Thin groves in stainless.

[traceflair]

I'm trying to come up with an efficient way to complete two operations in 304 stainless steel. The part is .250" thick, 1.5" wide, and close to 3" long, milled square on all six sides with a lot of detail work. It's a part my company produces in rather large numbers, and until I started looking for ways to improve the production, they had a guy make them on a manual Bridgeport. Most of it is a cakewalk, but the two operations that are stumping me are the following:

Top of the part: Two .125" wide grooves with radius bottoms that are 2" long and about .030" apart.

Bottom of the part: 1.944" radius with its center 1.874" off the part, located in the center of the long dimension and expanding the entire width.

I'll start with the bottom first. I've tried setting the part on its side and plunging both a boring bar and a fly cutter down to cut the radius, but I couldn't keep my cutting edge from chipping and dying. Speeds and feeds had no effect on the tool life, so I assume the interrupted cut and inconsistent pressure is the issue. I'm thinking about laying it down flat and trying a G19 G03 arc subroutine with a ball endmill while stepping over, but I'm not sure about speeds and feeds.

For the slots on top, I'm thinking about a ball endmill with either a high feed ramp subroutine or a simple flat cut and step down sub, but not sure on the speeds and feeds there either because I haven't had the opportunity to work much with solid carbide tools and ball endmill chip loads specifically.

Didn't mean for the post to end up so long. Thanks for any insight you guys can provide. Oh, and I'll be doing the job on either my HAAS VF-2 or my VF-4.

[chuck_hobby]

traceflair,
Well you've got me on the ~2in bottom radius and without seeing the part it's hard to tell what the choices could be. I would definitely ramp if using a ball-endmill for the smaller groove...plunging is harder on them, especially the smaller diameters.

Can you post a pic or drawing?
Chuck

[traceflair]

Originally Posted by chuck_hobby traceflair, Well you've got me on the ~2in bottom radius and without seeing the part it's hard to tell what the choices could be. I would definitely ramp if using a ball-endmill for the smaller groove...plunging is harder on them, especially the smaller diameters. Can you post a pic or drawing? Chuck

I don't have a CAD software at home, so I just had to do a rough sketch in MS Paint, which I think I've attached to this post. That's the basic form of the part with the radius on the bottom and the two groves. Hopefully my sketching ability doesn't suck too much to be useful.

The space between the two groves is very small, .060" or something like that, so I'll have to find a ramp angle and feed that will mill the slots without warping the wall between them while also not taking all day long to mill.

I'm quite lost on how to do the radius. I figure I can do a G03 arc in the G19 YZ plane and loop it while stepping over .005" or .010" but at 1.5" wide, that would probably take a while to complete, and it'd be a lot of surface time on stainless for my endmill to endure.

[CNCRim]

I will have the hard time finish the part in two operation, unless you are have multi axis machine like 4 axis machine.

I think it much easy to cut the slot with the saw instead the ball endmill. can feed faster, more rigid less like to break compare to small ball mill.

[Delw]

thats an easy one, just use a slitting saw with a spacer on the blades its a one shot deal two slots/grooves at one time.
Ball endmills suck on stainless way to slow compared to a slitting saw

[traceflair]

Originally Posted by Delw thats an easy one, just use a slitting saw with a spacer on the blades its a one shot deal two slots/grooves at one time. Ball endmills suck on stainless way to slow compared to a slitting saw

The slitting saw is how they did it previously, but they were having a lot of trouble with it because the wall between the slots is so thin. I thought maybe it would be better to do them on the HAAS because the part is on the HAAS already anyway for some holes and things -- one less set up, less man hours, perhaps more reliable in a production run.

[KenFoulks]

I would lay the part as shown in your top left drawing from the spindle point of view. Use spacers, milled soft jaws, or 2 vices. Then, I suggest a 3/4" 4-FL Carbide Flat bottom EM, two or three roughing passes @ 3 Z depths and 1 full length finish cut with a 5-FL EM. I recommend obtaining feeds and speeds from the tool manufacturer with your specifications.

[Delw]

did they run one slot at a time or 2? one wont work running 2 at a time will.
running to slots wont give the other side a chance to bend.

[Cmailco]

What kind of quantities?

That will govern which processes are actually feasible.

You'll need to do a bit of cost analysis: squaring to size vs buying 1/4" x 1-1/2" ground bar. Yes, buying ground flats may be the least expensive option after considering the material, tooling and labor costs involved in machining 5/16-3/8" bar to size.

By the way, what are the sizing, flatness and parallelism tolerances?

Another consideration I would have – and you should ask your engineers – is whether or not 303 SS is a feasible alternative for this particular component. If so, you've saved yourself a bit on tooling and run-time right there.

On to machining,

If using ground flat and a precision sawing operation, you could leave as little as 1/16" on the overall but I usually size it based on the stock length received. In other words, a 12' length (144") at 46 parts, leaves us with 3.130" lengths minus the saw-blade width and a leave of 3.2" for 45 parts, so whichever you feel most comfortable with for the clean-up cuts.

Mill a set of soft-jaws for 1/2" end mill plunge clearance leaving 3" of flat for the part to rest on. Mill the slots down .06 from the rest-portion of the jaw; this gives saw-burr clearance at the ends of the part.



1. Plunge and mill each end to achieve 3.0" length

Quicker slot to ±.005 width tolerance:

Option 1:
Plunge off end of part, 1/8" ball end mill, axial = .3-.5D and slot to the end, retract and repeat till reaching the floor.

This may work ok but 304 is notoriously gummy and varies lot to lot... chip clearing may well be an issue, especially at the bottom of a ball end mill. Needless to say, 2-3 flute would be the better choices.

Option 2:
Use a good square variable-flute end mill (small corner radii) designed for stainless, like Destiny Tool's "Raptor" or OSG's "Aero-UVX" and mill to the center of the floor radius. You should be able to achieve .8-.1 in³/min MRR.

or the fastest option:

Use a trochoidal toolpath and 3/32" 4 flute ball. Plunge to .050 from bottom of slot and take the slot in one trochoidal-slot run.

That's IF you have the CAM software to generate the toolpath, or care to code it manually.

2. Finish slot floor with 1/8 ball end mill.

You will need to do some cost analysis: Milling a slot as mentioned vs fixturing the workpiece to us a ganged slitting saw. I don't see the wall thickness at this height/thickness ratio being an issue either way. Milling looks even better should the material change to 303.

For the large radius, fixture in a set of softjaws with the proper clearance cut into the jaw for the cutter plunges. I'd probably fixture the part so it sits 1" down into the jaw, cut with a 1/2" 4 flute carbide end mill in two passes at full axial depth.

You might need to do a little number crunching to find the least expensive option.

Regards,
Chuck