Plunge Roughing - speeds/feeds guidance

[jmcglynn]

I have a small part I'm making, it's about .75" x 2" outside, 1018 steel.

I'm currently using a pocketing operation on the inside area -- the part in blue in the screenshot. With a .1875" 4 flute carbide EM, .015 DOC and 30 ipm it's taking like 15 minutes to clean this out. The interior is .537" by about 1.5 and I need to go .5" deep.

Waaaay too long for this part.

I'm going to try plunge roughing to speed this up, using a .5" carbide NC counterbore (essentially a flat bottom drill, no pilot).

Any recommendations on depth of cut, rpm and feed (plunge)?

At 400sfpm and .00275 CPT I get 3055 RPM at 33 IPM. Assuming a pecking operation at a .1 DOC, this would be under a minute to rough it, and maybe another 2 minutes to clean up the walls. Much better.

Anyone have some experience with this?

[dertsap]

why are you only taking a .015 depth of cut ?
could you not ramp in a .5 endmill with a .025 to .05 ramp then come in with a finish endmill to clean up the rest , it would be much quicker than plunging

[masonbcaldwell4]

Drill a hole down through, then use a .5" coated roughing mill to take the whole DOC in one, running about 200-300 rpm and 0.7 ipm feed. just keep it flooded.

[jmcglynn]

Originally Posted by dertsap why are you only taking a .015 depth of cut ? could you not ramp in a .5 endmill with a .025 to .05 ramp then come in with a finish endmill to clean up the rest , it would be much quicker than plunging

Oh, totally. I ran the initial parts this way to verify the design with the cutters I had on hand, now I'm looking for the fastest way to get the job done so I can blast out a bunch of these.

What I've read so far leads me to believe that plunge roughing will be faster than ramping in by a bunch. I could be wrong, that is why I'm asking.

At the same feed rate with a 7 degree ramp in the operation is about 50% longer than plunging, but I'm guessing on feed rates for plunge roughing right now, so that may not mean anything. Either approach is considerably faster than cutting the whole thing out with a 3/16 cutter

[dertsap]

i believe that plunge milling is a good way to remove materials in large parts with hard to machine material but if you calculate a .5 endmill ramping .05 dp at 20 -30 ipm with a distance of 1" ,how long will it take ?

[jmcglynn]

Originally Posted by dertsap i believe that plunge milling is a good way to remove materials in large parts with hard to machine material but if you calculate a .5 endmill ramping .05 dp at 20 -30 ipm with a distance of 1" ,how long will it take ?

Ramping, 7 degrees, .050 doc, 30 ipm = 110 seconds

Plunging, .1 doc (pecking), 30 ipm = 53 seconds

Like I said, both are way better than 15 minutes (plus ~ 3 minutes to clean it up and get into the small spots.

I'll try it both ways and see how it works out in practice. I've got about 100 of these to make, so a minute matters.

[dertsap]

it would only be 22 seconds
with a .05 depth of cut you would need to take 11 passes 30ipm = 2sec/inch
i wouldn't push it quite so quick with a standard carbide