Pocketing Strategy

turbotadd · Nov 1, 2016

I've got a bunch of parts to run with 100 or so of these pockets per part. Material is MIC-6. Machine is a '96 Tree VMC 500, 8k spindle. How would you go about pocketing these?
Thanks!

TeachMePlease · Nov 1, 2016

I'd try a 1/4" endmill trochoidal right through, if your machine and CAM and tolerance on the .250" width can handle it.

Atomkinder · Nov 1, 2016

I'd probably just ramp the whole thing with a 1/4" 3-flute at 3° with a maximum stepdown of .200" or so depending on how good your chip clearing is. MIC-6 is easy stuff to machine. Full 8k RPM, about .003"/flute.

Mechanola · Nov 1, 2016

Drawing sais through opening, not pocket.

Drill with a Y bit on one side, then enter [SUP]3[/SUP]/[SUB]16[/SUB]" endmill and do the rest in one pass.

Finegrain · Nov 1, 2016

Mechanola said:
Drawing sais through opening, not pocket.

Drill with a Y bit on one side, then enter [SUP]3[/SUP]/[SUB]16[/SUB]" endmill and do the rest in one pass.

Yes, this. Slam a 3/8" drill bit 3X, then finish with a 3/16" EM.

Regards.

Mike

Atomkinder · Nov 1, 2016

Mechanola said:
Drawing sais through opening, not pocket.

Drill with a Y bit on one side, then enter [SUP]3[/SUP]/[SUB]16[/SUB]" endmill and do the rest in one pass.

At 3.33xDia? You must have magic end mills!

Finegrain · Nov 1, 2016

OK, not one pass :crazy:

. Gotta whittle open the channels first with some HSM/Dynamic toolpath.

Regards.

Mike

CarbideBob · Nov 1, 2016

Basic rule is saw, drill, turn, mill, grind.
Saw and turn won't help here.
I'd drill three 3/8 holes and two 3/16 holes then mill....maybe.
Or three 10MM holes, end two offset a tad, and two 5MM holes which would be just a touch faster at the mill op.
Option three being one 3/8 hole and then plunge rough with a 3/16, then finish the walls which does not leave that "fin" of meat between holes to grab your endmill and break it.
Laying this out and programming without a CAM that automatically does it would be a lot of work but maybe worth the time.
Thinking a 96 Tree is not gonna be great at HSM trochoidal tool paths as a lot of time would be spent cutting air but it also may not be real fast at the plunge rough option also with all the Z retracts doing nothing.
Bob

Mtndew · Nov 1, 2016

Blast a hole in there,you only need 1 hole, rough with a HSM style toolpath (full depth), and 1 finish pass.

G00 Proto · Nov 1, 2016

If it wasn't mic6 and I had flood coolant, I would just ramp the whole thing with a 1/4" EM.... but Mic6 can be very gummy and loads up endmills badly. So, I would drill the holes with a gurhing stub 3/8" drill; ramp a straight line through the web areas that remain with a 3/16" EM back and forth at 3 to 6 degrees, then do a cleanup pass around the entire ID. I would try taking the entire cleanup pass in one shot and see how it looks... most likely 2 Z passes and one .005" cleanup in the XY, depending on the cosmetic requirements.

Mic6 is gummy, you may need to use extra concentrated coolant or cutting oil.

CarbideBob · Nov 1, 2016

Mtndew said:
Blast a hole in there,you only need 1 hole, rough with a HSM style toolpath (full depth), and 1 finish pass.

All fine and crazy fast on a linear motor 2 million dollar machine tool where total time here is way under 60 seconds.
Note the machine being used......The op has what he has.
Bob

Matt@RFR · Nov 1, 2016

CarbideBob said:
Thinking a 96 Tree is not gonna be great at HSM trochoidal tool paths as a lot of time would be spent cutting air but it also may not be real fast at the plunge rough option also with all the Z retracts doing nothing.

Bingo, especially when it comes to HSM with a tool that is not much smaller than the feature... it's going to be moving slow, and it's going to choke on the code too (from my limited experience with these machines). The tree will not run out of horsepower with a 3/16" or 6mm (my choice) endmill, so back to the old school ways for this kid if this was my part. Drill one 3/8" start hole, drop in and go. Experiment with how much DOC you can get away with and if you have a lot to do, use one feedrate while fully engaged, then another, faster feedrate on the way back to the start hole.

Mtndew · Nov 1, 2016

CarbideBob said:
All fine and crazy fast on a linear motor 2 million dollar machine tool where total time here is way under 60 seconds.
Note the machine being used......The op has what he has.
Bob

HSM paths aren't only for the newer/faster machines. They are still very efficient no matter what machine you run them on. Don't have to go 1,000 IPM with these paths :nutter:

triumph406 · Nov 1, 2016

I would drill 3 Y or Z dia holes as suggested. Then break the web between the holes by stepping down maybe .075-.100 at a time. If I don't break the endmill then increase the step down. One it's broken thru, run around the periphery, maybe step down in 2 steps leaving .002-.005, then 2 finish passes. I'd use a 6mm dia 2/3 flute endmill if availible.

I'd have the coolant nozzle(s) pointing down the length of the part as well.

Mike1974 · Nov 1, 2016

Depending on tool change time, it might be faster to helix bore with the same tool you cut the rest of pocket with.

edit: disregard, I misread the post, if he has 100's of pockets per part, tool change is insignificant...

G00 Proto · Nov 1, 2016

Just to reiterate. He is running an old slow machine with limited processing power. I doubt he has flood coolant, and if he does it probably very low flow. Mic6 can be as gummy as A356 castings... since it is cast plate. I would spend as little time as possible with full width engagement, and as much time as possible out of the cut in the drilled holes to get my tool cooled back down and lubricated.

Drill the holes with a high zoot drill (Gurhing or MA Ford stub carbide) going as fast as I can.

Break down the web with a 2 flute 3/16" carbide endmill (better gullet depth)

Do an old school contour and clean it up.

Or best option... set the entire plate up on a water jet and cut all the profiles and inner pockets at the same time. Expensive option, but it's gotta get blanked out any ways. Then just finish with whatever endmill would fit. Cheat the tolerance and you can get a 1/4" EM in there.

rlockwood · Nov 1, 2016

Mtndew said:
HSM paths aren't only for the newer/faster machines. They are still very efficient no matter what machine you run them on. Don't have to go 1,000 IPM with these paths

Indeed, the biggest advantage HSM gives is the ability to tweak an operation to suit the limiting circumstances. The ability to utilize horsepower when previously a limiting factor prohibited it.

MK Proto · Nov 1, 2016

I would helix down with a 6mm tool with a .2" ramp down per profile leaving .005 per side and finish with the same tool full depth.

Pocketing Strategy

Aluminum

Diamond

Titanium

Stainless

Diamond

Titanium

Diamond

Diamond

Diamond

Hot Rolled

Diamond

Titanium

Diamond

Diamond

Diamond

Hot Rolled

Stainless

Hot Rolled

Similar threads