anybody plunge milling?

[rsbeadle]

I occasionally plunge mill when cutting deep pockets, but I don't use it very often because of the wear it puts on the machine spindle. The Carboloy rep came by recently and asked why I wasn't plunging everything with their feed mill. I told him if he will send me a new spindle every six months or so I would be glad to. Is anybody out their plunging on a regular basis with a 40 taper machine and not trashing spindles? Thanks

[Code_Breaker]

no problems here . . . what tool are you using? Step over? feed rate/rpm??????

 

In fact, since the pressure is vertical to the spindle, it is actually better, in some cases, than side milling.

[Thad]

I've often wondered about this. Isn't there still a lot of pressure on the spindle? Compare these 2 operations and see what puts more pressure (wear) on the spindle (concept wise). Drilling a hole and plunge milling. When drilling, there is full diameter pressure on the Z axis. When plunge milling, there is side load (deflection) along with direct Z axis pressure, shared.

 

Thad teh doesn't plunge mill

[Metalmuncher]

plunge is the most effeicent way to remove material if you have the horsepower and the least wear on the machine if you have the horse power.

[Lumpnut]

Don't do alot of plunge milling , but I to am under the impression that is actually less wear on the spindle than side milling in most cases.

[tsewyek]

Plung milling is definitely easier on the spindle than side milling, axial load vs. radial load is much better and plays to the machine's strength. We used to plunge mill using a 2" Iscar cutter with about nine inserts and there was no comparison to side milling's stresses on the machine.

[Teh Bear without Brains kinda idiot]

~~~~~~~~~~~~~~

I've often wondered about this. Isn't there still a lot of pressure on the spindle?

~~~~~~~~~~~~~~~~~

wHEN PLUNGING THE MAIN load is axial load ,that bearings stand much better then axial + radial .

So even if siometimes you got the spindel load higher ,still it is better for a machine

 

Just my dumb thought

 

Winnie teh why not plunge milling (sometimes I do it ,especially for deep milling )

[rsbeadle]

Thanks for the input guys.

Code-Breaker, I am using Carboly feed mills and super turbo mills .75 to 1.5 tool diameter. We ran some tests taking cuts at .250 step over feeding about 25 inches/min. The tool did well with very little spindle or z load.

Every one else: The supervisor in our sister company swears that the offset load caused by only plunging with one side of the tool causes excessive wear on the spindle bearings. If anyone is plunging on a machine EVERY DAY and not trashing spindles please let me know as I can save loads of machine time by plunging out rough stock. Thanks

[Thad]

quote:

---

The supervisor in our sister company swears that the offset load caused by only plunging with one side of the tool causes excessive wear on the spindle bearings.

---

That was my concern. Anyway, people are doing it with apparent success. I can't argue with that.

 

Thad

[Scot]

Hello Everyone,

 

Interesting topic. We plung milled using the 2"Iscar also with no problems other than moving parts on occasion. We strayed away from it after moving too many parts. Now we have new magnets and I would like to go back to plunge milling. I will have to keep this in mind. Any more detail on this topic would be appreciated.

 

Scot

[robk]

Tried plunge milling in the past. Wasn't that impressed at all. It did not reduce cycle times all that much. Insert life was unpredictable. When the inserts let go you better be by the machine. Vibration was a minor problem at the top of the tombstone. Even getting the chips out was not working so great on very deep pockets on a horizontal.

Tried the new feed mills from a few different companies (Iscar, Mitsubishi, Carboloy, Ingersoll). Ended up using Mitsubishi AJX type. Very predictable cutter with an unbelievable insert life (inserts are pretty cheap too). For the 1.5" & 2.5" dia. cutters FPT is @ .060 with the SFM of 560 in 420ss deep pocketing. We trust the cutters so much that we run them in our "lights out" programs. Also you can't touch the warranty that Mits. offers. If you wreck the tool and they give you a new one for free. Get a rep in your door and give it a try.

[cncchuck]

just did a job with a kennametal "z" mill and it worked great. we had a pocket in a part and were having trouble getting the material out.kennametal brought in a 2 inch z mill and it worked great. we ran it dry in 321 st.st. and set up an air line blowing into the pocket to get chips out.how are you guys programing for plunge milling? i used drilling which worked but there must be a different way. i plan on using this more in future programs

[Guest CNC Apps Guy 1]

There's a "Surface Rough Plunge" Toolpath which is not supposed to violate surfaces. It works well. I've been a big fan of Plunge Milling for about 6 years now. Used to do it with V7 but had to use drilling cycles and had to figure things out myself as not many people were doing it at that time.

[Hardmill]

The plunge milling toolpath that James speaks of

has worked great for me on several occasions.

Speeds and feeds naturally are critical, as well

as rigid set-up.

 

PEACE

[cncchuck]

i tried messing with "surface rough plunge" but couldnt get it to do what i wanted. if i remember right it was plunging at the ends of my lines or something like that.i didnt have much time to play with it because the machine was waiting on me.

[rsbeadle]

Thanks for the info guys. I may do a few more tests in the near future and get back to let everyone know how it turns out.

[jeff]

is Plunge milling FASTER than say a pocket milling cycle?

If so,how much faster?

[Hardmill]

With all the proper variables in place, YES.

Not to mention it putting a lot less stress on

your machine tool.

Your utilizing the strongest part of your machine.

Again rigidity and speeds & feeds are critical.

 

 

PEACE

[chip]

http://www.emastercam.com/cgi-bin/ultimate...t=012926#000000

 

[thoskins]

{how are you guys programing for plunge milling? i used drilling which worked but there must be a different way. i plan on using this more in future programs}

 

I use flowline or parallel for plunge milling.

It will only work if you have a drafted wall or a radius at the bottom of the wall.

Set the cut direction to one way and the feed plane to the top of your stock and it works great. I prefer using flowline because you can set a scallop height and the software figures your step over. It also seems to be a little faster than parallel. The only problem I have is the surfaces selection has to be fairly simple for flowline.

[chopsley]

I've got a 3" dia. Kennametal Z axis cutter to try out on a part I've got coming up. The surfaces are simple and not in a cavity so chip

evac should not be a problem. The material is hard. About 48 Rc steel. Also we only have V9.1

Mill II. So I might have to get a little creative with this part. Cat 50 taper tool with

enough ponys to make this thing work but these are uncharted waters for me. Keep the info flowing in. I'll post what kind of results I get.

[Hardmill]

quote:

---

I use flowline or parallel for plunge milling.

---

Would it be possible to see one of your files.

:eyebrow raised:

I'm always in for something new.

 

 

PEACE

[thoskins]

Hardmill

 

as requested file is on ftp in MC9_files folder. Its named HARDMILL.mc9

 

[chopsley]

The Kennametal Z axis cutter worked better than I had hoped. The 3" dia. tool (6 inserts) plowed through the Rc40 steel at 400 sfm with a .006 per tooth chip load. 15 IPM. I was amazed how quiet it cut. Tightly curled blue chips raining off the part. The tool sounded like it was begging for more feed. I'm now a believer. After four of these parts the inserts looked just fine. I had to look close to tell that they had been used. Oh, used air only for coolant. I'll be busy implementing this tool into all similar parts or any part that it make sense to use.

Happy New Year to all!!

[cncchuck]

chopsley,

i have recently been using a 2 inch kennametal Z mill and have had good results. we had a deep pocket job recently and getting the mat. out was timely until kennametal brought one in. i will be using more often also .