Taking the plunge

[mofosheee]

Using a Tormach 1100 CNC machine, milling a 1.5" depth pocket x 3" long and using a HSS .375" endmill in 7075 T-6 Al........... would somebody please give me an approximate plunge depth for milling this pocket.

I'm not sure how hard I can descend in the "z" for each pass.

 

[JimDawson]

I would start with 0.050 and see how the machine ''feels'', if it likes it, try 0.100. I run mine all the time at 0.200 to 0.250 DOC with a 0.4 step over. I profiled a bunch of 5/16 thick 6061 parts at full depth and 100% cut width with a 0.375 end mill. The cutter will take the load, so it's just a matter horse power and how rigid your machine is. A lot of times I will drill a hole where the tool plunges that way you are not trying to drill with an end mill.

EDIT:

I should also add that I try to set up the tool path where it can plunge into air where possible. When I have to plunge into the material, rather than air, that I set the plunge speed to 0.2-0.5 of the cutting speed.

 

[mofosheee]

I would start with 0.050 and see how the machine ''feels'', if it likes it, try 0.100. I run mine all the time at 0.200 to 0.250 DOC with a 0.4 step over. I profiled a bunch of 5/16 thick 6061 parts at full depth and 100% cut width with a 0.375 end mill. The cutter will take the load, so it's just a matter horse power and how rigid your machine is. A lot of times I will drill a hole where the tool plunges that way you are not trying to drill with an end mill.[/QUOTe

Thank you for the quick response. Plunging with an end mill seems like an unnatural act. I like your suggestion of drilling holes / not using the end mill as a drill

Jerry

 

[12bolts]

Jerry,
End mills are not really made for plunging into material, as most are not designed to cut full diameter on the end. If you check your end mill you may note that the cutting flutes dont extend fully across the tip and there is a large area that just rubs if you plunge in. (disclaimer, they do make end cutting end mills)
Slot drills are what you should be using in your situation. Or drill a hole to depth and then your end mill can plunge into air.

Cheers Phil

 

[DMS]

This is one of those "over here, over there" sort of things. In the US, both center cutting and non-center cutting milling cutters are called "end mills" and the distinction is made of either center cutting, or non-center cutting. 2 flute cutters are always (as far as I know) center cutting. 3 flutes are almost always as well. 4 flutes and more, you have to check what you are buying.

Regardless, to answer the question, assuming a 2flute cutter, GWizard gives a plunge speed of 6.7 ipm at 3700rpm. I try to keep cut depth under 50% of the tool diameter when pocketing, as I have had bad times with chip welding with 6061 (I have never cut 7075, but I believe it should be less sticky). I tend to rough out the pocket leaving about 0.020 or 0.030" left, and then take a final finish pass or two at full depth of cut.

I might also recommend grabbing some 3 flute carbide end mills when you see them on sale at Enco or the like. You will be able to run your spindle up to top speed, and you will have less deflection in your tool to boot. I have been buying the Atrax 3flute cutters for a while, and they are my favored cutter for aluminum.

 

[mofosheee]

Thanks all! Great advice. My intended path will be to use a drill to extract the majority of the material (spare the end mill of plunging) and clean up the whole with the end mill at recommended feeds and speeds