Milling slot in aluminum t6061 - fast shallow vs slow deep

[dansawyer]

I have a project to mill a 1/2 inch deep 1/4 inch slot in aluminum. I have tried milling a shallow, 15 thousands, relatively fast, 20 ips at 1000 rpm. This works but it tends to clog the end of the mill. I did a small correcction cutting from the side of the cutter, this produced clean larger chips.
My question is: What is the most efficient way to cut aluminum? Is it to cut faster and thinner or slower and deeper?
Is this trial and error or is there a table?
Are fewer larger chips better or worse than more smaller ones?
Thanks, Dan

 

[mikey]

The fastest way is to use a roughing end mill and bring it to final size with a 2 or 3 flute high helix finishing end mill. In this case, a coarse pitch 3/16" high helix rougher, followed by a high helix 1/4" 2 flute end mill will work. If the slot has to be accurately sized then use a 3/16 finishing end mill and cut the slot to accurate width.

The rougher can handle a full diameter slotting depth of cut easily. Personally, I mill manually so I feed manually in slots so I can feel a slight resistance to the feed. Once the slot is roughed out, a finishing end mill can easily take a full diameter depth of cut to clean up the slot. Remember that roughing end mills can run 20% faster and be fed 20% faster as well.

Use a stream of compressed air to clear chips. This keeps the end mill from having to recut chips in the slot, making for a more efficient cut and you end mill will also live a lot longer.

 

[JimDawson]

I would use a 2 flute aluminum cutting carbide end mill or an equivalent router bit from Home Depot. 3000 RPM, 15 IPM, 0.125 DOC. Mist coolant with extra air for chip clean out. This would give you a chip load of 0.0025 and 196 FPM.

 

[markba633csi]

Trying to cut slots to final size in one shot often gives a poor, rough finish. Try to do an undersize cut first, clean out the chips, then do the final cut.
Use a light cutting fluid with aluminum for the finish cut- wd40, kerosene, or even liquid wrench in a pinch
-Mark

 

[dansawyer]

I would use a 2 flute aluminum cutting carbide end mill or an equivalent router bit from Home Depot. 3000 RPM, 15 IPM, 0.125 DOC. Mist coolant with extra air for chip clean out. This would give you a chip load of 0.0025 and 196 FPM.

I did a test run at 1000 rpm, .25 DOC, and 1 IPM without coolant. I only cut about 2 inched but it worked without issue.
My previous run was 1000 rpm, .015 DOC, and 20 IPM without coolant. In this case the work piece got very hot after a few minutes. (I was cutting a circle in 1/2 inch aluminum.) (I don't have coolant set up yet, however I can vaccum the chips as they are made.)

 

[JimDawson]

I did a test run at 1000 rpm, .25 DOC, and 1 IPM without coolant. I only cut about 2 inched but it worked without issue.
My previous run was 1000 rpm, .015 DOC, and 20 IPM without coolant. In this case the work piece got very hot after a few minutes. (I was cutting a circle in 1/2 inch aluminum.) (I don't have coolant set up yet, however I can vaccum the chips as they are made.)

The fact that your cutting parameters work for your application is good. The real problem with aluminum is that it tends to weld to the tool bit, this is where the coolant (or lubricant) comes in. Keeping the the tool wet is somewhat important. As I said above I use a mist system, maybe about a cup of coolant per hour.

Using the cutting parameters you state, I would expect the tool to be rubbing more than cutting thus the work would be getting hot as you experienced. Ideally you want to take a larger chip load to send the heat out with the chip. Cutting on size slots is always more problematic other cutting because of the difficulty of removing chips from the cutting area.

Most times I use a smaller endmill that the slot width and use a ramp-in profile or adaptive clearing cutting strategy to be able to more effectively clear chips.

 

[Mitch Alsup]

I have a project to mill a 1/2 inch deep 1/4 inch slot in aluminum.

With a narrow slot like this, I, personally, would be tempted to use a saw (slitting saw) instead of an end mill.

 

[Moe]

The fastest way is to use a roughing end mill and bring it to final size with a 2 or 3 flute high helix finishing end mill. In this case, a coarse pitch 3/16" high helix rougher, followed by a high helix 1/4" 2 flute end mill will work. If the slot has to be accurately sized then use a 3/16 finishing end mill and cut the slot to accurate width.

The rougher can handle a full diameter slotting depth of cut easily. Personally, I mill manually so I feed manually in slots so I can feel a slight resistance to the feed. Once the slot is roughed out, a finishing end mill can easily take a full diameter depth of cut to clean up the slot. Remember that roughing end mills can run 20% faster and be fed 20% faster as well.

Use a stream of compressed air to clear chips. This keeps the end mill from having to recut chips in the slot, making for a more efficient cut and you end mill will also live a lot longer.

 

[Moe]

You should use coolant if you can even a spray to lubricate it will help your clogging. There some cutting oil made specifically for aluminum I have use it before and it works well. When in a bind and didn’t, have any special cutting oil I used some of the solution that was in my cleaning tank .