Plunge milling tips

BRIAN.T · Jan 2, 2020

I'm working on a new part, aluminum. this part has an approximately 7" deep pocket 2x3 wide. I'm using an .750 iscar multimaster solid carbide bar with a 3 flute 1/2 loc end mill.

After roughing everything as far down as I can with other tools I've found plunge milling to be the best method to remove the rest, aside from a little chatter against the walls it sounds great, albeit a little slow.... Maybe. I don't often use such long tools, so I'm curious to know what everyone else thinks of my feeds and speeds. I'll be going in tomorrow to kick up the feeds and speeds, I feel like 75 percent step over should be fine... Maybe, For now I'm at.

350sfm (1782rpm)
.0023 chip per tooth (12.3 ipm)
.250 step over
.350 plunge depth.
Total material depth 2.100

Mastercam morph toolpath, if anyone's curious.

litlerob1 · Jan 3, 2020

Why not just use a Drill toolpath? Select points and drill.

IMO your Speeds and Feeds are painfully slow. I'd probably start at 600 SFM (3056 RPM). And feed at .0175"(53.5 IPM). But if I used those Feeds, I would not step over more than 50%. I'm not sure how the Multimaster is going to do with Plunging. The insert ends on a straight shank, but I think the chips will spin off with the higher RPM. I'm assuming "plunge depth" means using a G73 chip breaking cycle, not G83 full retract...

Plunge Milling is fast, fast. If it gives you the impression it's a slow process, that's the fault of the operator. Plunge Milling is/should be scary fast.

R

gregormarwick · Jan 3, 2020

Standard centre cutting endmill geometry is not optimal for plunging. The engagement angle on the face is the wrong side of zero, and the full side engagement causes the chatter you're experiencing.

You can get high feed geometry heads for your multimaster, you should ideally switch out to one of those to get the most out of plunging.

Stick to <30% stepover for plunging, so that you are always cutting near the peripheral edge of the cutter, that way you will not overload the centre and will have better chip control.

You don't say what grade of aluminium, but say for like 6061T6 for example I'd be around 500m/min and ,07mm/t - 8375rpm, and 2345mm/m (92ipm) for a 4 flute high feed geometry head.

BRIAN.T · Jan 3, 2020

litlerob1 said:
Why not just use a Drill toolpath? Select points and drill.

IMO your Speeds and Feeds are painfully slow. I'd probably start at 600 SFM (3056 RPM). And feed at .0175"(53.5 IPM). But if I used those Feeds, I would not step over more than 50%. I'm not sure how the Multimaster is going to do with Plunging. The insert ends on a straight shank, but I think the chips will spin off with the higher RPM. I'm assuming "plunge depth" means using a G73 chip breaking cycle, not G83 full retract...

Plunge Milling is fast, fast. If it gives you the impression it's a slow process, that's the fault of the operator. Plunge Milling is/should be scary fast.

R

I am drilling, in practice anyway. Why create a bunch of drill points when I can just select a drive surface an go. The motion is the same, I'm just using a different toolpath!

As for feeds and speeds, I'm glad to hear that, I'll kick it up based on what you are telling me, but as always, especially with a $1000 tool I like to start slow. As for plunging depth, this would be the depth per pass, so I am plunging the entire path (each hole if you will) .350 deep before moving to the next depth. So the entire pocket gets roughed .350 at a time. My thought is to allow the chip somewhere to go given the stubby length of the cutter. Granted this likely isn't a real issue with the low step over.

Thanks for your advice, I appreciate it!

BRIAN.T · Jan 3, 2020

gregormarwick said:
Standard centre cutting endmill geometry is not optimal for plunging. The engagement angle on the face is the wrong side of zero, and the full side engagement causes the chatter you're experiencing.

You can get high feed geometry heads for your multimaster, you should ideally switch out to one of those to get the most out of plunging.

Stick to <30% stepover for plunging, so that you are always cutting near the peripheral edge of the cutter, that way you will not overload the centre and will have better chip control.

You don't say what grade of aluminium, but say for like 6061T6 for example I'd be around 500m/min and ,07mm/t - 8375rpm, and 2345mm/m (92ipm) for a 4 flute high feed geometry head.

Thanks, I definitely love the idea of high feed for plunging, However, I still need to finish the walls and floors, so high feed is out. I could buy a second tool, but man they are expensive.

And yes 6061.

Mtndew · Jan 3, 2020

BRIAN.T said:
Mastercam morph toolpath, if anyone's curious.

How did you tell Morph to do plunge milling? I love that toolpath.

BRIAN.T · Jan 3, 2020

Mtndew said:
How did you tell Morph to do plunge milling? I love that toolpath.

Yeah morph is the absolute best. It's in" Utility" bottom right of that page. Chain everything as you normally do.

litlerob1 · Jan 3, 2020

BRIAN.T said:
so I am plunging the entire path (each hole if you will) .350 deep before moving to the next depth. So the entire pocket gets roughed .350 at a time.

Might as well use a file or a spoon.

Plunge milling is about moving material fast, not slow-doesn't make any sense. Use Gregor's advice with 30% step over, 100 IPM isn't weird.

Drilling is the fastest way to move material on the Machine. Using a Plunge Milling is theoretically to replicate Drilling but faster, with step overs.

R

michiganbuck · Jan 3, 2020

QT: gregormarwick: [Standard centre cutting endmill geometry is not optimal for plunging.]

I used to end sharpen for plunge milling with adding a couple degrees extra end clearance..and for aluminum avoid small/tight corners in gum-out.

Steel can use 5 to 7* end clearance for plane milling but for plunge 7 to 11 may be better, for aluminum plunge 8 to 15 might do better.

BRIAN.T · Jan 3, 2020

litlerob1 said:
Might as well use a file or a spoon.

Plunge milling is about moving material fast, not slow-doesn't make any sense. Use Gregor's advice with 30% step over, 100 IPM isn't weird.

Drilling is the fastest way to move material on the Machine. Using a Plunge Milling is theoretically to replicate Drilling but faster, with step overs.

R

Haha spoon. I'll give it a try in about 30 minutes, thanks!

Mtndew · Jan 3, 2020

BRIAN.T said:
Yeah morph is the absolute best. It's in" Utility" bottom right of that page. Chain everything as you normally do.

Of all the times I have used that toolpath, I never even knew that option was there lol

Search

Largest Manufacturing Technology Community on the Web

Search

Plunge milling tips

BRIAN.T

Cast Iron

litlerob1

Diamond

gregormarwick

Diamond

BRIAN.T

Cast Iron

BRIAN.T

Cast Iron

Mtndew

Diamond

BRIAN.T

Cast Iron

litlerob1

Diamond

michiganbuck

Diamond

BRIAN.T

Cast Iron

Mtndew

Diamond

Similar threads