pic: 696 Teaser 1

[sanddrag]

loading photo ...

[DampRobot]

My first thoughts after seeing that shade of green were: "It's 3d printed!" and "It's a render!"

Just curious, what was your CNC setup for those like? What tools/coolant/feedrates did you use, and how did you fixture them? That surface finish on your cuts (under the ano) looks really awesome, did you just go crazy with finish passes or do some sort of tumbled finish before anodizing?

[sanddrag]

Originally Posted by DampRobot

My first thoughts after seeing that shade of green were: "It's 3d printed!" and "It's a render!"

Just curious, what was your CNC setup for those like? What tools/coolant/feedrates did you use, and how did you fixture them? That surface finish on your cuts (under the ano) looks really awesome, did you just go crazy with finish passes or do some sort of tumbled finish before anodizing?

HAAS MiniMill. Trim C350 coolant at 7% Brix, 4 streams high pressure flood. Lakeshore carbide 1/4" 3fl ZrN coated endmill. 10% Stepover. 6000 RPM. 120 IPM pocketing. 0.010 finish pass at 60 IPM. No tumbling or anything. Just a deburring knife on the edges.

We fixtured by just bolting it down to a fixture plate that we drilled and tapped with a few holes.

[DampRobot]

Originally Posted by sanddrag

HAAS MiniMill. Trim C350 coolant at 7% Brix, 4 streams high pressure flood. Lakeshore carbide 1/4" 3fl ZrN coated endmill. 10% Stepover. 6000 RPM. 120 IPM pocketing. 0.010 finish pass at 60 IPM. No tumbling or anything. Just a deburring knife on the edges.

We fixtured by just bolting it down to a fixture plate that we drilled and tapped with a few holes.

120 IPM pocketing? I'm jealous, I usually consider myself lucky if I can get 20 IMP. Of course, that's with a something like 50% stepover and non HSM toolpaths...

[Gray Adams]

With a MiniMill, why not just do the deburring as part of the machining? Or did you, and the deburring knife was for the backside?

Looks incredible though, I never would have thought you didn't do any surface finishing like bead blasting or tumbling.

[sanddrag]

Originally Posted by Gray Adams

With a MiniMill, why not just do the deburring as part of the machining?

We ran a corner rounder on last year's plates, but it just takes too long. As shown, machine time was 22 minutes per plate. Adding corner round would be another several minutes. We can have a person deburring while the machine is running another part.

[Cory]

Originally Posted by sanddrag

We ran a corner rounder on last year's plates, but it just takes too long. As shown, machine time was 22 minutes per plate. Adding corner round would be another several minutes. We can have a person deburring while the machine is running another part.

You should be able to deburr with a chamfer mill in under 45s for the entire part.

I'm curious how you're getting a 22 minute run time, given those speeds. Our plates are generally similar and are more like 10 min with more conservative speeds/feeds.

[sanddrag]

Yeah, a chamfer I could run at 40 IPM but the corner rounder I usually run at about 12. The long run time may be due to the 10% step over and the machine acceleration/deceleration on all the HSM moves. Iirc, the inside pockets ran about 13 minutes. I ran the bearing bores rather slow, and probably spent too much time going helical around through air with a plunge clearance of too high. What speed do you helix in and what helix ramp angle?

[Cory]

Originally Posted by sanddrag

Yeah, a chamfer I could run at 40 IPM but the corner rounder I usually run at about 12. The long run time may be due to the 10% step over and the machine acceleration/deceleration on all the HSM moves. Iirc, the inside pockets ran about 13 minutes. I ran the bearing bores rather slow, and probably spent too much time going helical around through air with a plunge clearance of too high. What speed do you helix in and what helix ramp angle?

My strategy with gearbox plates is to not pocket and to contour slugs that drop out. You have to do this in the vise operation before you bolt it to your toolplate though.

At any rate I don't think HSM is gaining you much there. You could easily run 40% stepover full depth at 6k RPM and 54 IPM and only be limited by the rigidity of your machine, which I think would be fine. I routinely run those same parameters except at 10k RPM and 100 IPM.

I try to pre-drill plunge points for all my pockets whenever possible, to avoid potential edge chipping during plunging or the added time of helical entry. When I do helix I use the feed speed and 2-3*.

[Mk.32]

Originally Posted by Cory

My strategy with gearbox plates is to not pocket and to contour slugs that drop out. You have to do this in the vise operation before you bolt it to your toolplate though.

At any rate I don't think HSM is gaining you much there. You could easily run 40% stepover full depth at 6k RPM and 54 IPM and only be limited by the rigidity of your machine, which I think would be fine. I routinely run those same parameters except at 10k RPM and 100 IPM.

I try to pre-drill plunge points for all my pockets whenever possible, to avoid potential edge chipping during plunging or the added time of helical entry. When I do helix I use the feed speed and 2-3*.

$@#$@#$@#$@# I wish I had an machine that could do 10k.....

I was just running some parts similar to this on a Tormach P1100 was getting up to 5000rpm, with .1 DOC @ 50ipm with a 2 flute carbid 1/4 70% stepover. Just without HSM toolpathing which doesn't seem to gain you for a lot of the parts we have to run. Though I was doing a full pocket since I already was bolted to a tooling plate.