What's new
What's new

Torroidal Face Groove

Sith_Machinist

Plastic
Joined
Jan 21, 2024
So I have a few parts to make and 2 of the 3 are done. The third one I got it programmed but tooling im having issues.
If I want to use an OD groove/parting off tool as a face grooving tool, what would be the best way to touch off for the tool. Because no matter how I orient the bar it wont make contact with the tool setter and is definitely way off center. So this is a lathe part. Just a sectional view. I do very little face grooving of any type. Buying tooling is sort of not something my boss will wanna do. And a form tool is also not in the cards as these are for a burner of some sort and the tolerance and finish needs to be spot on.
 

Attachments

  • torroidal tip.jpg
    torroidal tip.jpg
    519.2 KB · Views: 45
If I want to use an OD groove/parting off tool as a face grooving tool, what would be the best way to touch off for the tool.

Chuck up a bar, turn the OD with the side of the grooving tool, measure diameter with micrometer and set X offset that way. Z can be set by touching off on a face at a known Z location like from being turned by another tool on the turret.


I do very little face grooving of any type. Buying tooling is sort of not something my boss will wanna do.

I'd be surprised if your OD grooving tool has enough clearance.

Draw a circle on a sheet of paper with diameter equal to that of the deepest point on the toroidal. Looks to be about 2.5". Hold your tool up to that circle to see if it clears. My guess is that it won't. Face grooving tools are made for a reason.

If you feed only from major diameter to minor diameter maybe you could get away with a tool that just clears the OD of the toroidal. Looks to be about 4"

You might be able to get away with something like a 35 degree insert boring bar.
 
Last edited:
Chuck up a bar, turn the OD with the side of the grooving tool, measure diameter with micrometer and set X offset that way. Z can be set by touching off on a face at a known Z location like from being turned by another tool on the turret.




I'd be surprised if your OD grooving tool has enough clearance.

Draw a circle on a sheet of paper with diameter equal to that of the deepest point on the toroidal. Looks to be about 2.5". Hold your tool up to that circle to see if it clears. My guess is that it won't. Face grooving tools are made for a reason.

If you feed only from major diameter to minor diameter maybe you could get away with a tool that just clears the OD of the toroidal. Looks to be about 4"

You might be able to get away something like a 35 degree insert boring bar.
I thought the 35 degree tool also. Still might end up doing that. But I dont think ill be able to set the x as the tool will be pointing perpendicular to the work piece. I will know better tomorrow.
 
But I dont think ill be able to set the x as the tool will be pointing perpendicular to the work piece.

If it's neutral then you'll need to get creative. But if it's a normal left or right handed boring bar then you should be able to turn an OD with it on a piece of scrap. May require reversing the spindle direction.

Heck, it's a boring bar, so you could use it as-designed and turn an ID and measure the ID to set your offset.

Check the angle between the tangent to the toroidal groove and the Z axis at the inside and outside lips using CAD to make sure the angles on a 35 degree are small enough. Looks OK, but don't want a nasty surprise.

If angle of tangent won't clear the edge of a 35 degree then you'll need to use both an L and an R bar and blend.
 
If it's a neutral 35 deg insert, what I did a long time ago was have our shop wire edm a gage, very similar to a fish gage for threads. It allows for perfect corner alignment. Just manually feed the insert into the wired area while holding the gage to the face/od of the part.
 
  • Like
Reactions: pcd
Still wish my company would bought the proper tooling would have made the job so much easier. And considering I got a quote for the proper tooling would have been like $180. for the bar and 1 button insert. Plus it would give the shop future capabilities.
 
To adapt an OD groove/parting off tool for face grooving on a lathe, you'll need to manually touch off the tool. Mount the tool and bring it close to the part's face, using a feeler gauge or thin paper to set the Z-zero position. For the X-axis, align the tool at the correct radial position by touching the part’s OD and adjusting until it aligns with the groove center, then set this as X-zero. Perform a light test cut and adjust as necessary. Modify your CNC program for precise dimensions and ensure the cutting path aligns with the desired groove. Verify the groove’s tolerances and finish, making any necessary adjustments. This approach, though hands-on, allows you to use existing tooling effectively without new purchases.
Thats exactly what I did. Used a 1" gage block and set it to the z offset of the parts overall thickenss. Worked great.
 








 
Back
Top