Results 1 to 20 of 56
10-28-2013, 04:55 AM #1
Mass material removal vs. Cutter dia
First off...most of the pieces I mfg dont exceed 12" in dia./length, and with that said I have grown accustom to using 3/8-1/2 dia endmills for the majority of my roughing routines.
When do you step up to 3/4 and such?
How Do you weight mrr vs corner radius vs tool cost ect?
I cant seem to get away from the 1/2" endmill and am very interested to see what some of you folks are using for tooling, as well as techniques and tool paths that work well for you.
Thank you in advance and happy Monday
This part is 6"x1" and im removing 2/3 of the stock
10-28-2013, 06:28 AM #2
we use 5" facemills at 0.150" depth of cut going 30 inches per minute to remove material fast
4" facemills at 0.150" depth of cut and 3" width of cut at 35-40 ipm
2" carbide insert end mill at 0.3" DOC and up to 1.5" WOC at 850 sfpm and about 30 ipm. a 2" diameter carbide insert end mill can often take 1" depth of cut if width of cut is 0.1" or less at 20-30 ipm at 850 sfpm for 1018 steel.
for slotting (full width cutting) i normally take less depth of cut to avoid chatter. end mills slotting if end mill if 3 or more diameters long sticking out we normally slow down to 300 sfpm. Facemilling (less than full cutter width) even with a carbide insert end mill normally we double sfpm compared to slotting with longer cutter.
the biggest advantage with 2" carbide insert end mill is length of cutter is 3 to 6" depending on tool. we use 3 different lengths of carbide insert end mills.
....... the other thing is ability to hold the part and part being thick enough or rigid enough to with stand cutting forces. trying to cut material less than 0.1" thick and part vibration can destroy a cutter. i would not use a 1/2" roughing cutter if i needed a 2" or more depth of cut or tool stick out. a end mill sticking out that much will vibrate too much.
10-28-2013, 06:35 AM #3
you may want to give some more information on your machine types that you have and types of material you cut. It will do you no good to tell you to use a 6" face mill .250 deep if you only have a R-8 spindle.
Big B liked this post
10-28-2013, 07:01 AM #4
It would sure be nice to work on itsy bitsy parts like that.
Do you do any machining with inserts now? Who's your tooling and insert supplier?
It's almost like chocolate and vanilla, everybody has a preference. We used to be a KM shop and now I don't think that they have 25%. Lots of SECO, Sandvik, ISCAR, and Mitsubishi. If we get a new product design or some exotic material, we'll have a supplier take a look and give us a recommendation. Most machines, we look at the tool change capacity and the HP available. We've got one application where we face mill a 16*36" casting face. Try that in a super duplex stainless.
A couple of the guys I know just love these: Harroun Enterprises HIBF Mold Masher 1.00 Inserts, Accessories
I've got one of these for my home BP, just awsome. Turbo 10 - Seco Tools
10-28-2013, 07:11 AM #5
10-28-2013, 07:14 AM #6
10-28-2013, 08:22 AM #7
I was at the Emuge booth at IMTS and they were running a 5 axis Hermle at 125% of spindle load with a 12mm end mill. It's unbelievable what these tools can do if you program them correctly.
I personally find that 5/8 solid to 2" indexable is a total no man's land where nothing really works very well. I skip right over it. There are exceptions, such as aluminum, where I have a 1" indexable mill that really works well. But, for steel, or general shop stuff, forget it.
10-28-2013, 09:41 AM #8
My goto tool is the 1/2".
Programmed right, it will peg your load meter, and stay there for a very long time.
Anything bigger in solids and the dollar amount goes up sharply, and for the metal removal,
generally, though not always, not worth it.
Like, Ewsley, indexables for facing and long reach stuff.
Aluminum is a bit different, its not that hard to pack up the flutes on 1/2" tool. In that case I like a 5/8 or 3/4, but they
last for fricken ever so... its worth it.
10-28-2013, 09:46 AM #9
In reference to the Load meter, Ideally what are you shooting for on it?
10-28-2013, 09:53 AM #10
10-28-2013, 10:03 AM #11
10-28-2013, 10:03 AM #12
I was talking to a Tech the other day who was repairing the ATC on our DMF 360 Linear, and he was saying that of course running the machine at 100% rapid and 100+% Spindle Load is going to take a heavy toll on the machine. So I've been trying to delve up more information on how to effectively run a machine in a way that will have it lasting for years and years ( barring crashes of course :P )
I do imagine that your end mill will probably be the weakest link in an equation, unless your parts are small. So you probably won't hit a high Spindle load with it.
I was about to say that you could use the Spindle Load to raise your DOC/Speed/Feed if you feel like it can take more. But then I realized y'all probably use that handy calculator thing that I need to buy to come up with all of that anyways.
10-28-2013, 10:19 AM #13
10-28-2013, 10:38 AM #14
I've only replaced one set of thrust bearings from wear in a little over 4 years, never a motor or servo drive (unless it was crashed!)
The damn ATCs though... Always fighting those, the pullstud fingers, belleville washers, turret fingers...
10-28-2013, 10:48 AM #15
10-28-2013, 10:49 AM #16
10-28-2013, 11:12 AM #17
We run most of the MAzak's at 25%, it's fast enough and we do very short run job stuff so it doesn't really make sense to kick it up past that. But everytime you turn the machine off and on. It defaults to 100%, and sometimes I forget so I'll load a program and it will just haul significant ass to the part. Scares the hell out of me everytime It's like it's testing how fast I can hit feed hold
10-28-2013, 11:18 AM #18
I machine a lot of 6061 Aluminum on a Daewoo DMV 3016. It only has 8000 RPM's, and 15 HP. So like you have already mentioned got the HSM calculator and dove head first into HSM. I actually took a block of 6061 that we used to face all 6 sides at about 10 min. a side, and with HSM I am running a 4in. Face mill. 175 DOC, .800 Radial or 20% at 500 IPM. As well as profiling with E.M. instead of Flipping part for next side. I use as big of an E.M. i can that's reasonable. Which is a 1.25 ALTIN coated carbide e.m. from Detroit Industrial and i take 1 in. DOC, .05 radial, and fees about 250 IPM. So i cut run time down from 10 min a side (6 sides) so 1 hour start to finish. To 12 min. Start to finish. This HSM has opened my eyes to a whole other world.
10-28-2013, 09:09 PM #19
We are machining a lot of Aluminum here.
Recently i fell in love with SGS Aluminum-Specific endmills.
Switf-Carb or something.
So i am taking a 1.5" deep cut at 0.25" radial at 7000RPM and 170 IPM and hitting a friggin strap clamp with the end of the tool.
Before i could hit a feedhold HAAS's Torque Limit kicks in at 120% and shuts it down WITHOUT breaking the endmill!
A the tool almost made it through case hardened clamp 3/4" deep at fill slot and only one flute got little chipped.
Still using the same tool. Works fine.
So for aluminum SGS SwiftCarb 3/4" Dia Can really haul more material than our puny conveyor can remove.
Still a 2" APKT16 Face Mill Easily removes 50in^3/min even when 5" long.
allloutmx liked this post
10-29-2013, 04:21 AM #20