Yellow Bullet Forums banner

1 - 20 of 25 Posts

·
Registered
Joined
·
1,574 Posts
Discussion Starter #1
At the Mastercam X5 launch party yesterday they highlighted a bunch of high speed machining techniques, it appears my methods are so yesterday but I still dont understand the concept.

Im side cutting hard Nickel Heat Resistant alloys, removing 150 mils from the side of a 5" tall block taking 30 mils off at a time, each cut is full depth.

My current specs are

1" Dia End Mil TiAlN coated (recommended SFM is ~100 @ .002 feed per tooth)
Speed 330 RPM
Feed 3 IPM

I have a 10K RPM spindle but keeping with the tools SFM recommendation limits me to around 330 so I guess I dont understand how to obtain the blistering fast RPMs and feeds without wearing out my tool.

Please give any thoughts.
 

·
Moderater
Joined
·
13,633 Posts
Funny you posted this. It's a great catch phrase in the industry right now. I have a lot of machine operators bitching right now because these sales men making all the bogus claims and the shop supervision expecting there machine time to be cut in half. I just had a customer call because of rough finish on there job. Every plunge cut they made left a huge surface violation. After checking the machine for geometery, ware, redoing the pitch compensation and backlash I had them do a test cut. Same thing. After going over the last couple files I found out they were cutting all surface in extreme mode which eliminates all acceleration and deceleration from the control so the machine is slamming around. Come to find out the programmer was told to use this mode by the software engineer. Not only dose this shorten the life of the tool but the machine gets beat up quick and the time saved is negligible.
 

·
Registered
Joined
·
1,574 Posts
Discussion Starter #4
They did say you must use gentle arcs when high speed maching so the motions are smooth. Basically the tool just glances the work piece using only circular motions.
 

·
Moderater
Joined
·
13,633 Posts
What if your machining a mold that has all tight radius's?
 

·
Registered
Joined
·
38 Posts
If you are talking about dynamic mill toolpaths they do work. The software allows for a preset chip thickness and the tool doesnt bury itself in the corners. You are using the whole flute length with small stepovers as low as 5%.
 

·
Registered
Joined
·
519 Posts
I find many people including supervisors, don't have a phuken clue what it takes or how long it takes, to machine anything. I always get a kick out of the guys that come over to the lathe/mill and go "Can you show me how to run this." Yeah sure, only takes about 5 minutes. Sorry....off topic a bit, this thread kinda hit a nerve.
 

·
Registered
Joined
·
333 Posts
HSM... Hmmm where to start. I would say any machine that can travel 250 ipm or higher.(upwards or 900 ipm) Haas on the low side up to Makino,Roder,Okuma (sp?) Its a lighter depth of cut with higher rpms creating a thinner chip alowing you to travel faster. The key is you half to have good tooling to achieve this. Something carbide and coated for what you are cutting. The harder the rockwell the better the cutter and coating. Aluminum is very forgiving but still calls for a good cutter with a good coating.
 

·
Registered
Joined
·
61 Posts
Mastercam's dynamic mill has proven itself very valuable in my shop, specifically rocker arms.
I am running a 1/2" dia solid carbide at 2800 rpm, 40. ipm with 1.00 of depth and .100 of width, on a 40 taper vertical.
The toolpath maintains a constant width of cut with a radial entry and exit, to avoid "slamming" the cutter into corners and overloading with changing width engagement.

Cutter life is exceptional and amount of material removed is excellent, a rocker starts at 12 lbs. and finishes at about 15 ounces, so I have to make a lot of chips.:)

FWIW, 1 endmill has removed about 120 lbs of material using dynamic mill. (it might have done more, but it isnt worth a scrap part to find out)

"D"
 

·
Registered
Joined
·
240 Posts
We don't use coated endmills in aluminum.....a good carbide endmill will last a LONG time...

Definitions in our shop (we are a aerospace maufacturer, cutting a lot of aluminum and titanium):

High speed - Very shallow axial, small to medium radial, go like hell
Low speed - Large axial, large radial (full slot) - slow feed

Vericut's Optipath (Which sounds like Dynamic mill), it cuts the feed rate down to maintain the chip thickness - We think that it is ass backwords - should speed up the the small cuts to match the large cuts
 

·
Registered
Joined
·
1,574 Posts
Discussion Starter #13
Do you still follow the manufactures SFM & chip load per tooth recommendations? If I do I get one speed and its not fast.
 

·
Moderater
Joined
·
13,633 Posts
Another misconception is you can add the latest control or software to your antiquated box way low helix ball screw machine and it will cut at 200 ipm. I hate seeing a shop spend 60k on a control up grade or software package and see very little return.
 

