circle milling oring groove

[bigmousepusher]

Hi, I am trying to mill an oring groove into 0.250" aluminum plate. The oring has a cross section of 0.0625" and is 0.500" ID - 0.6250" OD. I can not find an of the shelf radius cutter, does any body now where I can find one? I would first drill a hole smaller then 1/2" then use that radius cutter to enlarge that hole to 0.520" with an oring groove in the center of the alu. plate. How would you go about programming a CNC mill to do that? Thank you much.

[RICHARD ZASTROW]

Be careful about using circular interpolation to mill an "O" ring groove. Had bad doing that on high pressure hydraulic valve bodies.

The pattern left by the end mill (63 rms) allowed a minute amount of hydraulic oil to leak. The leak eroded the "O" ring and it failed. This happened in a matter of minutes.

Solution was a hollow mill type of tool that left a pattern which laid in the same circle as the "O" ring.

I don't know if this applies in your case, just a "heads up".

Dick Z

[78nova]

PH HORN should have the tool you are looking for. We have one of their cutters and we use it to finish face a part then drop down into the bore to finish a +/-.002 diameter o-ring groove while also holding a +/-.0005 depth to the milled face. The finish is well within a 32.

Kenny

[bigmousepusher]

Thanks 78nova, Horn does have the cutter that I wanted. Can a circle mill cut the profile that I need or do I program one circle, drop down a few thou and cut another circle and keep doing that till I'm done. If I do it that way do I use high speed machining or do I cut rough and than come back and cut finish.

[78nova]

The PH Horn tool I use was selected for its width a radius for cutting the o-ring groove we are cutting. It is wide enough that no extra move ment in Z is required but we do make a rough diameter pass and then a finish diameter pass.

If the cutter you chose from Horn is not wide enough then yes I would make the cuts you described.

If the Horn cutter you chose is wide enough, these cutters will cut full width and depth is asked to do so.

Hopefully you purchased a carbide cutter that screws onto their shank. These tool will run a whole lot faster than you might think depending on your specific situation.

If need be, try using the recommended speed & feed from horn on a scrap piece of material to get a better feel for how these cutters will perform.

Which cutter did you or are you going to purchase?

[bigmousepusher]

I plan on using the MU306 model with the U306.0031.62 insert. It's 0.005" shy of the oring cross section so I will have to cut around twice. I have a lot of holes to do in a few different configurations, so I think I'll do the oring groove cutter in a subroutine and do my positioning with a different program. Never done subroutines but I do have the manual so I don't think it will be a problem. This way I'll be able to use the same subroutine for all my configurations. Thank you guys.