Advice on cutting a dovetail in 6061 T6.

I could use a starting chip load for cutting a 60* dovetail slot single side in some 6061 T6. The slot is .380" deep in the side of a part that will be a lock on a male dovetail rail. I only have one cutter so I want a good starting point. The VMC has flood cooling and the part will be held in a vise with soft jaws. it is just a simple 60* angle notch in the top right hand corner with the machine traveling in the X axis.

View attachment 308985

How many?
Carbide or HSS?
Rule of thumb would be 3-4 cuts at least, and leave material on the floor and wall for semi-finish, and for the last cut leave material only on the angled wall.
My suggestion would be .0015 per tooth, or less, even with multiple passes. My experience has been that these are kind of fragile. Carbide could live with more, but not worth pushing it, especially with only 1 cutter. Good luck!

eaglemike said:

How many?
Carbide or HSS?
Rule of thumb would be 3-4 cuts at least, and leave material on the floor and wall for semi-finish, and for the last cut leave material only on the angled wall.
My suggestion would be .0015 per tooth, or less, even with multiple passes. My experience has been that these are kind of fragile. Carbide could live with more, but not worth pushing it, especially with only 1 cutter. Good luck!

Click to expand...

The cutter has carbide edges. Thanks I was going to start at .002" 6000 RPM. I will try .0015.

Rough out all you can with a end-mill first, use a full steam of coolant to wash the chips away and .001/.0015 chip load per tooth...Phil

Hi gundog:
I prefer to run my cutter down the angle of the dovetail in smaller steps so I never take a full width cut.
It's easy to do with CNC and it's kinder on the machine and the workpiece (and the cutter too!)
So I will make a square step first as others have described, and then I will start at the top with a 0.050" to 0.100" DOC and mill my first step leaving 0.010" or so on the sides.
My next pass will be positioned in and down so I take another 0.050" to 0.100" DOC but nothing on the sidewall of my first cut.
I will rinse and repeat until I've traversed all the way to the bottom of the dovetail.
Then I'll do the same again for finishing.
It takes longer, it's more cuts, but it makes a better, more accurate dovetail and it doesn't try to shake the machine apart while it's doing it and it eliminates all the groaning and graunching typical of full-depth dovetail cuts.
You can also feed it a lot faster.

So it's not a good production strategy, but for one-off's it works very well.

On the other hand, if you need balls-out productivity, go for the biggest most rigid cutter you can get your mitts on...mount it as close to the front spindle bearing as you can, fixture your part so it's bomb proof, and do it on a beast of a machine in one pass.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

lF access allowed I would use a angle cutter to do the job.Stronger tool one rougher and a finishing cut.Borrow a cutter or buy a used one off Ebay

gundog said:

I could use a starting chip load for cutting a 60* dovetail slot single side in some 6061 T6. The slot is .380" deep in the side of a part that will be a lock on a male dovetail rail. I only have one cutter so I want a good starting point. The VMC has flood cooling and the part will be held in a vise with soft jaws. it is just a simple 60* angle notch in the top right hand corner with the machine traveling in the X axis.

Click to expand...

I usually run carbide dovetail mills in 6061 at 1000 SFM. Chip load varies by neck diameter -- from my notes, 1/8" neck = 0.0014 FPT, 1/4 = 0.00275 FPT, 3/8 = 0.0040 FPT, 1/2 = 0.0055 FPT. Usually three passes per side.

But, I ran a bunch of Picatinny rail parts a while back. I got a form tool from AB Tools. I don't remember the exact cut parameters they gave (I think I remember 2000 SFM?) but it was crazy fast and full depth. Worked great, so maybe I'm too conservative.

AB tool was the only ones worth buying ,, I started with MSC cutters and the finish was crap on the parts tell I ordered my first one from AB tool and I was so happy with it I ordered 2 more for the shelf ,,, that was about 6 years ago and there is still 2 on the shelf, they make solid carbide I think up to 5/8" shank and then do the carbide tipped for 3/4" and larger , I have been running the 3/4" at 6K and 30 IPM ,

you might want to turn your feed and speed down to like 25% and single block the first part ,,, I have found programming is easy to screw up on odd shaped cutters ,,

It's a dovetail for clamping, and it's aluminum, nothing special. Go to town on it.

I cut the first batch of 106 parts today they came out good. I started at .0015" IPT and it sounded happy so I left it alone and ran them.
Thanks For the help.

The cutter I would use would be an angle cutter the wheel type with inch bore and keyway in.Mounted on stub arbor in spindle dovetails often fail and snap at the neck the weakest point the wheel type cutter is stronger take that depth in onecut and no babying with feed

onecut said:

The cutter I would use would be an angle cutter the wheel type with inch bore and keyway in.Mounted on stub arbor in spindle dovetails often fail and snap at the neck the weakest point the wheel type cutter is stronger take that depth in onecut and no babying with feed

Click to expand...

Do you have a link or picture of the type cutter you are referring to? I will be making a lot of this part so I don't mind spending some $$ on a better cutter.

Is this the type cutter you are talking about?
2-3/4 x 1/2 x 1” bore single angle (60 degree) Milling Cutters, lot of 2, LOOK | eBay

Yes thats the one I mean "single angle" cutter.Just make sure the length of flute will cover the full face of the angle you want to machine.Why would you want to use a dovetail cutter unless there was no alternative if you have the room to get in with one of those get rid of the dovetail cutter.The angle cutter is easier to sharpen but I doubt you will need a regrind before your finished providing you choose the correct speed-I would do it in onepass on depth,Maybe run back with a dummy cut if finish dictates

I had a Cat 40 1 1/4" shell mill arbor I was not using so I picked up a 60 degree 3"x 1/2" x 1 1/4" single edge Doall HSS cutter off ebay new old stock $36. I will give that a whirl on the next batch. They had more with a 1" bore but I have a face mill on the only 1" bore holder that I have and I use that tool a lot so I don't want to change them back and forth or spend the $$ for a new holder.