Machining Internal Corners / In Corner Cutting

[MJ2005]

We are having relatively small cylindrical components CNC machined out of 316L stainless steel. We are using a 30-taper machine. We would like to machine a small rectangular slot in the rim of the component, the slot measuring approximately 0.6" in length by 0.08" in height. It would need to penetrate through a rim wall thickness of approx. 0.16". We would like the slot to have sharp internal corners (90 degrees, or as close to that as possible). Is there any practical way to achieve this on a 30-taper machine? Could the corners be broached in a secondary operation? Because we are planning on machining several thousand of these, the least cost method for volume production is preferred. Any advice or suggestions would be much appreciated.

 

[DAVIDSTECKER]

If you have a sharp cornered "key" that goes into the slot you might run the end mill out of the corners at 45 deg to allow the corners of the "key" to clear. It would make the slot look like it has Mickey Mouse ears but if it works who cares. It also relieves stress concentration.

 

[MJ2005]

Thanks for the reply, David. Unfortunately, I forgot to mention that cosmetics is of some concern, so that, from the exterior of the component, the slot must have a rectangular outline -- no Mickey Mouse ears allowed! Good idea, but it won't work for our particular situation.

 

[aamoroso]

Sounds like you may be best off drilling a .02 hole in the corners then rough the slot with a .06 end mill, followed by a finish cut with a .032 end mill. Follow up with a file to hit the corners, you will only have to remove about .01 - .015 with the file. (Downside to that is you will most likely have some broken drills stuck in parts to deal with).

Another option (depending on the component) may be cutting it on the side using a key cutter, rather than on the top with a conventional end mill.



Fill what's empty. Empty what's full. And scratch where it itches.

 

[BillPSU]

What is the orientation of the slot to the tube. Is the slot through the OD into the ID or through the end of the tube? If the slot is through the OD is the milling to be done radially by rotating the part or straight through?
If the slot is straight through a tool could be made to the finish size of the slot. For lack of a better description lets call it a punch. The punch could have back taper on the outside and a radius ground in the end to give some primary clearance. Some machining centers allow the locking of the spindle in one orientation which is the tool change position. You will have to check if your machine is capable of this. Put the punch in the spindle and adjust orientation of the tool and basicly punch the hole after you rough machine the slot. You may need multiple punching tools to maintain the corner radius.

 

[MJ2005]

Bill:

In answer to your question, the slot will be milled from the OD of the cylinder into the ID (along a radial line emanating from the primary axis).

Do you think the punch idea is superior to a broaching operation?

AAmoroso:

I see your point, but sounds a little tedious if we're producing a few thousand. We're looking for something a bit more automatic, and a process that we wouldn't have to continually be measuring to make sure we were within tolerances.

Thanks for all info.

 

[CSLufkin]

If your spindle will lock in the oriented position (Usually M19) you can use a small square punch and move it into position to punch the four corners separately (after it is rough machined). This way you have size adjustment and are not dependent on the size/shape of the punch. The only lookout is that the tube may bend in slightly if you dont put a mandrel inside before punching.

 

[unclesyd]

I don't believe that you will be able to mechanically form your notch with any degree of repeatability. I believe that your best bet will be to EDM the slot in a secondary operation.

Are the ends of the slot going to be radial or can they be parallel to each other?

Aside from the implied accuracy what is the required accuracy?

 

[BillPSU]

MJ2005
The punch I am talking about is basicly a broach with a single cutting edge. A true broach probably would not work due to the required length of the broach and size of the slot. You were also looking for a tool to use in a machining center. You have also not talked about the tolerance or finish of the slot. I have used punchs to cold work material before. When punching holes there is breakout with the punch entry side being the size of the punch and the exit side being the size of the die. This condition is not acceptable for some self tapping screws. I have punched the holes undersize and then repunched the hole with a on size punch cold working the ID. Punches suffered due to galling but avoided a drilling operation on these types of holes.

 

[griffengm]

MJ,
If I understand your issue correctly, you want each side of the notch to be on a radial fron the center of the part.
The tool path of an end mill would be a vee offset inside the vee formed by the radials of the notch edges.
I suppose it can be done on your turning center if you can turn the work through the arc needed or if run as a second operation.
My apologies if I misunderstand.

 

[jbel]

We're looking for something a bit more automatic, and a process that we wouldn't have to continually be measuring to make sure we were within tolerances.

How else would you know if it is in tolerance???