Engraving serial number, etc. (7075-T6 aluminum) via CNC mill?

[JimDawson]

Would somebody please give me a feeds and speeds for engraving text (about 1/4" vertical height) into a sheet of 7075 T6 using a; 1/8" shank, .005" tip, 60 degree etching bit.

From cruising around the threads I am thinking about 4 ipm @ 5000 rpm using a spring loaded etching tool. I am thinking that .015"depth of cut would look good, 3 passes at .005"


Please advise. Thank you.

I think you are right in the ball park. A higher spindle speed would be helpful, but ya gotta use what ya got.

I did this in one pass with a 90* V-cutter at 3 IPM, 0.006 DOC, 3000 RPM, in 6061 T6. Not the best I have seen, but it looks pretty good, and the tool was a bit dull. I did a couple of test runs to figure out the best combination of feed and speed.

 

[Drew Eckhardt]

Would somebody please give me a feeds and speeds for engraving text (about 1/4" vertical height) into a sheet of 7075 T6 using a; 1/8" shank, .005" tip, 60 degree etching bit.

10 ipm (5 ipm plunge) @ 5450 RPM using a single flute .010" 60 degree single flute bit cutting .010" deep in one pass. Logically half those feeds using a .005" tip and the same if you can double the speed - I was limited by Tormach top spindle speed in high gear.

Please advise. Thank you.

Play with it and see what works for you.

The examples are 6061-T6. Ones lacking a feed rate are 10 inches per minute which I used on my lower.

.010" tip 60 degree included angle 1/4" shank single flute solid carbide engraving tool. 5450 RPM (more would have allowed a higher feed rate, but that's the Tormach PCNC1100 limit). 5 ipm plunge.

Apart from the .006" example everything including my lower is .010" deep. Except for the 2-pass example (.005" then .010") everything is single pass including my lower.



This is 7075-T6 at 10 ipm (5 ipm plunge) and 5450 RPM .010" deep in one pass with a .010" tip 60 degree single flute .250" engraving bit

 

[JimDawson]

Looks good!!

 

[mofosheee]

10 ipm (5 ipm plunge) @ 5450 RPM using a single flute .010" 60 degree single flute bit cutting .010" deep in one pass. Logically half those feeds using a .005" tip and the same if you can double the speed - I was limited by Tormach top spindle speed in high gear.



Play with it and see what works for you.

The examples are 6061-T6. Ones lacking a feed rate are 10 inches per minute which I used on my lower.

.010" tip 60 degree included angle 1/4" shank single flute solid carbide engraving tool. 5450 RPM (more would have allowed a higher feed rate, but that's the Tormach PCNC1100 limit). 5 ipm plunge.

Apart from the .006" example everything including my lower is .010" deep. Except for the 2-pass example (.005" then .010") everything is single pass including my lower.

View attachment 75771

This is 7075-T6 at 10 ipm (5 ipm plunge) and 5450 RPM .010" deep in one pass with a .010" tip 60 degree single flute .250" engraving bit

View attachment 75772
View attachment 75773

Did you use a spring loaded engraving tool and coolant? Thanks very much. Jerry

 

[mofosheee]

Dear Members:


I am about to cut fcp pockets in 7075 T-6 Al using a cnc mill. I've successfully done this before using a 1 h.p. cnc machine, .25" end mill and program that I wrote..........and it was a slow process.


Since there is more than one way to skin a cat my question is..............

If I used an end mill only, how much should I plunge my end mill bit per pass i.e. .025" per pass?

Or should I "hog" out the major material with a .5" and .375" drill bit then finish up with an end mill?

Thanks all

 

[JimDawson]

If your machine is stable enough, 0.125/pass should be safe. I don't think that would require anywhere near 1 HP. In a scrap piece, try it at 0.060 first then try 0.125 to see how your machine reacts. WD-40 as a coolant.

I have cut 0.625 deep, full width, in 6061 with a 0.25 bit @ 8 IPM with no problem on my mill.

 

[Rick Leslie]

Forgive me if I'm wrong, but I thought ATF required .030" depth on identifying marks, not .003". I've got quite a few to mark at some point so I appreciate the input and samples here. Although it will take some doing to get my tired Sherline spindle up to a respectable speed.

 

[Beone]

I am doing a lot of engraving on cast plaques cast from 6061. I use a 60 degree engraving cutter. Two passes of 20 thou for 40 thou total at 20 ipm on a router around 20000 rpm. No problems. I do have an air blast of a HF airbrush directed at the tip with a barely discernible mist of plain water.
dave

 

[Ebel440]

If your using a cnc to cut the pocket you could ramp the tool in depending on the size of the pocket. It helps to prevent chips from building up in the center of the end mill.