Plunge rough... d yo guys use it?

[snowshooze]

It seems a bit harsh to me, when I have to, I use it, but with a drilled starter hole.
Generally, I make all my end mill entries into material, perpendicular.
Thanks,
Damn, keyboard is due for replacement..
Mark

 

[mhajicek]

I think highfeed cutters have made plunge roughing largely obsolete.

 

[Milland]

I think highfeed cutters have made plunge roughing largely obsolete.

Maybe. I could see when you're dealing with a flexier machine and cutting deep features how plunge cutting might still be preferable.

 

[gregormarwick]

I think highfeed cutters have made plunge roughing largely obsolete.

Plunge roughing - with high feed cutters - is an extremely efficient way to remove material. If you are trimming the edge off a plate for example, you can plunge rough the material off in a fraction of the time using the same tool as you would to high feed it.

It is by far the fastest way to rough material at very high LxD. Caveats are that it is not so great cutting down to a flat floor, and there needs to be a good route for chip evacuation.

 

[kenton]

I use it for rough facing acrylic to keep the edges from blowing out.

 

[Jashley73]

It works great for long tools. Doesn't need to be a high-feed cutter, or even a specially-designed plunge-milling cutter. (Though the do even better.) You can do it with any square-shoulder cutter really.

 

[snowshooze]

It appears I need to look into high feed cutters...
Thanks!
Mark

 

[Eric U]

Any particular reason you have two threads on the exact same topic?

 

[michiganbuck]

Back when I was making dies would plunge an end mill to near depth, and the finish with conventional milling, I thought the method saved at least 1/3+ the time. Good to have an endmill in an end mill holder, and pulled down against the double piggyback set screw. and a little extra end clearance on a center cutting end mill, 9 or 10* seemed good.

Nowadays I would likely make a touch/spot depth probe to see my depth as it seemed what turn to stop in was always a worry when doing that.

 

[snowshooze]

Any particular reason you have two threads on the exact same topic?

Yeah, because it was on my to-do list to check and see if I was leaving a good strategy of chip removal left rarely used... wondered if I was doing something wrong.
A duplicate thread, and I can't figure out how to get rid of it...
Sorry.
Mark

 

[Scruffy887]

In the past I used it with a plunge insert tool. It just munched away and saved me a ton of time on that part. Chip exit is key. All I did was waste away a big corner on 1 x 5" bar stock. I like chips that ring if dropped on he floor.

 

[snowshooze]

In the past I used it with a plunge insert tool. It just munched away and saved me a ton of time on that part. Chip exit is key. All I did was waste away a big corner on 1 x 5" bar stock. I like chips that ring if dropped on he floor.

A plunge insert tool...
You got me there.
I will look forward to maybe you putting me on to one?
Thanks!
Mark

 

[CarbideBob]

I plunge rough almost always when making toolholder pockets on a B-port.
Not so much on the cncs but sometimes.
Nothing fancy, just pain endmills.
Bob

 

[gregormarwick]

A plunge insert tool...
You got me there.
I will look forward to maybe you putting me on to one?
Thanks!
Mark

Although plunge milling is still a useful strategy, actual plunge mills seem to be getting phased out. Most of the big names might still have one hanging around in their lineup, but they are all older tools that are not getting updated.

The reason being that high feed mills generally work just as well when plunging and are not a one trick pony like plunge mills. The caveat is that real plunge mills can stepover much more than a high feed mill and leave a flatter floor, but those are pretty small concessions in reality, unless you are using a 50 taper machine with lots of torque and rigidity that can actually handle the larger stepover.

It works great for long tools. Doesn't need to be a high-feed cutter, or even a specially-designed plunge-milling cutter. (Though the do even better.) You can do it with any square-shoulder cutter really.

While true, I'd add for clarification that most modern/contemporary shoulder mills cannot plunge, and you will wreck them if you try.

 

[BugRobotics]

I use plunge milling on the smaller Hermle when doing deep stuff on harder materials. I pattern cylinders along the profile I want to cut and use a drilling toolpath in HSMWorks. Works fine.

 

[empower]

Plunge roughing - with high feed cutters - is an extremely efficient way to remove material. If you are trimming the edge off a plate for example, you can plunge rough the material off in a fraction of the time using the same tool as you would to high feed it.

It is by far the fastest way to rough material at very high LxD. Caveats are that it is not so great cutting down to a flat floor, and there needs to be a good route for chip evacuation.

wait what? plunging with high feed mills?

 

[Scruffy887]

A plunge insert tool...
You got me there.
I will look forward to maybe you putting me on to one?
Thanks!
Mark

I will check when I get back in the metal shop. Just a WAG but I think it used standard inserts turned 90 degrees. I tested the 2" plunge on a piece of 1x3 bar stock. It made a lot of normal noise as it started plunging in. But once it was 1" in it was very quiet. Cutting thin to thin.
Some CAM packages even had PLUNGE routines where the cutter would plunge and back away slightly on retract. Cutter does rub when retracted straight up without this. Not an issue for my use.

 

[Snoopy-16]

I'm looking into this technique for a 5 axis job I have coming up:
It's in 6061 Aluminum and I'm looking at using a 16mm (5 x D) U'Drill to create a series of narrow 75mm deep pockets. I have powermill to create the plunge milling cycle, however it seems really 'clunky' at working within pockets, so I might just manually program the plunges using drilling cycles.
For those that have previously used plunge milling, did you see any real benefit in doing so? Perhaps I should just ramp in and trocidal rather than try something new...
ps. I am running a haas UMC750 with an HSK63 spindle

 

[michiganbuck]

I think the advantage of end plunge milling is by far the fastest method to make a cavity in a steel part. It also saves the endmill from side wear.
The cutting forces are much better applied than the forces being applied to the side of the cutter where deflection is included.
Pull out should be considered so end mill holders are much better than collet holding cutters. Collet holding end mills leads to babying every job.
Plunge is best served with end mills having center cutting geometry and end primary clearance a few degrees greater. The thin-ribbon chip suggests the end mill does not have enough clearance, 9 to 13* is often a better end primary clearance for plunging.