Milling Deep pocket ?

[david parkhurst]

I have been working on trying to mill a deep pocket in a oil pan project with not much luck , I'm looking for some input on type of cutter you may have used, feed and speeds . not only the in side ; the out side too (deep milling over all ) Tormach 1100 alum 6061 Thanks Dave P 3.400 in pocket at the deep us point

Similar Threads:

• Deep pocket milling
• Need Help!- Deep Pocket Milling
• Not very deep pocket problems
• Deep Pocket In Aluminum
• milling deep pocket

[IMT]

How deep is the pocket?
If I were doing this I would:
1) Use the Tormach 25mm insert cutter with the short holder. This gives a reach of 1.9", run at 2500rpm, .100DOC, .700WOC, 50IPM. Reduce to 35IPM for full slotting.
2) Use the Tormach 25mm insert cutter with the medium holder. Reach is about 3.5", run at 3500rpm .030DOC, .700WOC, 70IPM.
3) If it's deeper that that, a 3/4 endmill directly in the R8 collet. Plunge cut for roughing followed by very light finishing passes. I've done that with a 3" flute length EM sticking out 4.5" from the spindle.
Good luck.

[ERUS]

Personally I would go with a extended reach. I'm not sure what size the radius in the corners is, which impact the diameter tool you would need, but something like this would work.

1/2 Inch Diam, 0.02 Inch Radius, 5/8 Inch 02856409 - MSC.

The corner radius should allow you to radius the bottom corners. I would go with as short a flute as you can because this greatly increases the rigidity of the tool. I've run these at 10K rpm and maybe 80 or 90 IPM without causing harmonic issues. I personally didn't think something that long would do it until I tried.

[Steve Seebold]

Can you give us a better discripton of what you are trying to do. What's the material? How deep? Give us more information.

[IMT]

Can you give us a better discripton of what you are trying to do. What's the material? How deep? Give us more information.

The OP does state the material as 6061 and the max depth at 3.400. Somehow I missed the depth part too.

With a depth of 3.400 I would use the Tormach 25mm insert tool as described above for roughing. Plunge rough the corners with the appropriate size EM (assuming the corner rad is smaller than .500"). Then use a corner radius EM with the right size cr to finish the walls and bottom, although the bottom to wall radius looks about the same as the corner, so you might have to finish the walls with a ball end mill and finish the bottom with a corner rad EM.

[david parkhurst]

Radius could be as high as .750 on the in side . 6061alum bottom is 1.5 down to 3.4 New pic are the pan I'm currently making cnc flange rest is sheet metal welded up .,

[SCzEngrgGroup]

Looking at that thing, I'm wondering why you would want to mill it, rather than just welding it up as in the photos. The welded assembly will be FAR cheaper, and quicker, to fabricate.

That said, I'd find a long, large diameter insert endmill to do the roughing, then an extra long regular endmill for the finishing. Or you might find a corner-radius insert endmill for finishing as well. On a Tormach, it will take a looooooong time to machine. Finishing will be very slow indeed, due to the use of very long tools. discount-tools.com has many endmills up to at least 4" long for very reasonable prices. You'll want carbide, for the extra stiffness.

One way to greatly simplify and speed-up fabrication would be to split the part vertically into two pieces that bolt together. That would allow you to angle the parts to eliminate machining steep walls, and reduce the amount of waste. I'd bet that would cut machining time almost in half, and allow use of shorter tools.

Regards,
Ray L.

[RussMachine]

If you have a manual mill, drill out as much material as possible, before trying to finish-mill that deep.
Drilling is the quickest, and easiest way to remove material.

[IMT]

Radius could be as high as .750 on the in side . 6061alum bottom is 1.5 down to 3.4 New pic are the pan I'm currently making cnc flange rest is sheet metal welded up .,

If the corner radius can be .750 then this is very doable. I see now that the bottom is sloped so you will have to profile that with a ball end mill. So I would rough with the insert cutter then finish the sides and profile the bottom with a 3/4" ball endmill directly in the R8 collet. It will take a while and make a big pile of chips but you can get it done on your 1100.

[Steve Seebold]

I would create a hole pattern, drill the first hole then use an end mill and take a 30 to 40% step over and go straight down. You'll find you'll remove a lot more material faster than you can by conventional milling.

I have tone pocketing this way for years, and you can feed straight down at 30 to 50 inches per minute because all the tool pressure is against the spindle.

[Steve Seebold]

Looking at that thing, I'm wondering why you would want to mill it, rather than just welding it up as in the photos. The welded assembly will be FAR cheaper, and quicker, to fabricate.

That said, I'd find a long, large diameter insert endmill to do the roughing, then an extra long regular endmill for the finishing. Or you might find a corner-radius insert endmill for finishing as well. On a Tormach, it will take a looooooong time to machine. Finishing will be very slow indeed, due to the use of very long tools. discount-tools.com has many endmills up to at least 4" long for very reasonable prices. You'll want carbide, for the extra stiffness.

One way to greatly simplify and speed-up fabrication would be to split the part vertically into two pieces that bolt together. That would allow you to angle the parts to eliminate machining steep walls, and reduce the amount of waste. I'd bet that would cut machining time almost in half, and allow use of shorter tools.

Regards,
Ray L.

If you're gonna do it that way Ray, why not make it out of 6 pieces and weld it together.

[SCzEngrgGroup]

If you're gonna do it that way Ray, why not make it out of 6 pieces and weld it together.

Did you not bother to read ALL of my post? Did I not recommend exactly that as the most cost-effective approach?

Regards,
Ray L.

[AUSTINMACHINING]

I have been working on trying to mill a deep pocket in a oil pan project with not much luck , I'm looking for some input on type of cutter you may have used, feed and speeds . not only the in side ; the out side too (deep milling over all ) Tormach 1100 alum 6061 Thanks Dave P 3.400 in pocket at the deep us point

That's a lot to hog out.if your going for asthetics, I would do through outside first, them use a 1/2" 2" long end mill, helix to 1/2" deep, HSM out to the edge. Repeat until you run out of flute length. To go deeper, I use a long 1/2" reduced shank end mill made by YG-1. Cutting will be light at those depths.

Thats with my current tooling. I would like to try a AB tools single tooth shear hog. Put the long 3/4" shank directly in the R8 collet and plunge rough the hell out of it. They have videos plunging in Z. That will,probably be,my next tool purchase, however that would be pushing these little machines hard, and may not have the rigidity/horsepower to do the tool justice.

[tmarks11]

Looking at that thing, I'm wondering why you would want to mill it, rather than just welding it up as in the photos. The welded assembly will be FAR cheaper, and quicker, to fabricate.

That said, I'd find a long, large diameter insert endmill to do the roughing...One way to greatly simplify and speed-up fabrication would be to split the part vertically into two pieces that bolt together.

If you're gonna do it that way Ray, why not make it out of 6 pieces and weld it together.

Too funny!

A swing and a miss...