[deepaknatraj]

Hello,

I have to groove a 1.01" O.D X 0.71" I.D. to a depth of 1.44" on 12L14.

Does anyone have any idea or a tooling recommendation for accomplishing this?

This is turning out to be too much of a headache.

Thanks

[RCaffin]

Try the ThinBit catalog. They specialise in that.
Um ... to depth of 1.44"?
Fabricate.
Cheers
Roger

[robbyfischer]

Deep,

Try PH horn or Iscar.
What seems to be the problem? Chips won't break?
What are you currently using? Feed/Speed

[deepaknatraj]

I contacted Thinbit. They said they cannot help us in the situation.

[deepaknatraj]

Deep,

Try PH horn or Iscar.
What seems to be the problem? Chips won't break?
What are you currently using? Feed/Speed

I fabricated a trepanning tool with HSS.

Chips are breaking great. I don't have a problem with that.

But the problem with that is it's leaving a rough surface finish and it leaves a bump of a 1/4" long at the start of cut.

[ERUS]

The tool isn't rigid enough. Take a broken half inch long carbide end-mill and have someone grind it for use as a face groove, or grind it yourself.

My experience with face grooving depends on the material and tool. One universal rule is rpm speed is not your friend. I did a face groove in a 9" diameter tub of 6Al4v and ended up going at 25 rpm for the finish pass.

I've noticed on softer materials like aluminum you really don't want a low feed-rate because it causes harmonics and finish issues. My observation is if the tool is always biting then it quiets down. For aluminum, on a finish pass, try a SFM of 25 - 75 and a feedrate of .002" - 0.004 per revolution with a tool edge radius of 0.008", with a edge radius of 0.002" - 0.004" you can get away with a lower feedrate like 0.0005 - 0.0015 per revolution. A larger radius requires a faster feed to keep the tool cutting and not wanting to push away from the material. A sharper edge tool you can get away with a lower feedrate. SFM still needs to be fairly low for the finish pass. And if you can, avoid spring passes because if the tool runs over the part again with out cutting it causes finish issues.

Grooving sucks.

[flick]

Attachment 336496Attachment 336498

Your problem interested me, so in thinking about how I would tackle it, I designed this simple tool.

I think you want a face grooving tool, not a trepanning tool. That way you can take a finish cut on the diameters, as ERUS describes. Luckily, a face grooving tool can be thought of as half a trepanning tool with only one tooth. If you've already built a trepanning tool, you could build this. I thought a 2.5mm/.1" width of cut would be good, leaving about 25 thou to finish on the OD and ID after the initial plunge. Best of luck!

[RCaffin]

I do not know whether this would work or not, but it might be simple to try.
Have you tried using a broaching drill a shade undersize? You would need a fairly heavy machine to get the rigidity of course. Then finish to dimension with smaller tools.

Cheers
Roger

[Black Forest]

What machine tool are you using to do the grove?

[deepaknatraj]

I do not know whether this would work or not, but it might be simple to try.
Have you tried using a broaching drill a shade undersize? You would need a fairly heavy machine to get the rigidity of course. Then finish to dimension with smaller tools.

Cheers
Roger

What machine tool are you using to do the grove?

I haven't tried the broaching drill yet. I have a Haas SL20 and i don't think it's rigid enough to take a broach drill. But I might be wrong.

[RCaffin]

Start the groove with a conventional tool. You would only need to go in a millimetre or two, and it should be a whisker undersize at the ID and OD. That will locate the broaching drill so it does not chatter all over the place. Once it is 'in the groove', it should be OK. Then go very slowly in both RPM and feed - but keep cutting. Don't skate.

Cheers
Roger

[deepaknatraj]

Attachment 336496Attachment 336498

Your problem interested me, so in thinking about how I would tackle it, I designed this simple tool.

I think you want a face grooving tool, not a trepanning tool. That way you can take a finish cut on the diameters, as ERUS describes. Luckily, a face grooving tool can be thought of as half a trepanning tool with only one tooth. If you've already built a trepanning tool, you could build this. I thought a 2.5mm/.1" width of cut would be good, leaving about 25 thou to finish on the OD and ID after the initial plunge. Best of luck!

The trepanning tool I have is made of one cutting edge. It is similar to the design you have. I made it so that it just makes one pass (width of .15"). But I'm getting a bump on the surface where it starts machining.

[ERUS]

I can't find anything off the shelf that can do a 0.15" wide groove by 1.44" deep. I looked at Iscar, PH Horn and Kennametal.

Just for finishing you might be able to grind a 9/64" drill rod or broken endmill. Won't be very rigid but might work just for finishing.

Could also finish by interpolating on a mill with - http://www.harveytool.com/ToolTechIn...mber=982209-C3


All I can think of. Good luck on the part.

[ERUS]

The trepanning tool I have is made of one cutting edge. It is similar to the design you have. I made it so that it just makes one pass (width of .15"). But I'm getting a bump on the surface where it starts machining.

Make the tool smaller than the finish width of the groove. Maybe 0.100" then that leaves 0.025" per side to cleanup. I don't think you will ever get a good groove trying to cut it to finish size in 1 shot.

[deepaknatraj]

I can't find anything off the shelf that can do a 0.15" wide groove by 1.44" deep. I looked at Iscar, PH Horn and Kennametal.

Just for finishing you might be able to grind a 9/64" drill rod or broken endmill. Won't be very rigid but might work just for finishing.

Could also finish by interpolating on a mill with - http://www.harveytool.com/ToolTechIn...mber=982209-C3


All I can think of. Good luck on the part.

Thank you. I'm thinking of grinding an end mill or using a broaching drill like RCaffin Suggested

[RCaffin]

Or, you could just buy the right tool for the job See the top entry here:
https://www.tungaloy.com/us/products...cutting_04.php
Pretty neat cutters, but minimum groove width 0.157". Do they have one which will suit you? Dunno.

Cheers
Roger

[ERUS]

If they made one. The length is almost 10 x the width.

There is only a couple ways he is going to be able to achieve it. Being on a ST20 doesn't help.

If he can get away with the standard .157 \ 4mm, go for it.

Generally its bad machining practice to try and do that in one go. If workmanship isn't a issue then who cares. I'm just trying to tell him the right way to make a nice part. Only he knows what he can and can't do. If its a G-job then its all moot anyways.

[RCaffin]

One sometimes wonders about the people who design these things, without any regard for feasibility. There's a thing called Design For Manufacturability (DFM) which seems to be missing here.

Cheers
Roger