·
Registered
Joined
·
640 Posts
I program in Unigraphics NX here at work and I am amazed at how tools are created for nothing but sales.
It's all about the $$$, ALWAYS, wether UG, Pro_E, Catia...all about the money.
The catch pharse description was given earlier, yep, pretty much.
I have seen alot of new machining centers being built with higher RPM spindles to allow some of this stuff, but only certain applications will benefit.
We do all super alloy here and very little is milled or drilled due to the rotten material. I have had the most sucess with just playing around with "trochoidal" cutter paths. Much easier on the tool, fixture, part, and machine. Less tool pressure and cycle times get reduced somewhat. Not the super duper savings that get boasted and bragged about by salesmen, but improved.
BTW: We have had a few programs created accidentally shut off the accel/decell ramps and it was never pretty. Like mentioned also, poor finish and shaking floor under the poor ole' mill:(
 

·
Registered
Joined
·
334 Posts
HSM... Hmmm where to start. I would say any machine that can travel 250 ipm or higher.(upwards or 900 ipm) Haas on the low side up to Makino,Roder,Okuma (sp?) Its a lighter depth of cut with higher rpms creating a thinner chip alowing you to travel faster. The key is you half to have good tooling to achieve this. Something carbide and coated for what you are cutting. The harder the rockwell the better the cutter and coating. Aluminum is very forgiving but still calls for a good cutter with a good coating.
Now here's something right up your alley PFM......
 

·
Registered
Joined
·
1,301 Posts
I run a machine shop where we run 80% high strength Inconel and other high nickel exotics. These type of materials practically REFUSE to be cut fast. You can do SOME high speed machining with ceramics, but its hard on the part(warping) and the machine and you are limited to mainly large areas that do not have small detail.

I use to work in a shop where we built plastic injection molds. We were milling a pocket in some P20(which is similar to 4130) that was approx. 2" deep and 14" x 14" square. The plate was only 2.5" x 16" x 16", so a majority of the material was being machined away.
With the conventional method using HS cobalt roughing endmills we would get .050"-.060" warpage in the plate and would have to mill the top and bottom of it flat and re-grind the surfaces. This was also rough on the machine as it was a small 30 taper machine. It also took a long time. Its been years, so I dont remember how long it took.

I called the local Iscar pimp and told him what we were doing. The next day he shows up with a 1" diameter 4 flute Iscar HELI 2000, with I think, a 3" or 4" length to it. IC950 I believe was the grade of insert. He tells me to run it 4000rpm, 110 IPM, .030" deep at full diameter, and no coolant, just air blast. I knew the guy was crazy(known him for a long time), but I also knew he was good. I had my doubts. The length of the tool, the rpm, the feed rate, no coolant. It was all too weird, but he was paying for the tool if it fried.

This thing threw a glowing orange rooster tail of shavings and went to removing metal at a rate I had never seen before in steel. The machine was actually handling it quite well also. We would stop every 1/2" of depth and change inserts. The tool was barely warm and the part had NO heat in it. When we were done, it took about 2/3 the time and the plate was only warped .002"-.003". It was the coolest thing since I discovered my dads micrometers were precision measuring tools, not some weak-ass c-clamps. lol

Call your tool rep and see what they have for your situation. For nickel base alloys, I like a 1" 5 flute high helix carbide endmill with a .030" corner radius for removing large amounts of material where a face mill cannot be used. We will go .300" deep at full diameter with these in heat treated 718 Inconel! Your machine has to be stout though.

At times when the latest and greatest new carbide/coating grade will not do what its price tag says it should, I will buy the grade that says its for cutting cast iron. It works well on Inconel believe it or not.
 

·
Registered
Joined
·
893 Posts
X2 on Iscar, they build great tooling, we rough out our forge dies at 85 ipm with a 1" inserted cutter, 38-42 Rc in Timken Latrobe 2714 steel. This crap is nasty to machine, drill, ect.ect. Give'em a try.
 

·
Registered
Joined
·
695 Posts
We have Rambaudi's with ceramic cutters and air bearings, it cuts blocks of billit down to frames and gussets in no time, the nice thing about ceramic cutters, is if they break, it just drops, no spinning off into the shop. We also have a sewing machine that will stitch composite prepregs together: skins to I, J, and C channels to make structural items. This thing will stitch 2 pieces of 1" plywood together, it's that tuff! Uses kevlar thread.
 
1 - 20 of 25 Posts
Top