Need advice milling deep slot.

I have a 6061 part with 2 slots, about 11mm wide and 5" deep. The slot ends up through. I am able to attack them from both sides, however there are other features next to them that require a minimum of 3.25" extension. I'm using a 3/8" endmill with a reduced neck and 1/2" for length. Not exactly the greatest set of requirements, but that's life.

I've tried all sorts of different things. 

Helicals MAP suggestions, HSM Advisor's suggestions, and everything in between. 1500-15000 rpm. I've held it in a lyndex SK10, and a VC13 holder. As of now I've got nothing but chatter, broken tools, and broken dreams. If anyone has any suggestions, I'd really appreciate it!!!

pre drill with as thin of a web as you can get away with. Use a tool with a corner radius to keep from blowing up your edge and finish the wall as you step down.

I routinely mill slots 8-10X dia in 6061 and this works well for me.

Is it a 3.25 extension or 3.25 gauge length?

yoke said:

pre drill with as thin of a web as you can get away with. Use a tool with a corner radius to keep from blowing up your edge and finish the wall as you step down.

I routinely mill slots 8-10X dia in 6061 and this works well for me.

Is it a 3.25 extension or 3.25 gauge length?

Click to expand...

3.25 extended from the collet. Any suggestions on speeds/feeds and stepdown?

I use shrink fit holders which is probably a bit more rigid than your setup. Maybe?

I would just sure the recommended feeds and depth of cut. Try to keep wall engagement as a constant so it isn't only hitting the web.

You're around 8.6X diameter which is getting up there. You could try to plunge on the web left from pre drilling operation with your end mill to create some separation then go back and finish the wall with the endmill.

I typically stick to .25 tools and under...

What tool are you using? I have a few of these Reduced Shank 3/8 3 Flute End Mill Finisher 5.0 long X .354 Shank MariTool
and typically use them at 2.1 or 3.1" stickout with good results. I'm only using an ER20 as well.

Look at gw Shultz tools they make a cutter for ar15 mag wells that is reduce and ready to go. It works good
Don


Sent from my iPhone using Tapatalk Pro

I used to mill pockets into the end of 6061 stock. The pockets were about 3.500 deep, I would drill a hole and program a bunch of plunges with an endmill...only way it could be done. Then machine the walls stepping down. Chatter is just a part of life with long thin cutters.

thesidetalker said:

What tool are you using? I have a few of these Reduced Shank 3/8 3 Flute End Mill Finisher 5.0 long X .354 Shank MariTool
and typically use them at 2.1 or 3.1" stickout with good results. I'm only using an ER20 as well.

Click to expand...

It's a Helical 82480

Helical Tool

plastikdreams said:

I used to mill pockets into the end of 6061 stock. The pockets were about 3.500 deep, I would drill a hole and program a bunch of plunges with an endmill...only way it could be done. Then machine the walls stepping down. Chatter is just a part of life with long thin cutters.

Click to expand...

Any idea on S/F of the wall machining?

As said earlier,
1. Remove maximum stock with drilling.
2. Plunge thin webs -- ask your tooling supplier for special "Plunging" geometry endmills.
3. Finish the walls with reduced shank endmills.

JBethell said:

Any idea on S/F of the wall machining?

Click to expand...

Not very good lol

plastikdreams said:

Not very good lol

Click to expand...

Speeds/feeds, lol, not surface finish.

It has a 3/8" shank. Grind a little flat on it and stick it in a set screw holder.

What machine are you doing this on.. Maybe its just a floppy POS to begin with..

Here is some of my chatter stopping methods when working with long endmills.

Looks like your endmill is a square corner, try something with a radius or a chamfer.
Feel free to chamfer it yourself. Its not that hard, and if you have some practice,
you can even put your own radiuses on. Sharp square corners on long endmills can
get really grabby.

Make the tool "MORE VARIABLE".. Seriously.. Just grind a big honking chamfer on one
flute. It works, I've done it a bunch of times. I had one machine quite a while ago
that would do it for me.. Shake, rattle, noisy.. Until a corner broke off, and then it
cut clean.. Occasionally taking the cutter with it, so I started just taking new endmills,
Vari flutes, with corner rads and just grinding a big chamfer on one flute. Floppy machine,
FLOPPY!!! The X-Y was pretty stout, the spindle was the problem, and tool interface was
shit. A series 10 Acroloc..

RAMP!!! It puts pressure straight back up through your spindle. Sort of like how a high feed
mill works, and why they can hang out a mile. You're taking that little bit of flex out of the
Z axis.. You're making your machine and tool more rigid than it actually is.

Those are my little tricks. Though one more thing. In my experience using long endmills,
chatter happens when the tool doesn't have much to do. If it doesn't have much to do it
bounces around and makes a lot of noise. Like an employee with a cell phone.. Keep it
busy and it tends to be calmer and less noisy... Almost like a little kid.

I've roughed out a pocket or an outside wall, and left a little more on the last step down.
Keep the bottom of the tool busy on the finish, and the tool calmed right down.. Ran it
faster and ran it harder..

Lots of a little tricks, and essentially none of them have to do with slowing down
the speed, or feeding it lighter. Occasionally that is the only answer, but what you
are doing isn't that crazy.

One last though. Only use the long tools when you need them. Go as deep as you can with
a short one. Go deeper with a little longer one, and then waste the time with the long
expensive endmill, only where you actually need it.

Bobw said:

It has a 3/8" shank. Grind a little flat on it and stick it in a set screw holder.

What machine are you doing this on.. Maybe its just a floppy POS to begin with..

Click to expand...

Thank you for the suggestions. The machine is a 2 year old Matsuura H.Plus-500, so I think the machine is fine. As far as the holder, I have a set screw holder on the way. Originally, I wasnt able to find one. It's a Cat50, in which we run all dual contact to keep the spindle face clean. We stick to lyndex and big kaiser if we can. However lyndex doesn't make a 3/8, and big kaiser's shortest is 6" gage length. Ended up finding a YG-1 holder which should be here tomorrow.

Regarding the concept of cutting harder to get rid of chatter, generally, I agree that it's the way things go, although on these long reach tools, it always seems to make it worse when. I try it. Helical suggests something like a 7° ramp angle at max RPM which absolutely did not work. I'd love to see it done successfully, because I usually end up having to drop the SFM way down and keeping the chip load up when using long tools.

As far as the radius, I couldn't find one with a radiused corner and enough of a reduced neck, and due to the production nature of the part, we try to keep tools "off the shelf" whenever possible for our automated ordering system. I only looked briefly for a radiused tool though since I got through the slot and need to get the first part out. Once that's done, I'll definitely be trying a radiused tool if I can find one.

Thanks again!