, plus the tab clamps you have at the ends. (although the 5 screws
in the main workpiece would probably be sufficient, with washers under the screws to help spread the force)
Often it is difficult to make a clean slot to size, due to chip buildup. If possible use an undersize endmill first, then finish with the
desired size.  Stop and brush away chips frequently.
-Mark


----------



## RJSakowski (Apr 29, 2022)

I would make a first pass as a skim cut and make multiple passes.  Say .01"  on the first cut and .02" on subsequent passes.  Use a sharp end mill and WD40 as a lubricant to prevent galling of the end mill..  I wouldn't leave the waste piece free as it has a tendency to jump when making the final separation.  I would add an additional screw in the center hole and possibly a bar across the  entire width to reduce flexing.


----------



## Pumper (Apr 29, 2022)

Thanks markba633csi, I will try your suggestions.
It may be chatter but what I see in the picture is too much tool loading and the aluminum is welding itself to the tool bit.
I was brushing the chips away as the tool progressed.
I should have told what tool I am using, it is a 1/8" 3 fluted HTC carbide  100-3125  3FL SE SO BRITE.

How do I calculate the proper speed and feed to start with to be extra conservative?


----------



## Pumper (Apr 29, 2022)

Thanks RJSakowski.
I was doing something similar at first but going down 0.02 each time and using 1770 RPM and 2 inches per min.
That was somewhat successful but still leaving a small burr which I could handle.  I was trying to speed up the process but maybe I can't.


----------



## Road_Clam (Apr 29, 2022)

4000 rpm is WAY too fast for the hobbiest with no coolant. I would try at about 1600 rpms and about 3.5 ipm , and also important is having an air blow setup to expell the chips out of the slot as you are milling. I also agree do multiple doc passed such as .015" Have patients when hobby machining on benchtop mills. They will do a great job, just execute very conservative . I like using Cool Tool II as a cutting lubricant with aluminum. 






						Cool Tool II - Industrial Cutting & Tapping Fluid - Monroe Fluid - MCE Chemicals
					

Cool Tool II - Universal cutting and tapping fluid for ALL metals!



					www.cooltooldirect.com


----------



## Jim F (Apr 29, 2022)

Pumper said:


> Thanks markba633csi, I will try your suggestions.
> It may be chatter but what I see in the picture is too much tool loading and the aluminum is welding itself to the tool bit.
> I was brushing the chips away as the tool progressed.
> I should have told what tool I am using, it is a 1/8" 3 fluted HTC carbide  100-3125  3FL SE SO BRITE.
> ...


RPM= ( CSx4 )/Dia.


----------



## Aukai (Apr 29, 2022)

Are you using a 2, or 3 flute cutter?


----------



## mattthemuppet2 (Apr 29, 2022)

give it a squirt of kerosene or WD40 as it cuts, that will help reduce chip build up. that pushed up material is either from a dull cutter (or chip build up ) or from the unsecured part of the work piece bouncing up and down in the cut. Cutting thin sheet is a pain, you'd be better off clamping it between two sheets of alu and clamping that to the table. Cutting wood with HSS endmills, especially that fast, will take the edge off them really quickly.

But definitely use some sort of cutting fluid, makes a world of difference using HSS with alu.


----------



## Pumper (Apr 30, 2022)

Here is my latest try.
Feed 3.5 inches/min
1640 RPM
0.010 depth added each pass, took 3 passes to cut 0.040 material I suspect the bit is lifting the part a little.
I will be adding a bar across the entire piece.
New 3 flute 1/8 carbide bit.  The bit is clean after milling, no welding.
I used WD40 and compressed air through the process(don't like the mess it creates).
Basically I can use the piece this way after a little clean up.  But I will experiment more with your comments.


----------



## Road_Clam (Apr 30, 2022)

Looks much better. The speed and feed I gave you is a .0007" per tooth chip load (based upon a 3 flute mill). If you try 1900 rpm and 3.5 ipm  that works out to be .0006 . Try different chip loads and feel how the tool is cutting. Once you start to gain experience you will be able to "feel" on the table handwheels how the tool is cutting. You can start to feel when the tool is getting worn or getting clogged by feeling added resistance as you feed into your workpiece. You ideally want to mill to feed exactly the same throughout your entire cut.  Good luck, keep at it.

Simple chip load calculator :









						Chip Load Calculator - Calculator Academy
					

Enter the feed rate, RPM, and the number of flutes into the calculator to determine the chip load.




					calculator.academy


----------



## Pumper (Apr 30, 2022)

Thanks for that suggestion.  I assume the less chip load the cleaner the cut?  To a point where it is too low?
If I use 1800RPM and 3 inches/min I get 5.5 chip load.  1800 is the max RPM I get on the low speed setting, it is belt driven.
My mill is set up as CNC so the feed rate is constant.


----------



## Pumper (Apr 30, 2022)

I mean .00055 chip load not 5.5


----------



## Alcap (May 1, 2022)

Would a downward spiral bit have any advantage in this situation?  I’ve used them in my woodshop but not in metal .     https://www.precisionbits.com/down-cut-bits/


----------



## Road_Clam (May 1, 2022)

Alcap said:


> Would a downward spiral bit have any advantage in this situation?  I’ve used them in my woodshop but not in metal .     https://www.precisionbits.com/down-cut-bits/


I've been cnc machining for about 21 years and never heard of this type of mill. A quick read of the description would tell me a definate NO in aluminum. There is what's called "high rake" type mills that are ideally suited for aluminum work only. But again this is for a high rpm / high SFM  feeds in a CNC application. The limitations of the hobby benchtop mill require very conservative trial and error.


----------

