What's new
What's new

60 Degree Groove

rokstarr999

Aluminum
Joined
Feb 7, 2014
Location
Sonoma County, USA
I'm looking for some advice on machining these grooves. I programmed it to rough out the groove with a .03 ball mill and then finish it with a 2FL .25" Dia 60 Deg chamfer tool. The tool has around a .015" flat at the tip and I'm thinking its just going to break at the tip. Material is 416 SST. The groove comes to a sharp point in the model. I think I can get away with the .015 at the tip. I have 4 of these to do. 2" wide x 9" long/ 34 grooves per part at .121" deep. Whats the proper way to make a groove like this?

Thank you.

V Groove.jpg
 
On a horizontal mill with a gang of 60* saws. But that's not an option, is it?

Do you have a right angle head? Still the way to go, just one at a time. And what machine are you using to make these?

If the machine's robust enough, you could make a long arbor and use a saw, fixturing the parts vertically on a right angle plate. I'd want to use a minimum of a 1.5" arbor, down to 1" pilot for the saw. I've done some custom arbors when I've had the need, it's not that bad. Just slow the RPM and feed to suit your setup.

Mating the arbor to the toolholder is the issue, you want it robust - best way (presuming a BT/CAT40 taper) is use a suitable long blank like this: https://www.amazon.com/Lyndex-C4008...Bar,+CAT40&qid=1595543388&s=industrial&sr=1-3

looks perfect, except for likely wanting to turn the OD down a bit - but if you use a 3" saw, then just the pilot and tapped hole need to be made. Well, and the cap too, of course...
 
On a horizontal mill with a gang of 60* saws. But that's not an option, is it?

Do you have a right angle head? Still the way to go, just one at a time. And what machine are you using to make these?

If the machine's robust enough, you could make a long arbor and use a saw, fixturing the parts vertically on a right angle plate. I'd want to use a minimum of a 1.5" arbor, down to 1" pilot for the saw. I've done some custom arbors when I've had the need, it's not that bad. Just slow the RPM and feed to suit your setup.

Mating the arbor to the toolholder is the issue, you want it robust - best way (presuming a BT/CAT40 taper) is use a suitable long blank like this: https://www.amazon.com/Lyndex-C4008...Bar,+CAT40&qid=1595543388&s=industrial&sr=1-3

looks perfect, except for likely wanting to turn the OD down a bit - but if you use a 3" saw, then just the pilot and tapped hole need to be made. Well, and the cap too, of course...

Using a Haas Mini MIll so I definatly don't have enough travel for that.
 
If the part is short(ish). Make a soft jaw to kick it up at a 60 degree angle and just
blast it with a dove tail cutter.

This isn't for 60 degrees, but to make 90 degree serrations for my lathe soft jaws. It was
going to be 60 degrees and a dove tail cutter until I realized that my lathe chuck is a bastard
that nobody will admit exists. Half metric, half imperial.

This jaw (I actually made 2) has come in handy for a whole lot of other odd jobs. But its not
hard to make and the programming is stupid simple. Just a simply sub, Up and Over, Up and Over.
Of course the math is a little harder for 60 than 90, but its still pretty farcken easy.

26053328313_fd5532d5a4_c.jpg
 
Like Bob said, kick it up and use a dovetail cutter. I do a few parts like this on the 5axis and horizontal with an ABTools dexi-tovetail

Or if small enough, you can hold it at 90° and use a single-point threadmill.
 
I'm looking for some advice on machining these grooves. I programmed it to rough out the groove with a .03 ball mill and then finish it with a 2FL .25" Dia 60 Deg chamfer tool. The tool has around a .015" flat at the tip and I'm thinking its just going to break at the tip. Material is 416 SST. The groove comes to a sharp point in the model. I think I can get away with the .015 at the tip. I have 4 of these to do. 2" wide x 9" long/ 34 grooves per part at .121" deep. Whats the proper way to make a groove like this?

Thank you.

View attachment 294756
done quite a few parts like this on my vf2ss years ago in 316 ss. we used 60 degree thread cutters on a long shaft. I forget where I bought them made but they worked really well. tips held up good too. had the option of a steel shank with carbide cutter or solid carbide. I went with the steel shank. if I recall it was a 3/4" shank with 1" dia cutter. we didnt go 9" I think we went like almost 6" the 1/2" shank ones will work till about 4" depth before any vibration/flex .
I wanna say it was that place out of ca. internal tool? but i just looked and they didnt go that long.
 
Yeah, maybe someone already suggested that in #2...

Ahh, your post was the inspiration to drag up the old picture. I should have credited your comment!

I realize it may not be useful for the OP and his available machinery, but I thought you may like it ;-)
 
I know it sounds crazy but can you stick a little 60 degree threading insert in a lathe tool holder and hold that in a square collet in the Haas and go down in Z, rapid in Y to cut/thread, then back up in Z, back back in Y, then back down in Z just a thou or two, and repeat? Just thinking outside the box here.... I also don’t know anything about SS.
 
So the engineer brings me the last one of these parts that were built and there was a radius in the bottom of the groove. So either the vendor made the part the way they wanted to make it or they got a deviation that was never documented.

I do have another question though.
I added a .063 radius to the bottom of the groove and am running the part in a two vise set-up. 1/8" 4Fl ball mill roughing out the groove and finishing with a 1/16 Ball Mill. I'm at 3 hours per part and am wondering if this is reasonable. 34 grooves per part. 1/16 BM running at 9400 RPM and 18 IPM with a .006 Step Down is roughly 5 min a groove. Also, the roughing cycle is a trichordial tool path and am wondering if running these tiny arcs at 30 IPM is bad for the machine?

Thank You to everyone that had input on my post.
 
You are 1/8" or so deep, with a 1/8" or so ball mill. Just plow it through,
I can't imagine any reason to use a trichoidial path at that depth.

And what is your tiny radius, it has to be itty bitty. And yes, that
can mess up your screws if done for a long duration.

Also. Why switch to a 1/16 ball? Just use the 1/8" and blast it. Run
bottom to top, take advantage of the chip thinning, and run your feed
per tooth the same as your step down. Be done in no time.
 
You are 1/8" or so deep, with a 1/8" or so ball mill. Just plow it through,
I can't imagine any reason to use a trichoidial path at that depth.

And what is your tiny radius, it has to be itty bitty. And yes, that
can mess up your screws if done for a long duration.

Also. Why switch to a 1/16 ball? Just use the 1/8" and blast it. Run
bottom to top, take advantage of the chip thinning, and run your feed
per tooth the same as your step down. Be done in no time.


Made a mistake in my last post. Should have been .03" Rad at the bottom, hence the 1/16 Ball Mill. I will try doing away with the trichord tool path and plow through as deep I can with the 1/8".

Thank You.
 
Running a dynamic path with really small movements will ruin your screws/nuts. There's not enough movement for lubrication to get to that area on the ball screw.

It's happened to others before...
 








 
Back
Top