[TomL21]

I'm working on a part with some small face grooves, the largest groove diameter is .250, followed by: .188, .125 and .0625. They are .010 to .015 deep and are a triangular shape (think of a 60deg threading tool). The .250 and .188 dia grooves come out pretty good. The smaller ones get wiped out by the backside of the threading insert I'm using. We've clearanced the backside quite a bit, and are working on even more but I don't think the tip will hold up. Has anyone here done something similar? What tools have you seen/used to make grooves like this. I'm pulling my hair out on this one. Any help would be greatly appreciated.

[John Welden]

I'm working on a part with some small face grooves, the largest groove diameter is .250, followed by: .188, .125 and .0625. They are .010 to .015 deep and are a triangular shape (think of a 60deg threading tool). The .250 and .188 dia grooves come out pretty good. The smaller ones get wiped out by the backside of the threading insert I'm using. We've clearanced the backside quite a bit, and are working on even more but I don't think the tip will hold up. Has anyone here done something similar? What tools have you seen/used to make grooves like this. I'm pulling my hair out on this one. Any help would be greatly appreciated.

You could draw the cutter in cad to figure out what it needs to look like.

Or use a live tool.

[TomL21]

Thought about the live tool, but with out breaking into high production lines the only machine available is an old SL-1A.

I started to draw it up quick after the first trial. Waiting on that to get ground. We're afraid there wont be enough material to support the tip and it'll just break off.

[PixMan]

I've had to do this a few time on CNC screw machines. In the end, I found no bought tool that would do it so I took a Micro 100 carbide "blank" boring bar (a round with a half-round ground on one end) and made a tool by hand on an Agathon tool grinder. I eyeballed a 30 degree conical shape to a point, then flatted-off the other 30 degree angle.

The part I was doing had concentric face grooves from the first at .035 diameter out to .160, .012~.015 deep at .025 distance between centers of the grooves, max .002r at the bottom of the grooves, in 303 stainless. One tool made whole 300 pc order...but it wasn't the first tool.

[TomL21]

PixMan, I ended up with something very similar I think. I had a tool made in the tool room, looks like a 60deg (included angle) engraving tool. Basically a 1/4 diam carbide shaft with half of of 60deg cone on the end.

I cut the first few test pieces, it seems to cut very well. At least it makes nice clear, distinct grooves. They are running tonight so we'll see how the tool life looks. I'm going to have some made up with flats so it's easier for the operators to orient the tool when replacing.

[crabbass]

Try shimming your tool so it is above CL. If you are doing high production I agree a custom grind would be best, however the custom tool will most likely look just like the threading tool , just rotated a bit. by moving your tool above CL it will rotate the relief angles, and change the rake as well. you can customize the rake easily enough by hand. If the diameter tolerances of your groove are fairly tight, you will find that .001" offset doesnt equal .001" offset on the part. You might have to offset .0013" to obtain a .001" change in your parts size( This would be easy to calculate once you find the right shim height)

AC

[TomL21]

Our custom grind looks more like a single flute engraving tool (like this tool from Harvey Tool) instead of a threading insert. I had a tried a few configurations with a thread mill to do it in one shot, tried shimming it either way and also rotating it out of the cut, didn't work out well. We also modified a top-notch threading insert for more clearance on the back, but we started to grind into clamp area of the insert before we gained any improvement in the cut. The custom grind is working very well, nice clean cut and holding up well in production. The grooves only serve to provide traction for your finnger. Thank you for the help!