Need some 6" face mill recommendations

dodgin · May 25, 2017

Hey guys - looking for a new 6" face mill and some tough inserts for a certain application. Job is milling some cast steel - coming in about 300 BHN, believe it's also annealed. Between two operations we're milling off about 20 cubic inches of material total, and with the inserts we're running we're getting about 4 or 5 completed pieces before indexing. Hard to explain but there's a tricky part about the way the work sits on the fixture, there's two pads on either side getting milled down that are just kind of hanging out in space, and we're playing with the idea of some kind of jackscrew to put in there for some support. Anyways, for the time being we're fighting a bit of chatter on those surfaces.

Machinist hates indexing inserts and wants to know what else is out there for us to further limit the dead spindle time he's getting, and maybe run a bit faster while we're at it - currently running these (THLS130608R IN2530) about 350 RPM, 17 IPM. Tried out an OSG Phoenix already and it didn't go over particularly well.

Anyone have any good input for what to use in that kind of material (cough, Jashley, cough)?

Hazzert · May 25, 2017

How about a feedmill? Assuming the part is supported right below these pads you might be surprised at what you could do with a Ø2-3" feedmill, we use iscar but there might be better nowadays.

Edit you say they're hanging in space but you're considering a jackscrew, definitely a must if you try a feedmill.

dodgin · May 25, 2017

Hazzert said:
How about a feedmill? Assuming the part is supported right below these pads you might be surprised at what you could do with a Ø2-3" feedmill, we use iscar but there might be better nowadays.

Edit you say they're hanging in space but you're considering a jackscrew, definitely a must if you try a feedmill.

Yep, yep...we had visited that idea a bit back and if I'm not mistaken for the couple of feed mills we had looked into there were some clearance issues. The areas being milled sit just above the table (HBM) and to use a smaller mill and not run the spindle into the table we were going to need a pretty considerable extension for that clearance. Might not be bad to revisit if we can maintain our rigidity - each surface only has about .125" coming off of it so a feed mill could make quick work.

Mtndew · May 25, 2017

Sandvik R245

"Machinist hates indexing inserts"-- tell him it's his job,

Jashley73 · May 25, 2017

dodgin said:
Anyone have any good input for what to use in that kind of material (cough, Jashley, cough)?

If you're asking me specifically, I'd point you to our Double-Octomills. The small version gets you 3mm cutting depth. The big version gets you to 6mm cutting depth. Lots of grade & edge-prep options, especially in the large version. Our MP2500 grade would probably be a great place to start, and best of all - you could run dry! (I hate coolant with a passion...)

https://www.secotools.com/#article/m_6898
(And as of Monday, our website no longer sucks. )

I would definitely recommend the jack-screw, regardless of who's cutter it is. It doesn't take much pressure to provide support. Like finger pressure on the jack-screw.

It also doesn't take much more than finger pressure to move the part - that is, to bend/distort the part - with jack screws either. If you really need to crank down on the jacks to secure the part, then you'll have to toe-clamp over the jacks, and use an indicator on the part. Zero the indicator with the part sitting free, and then tighten the jacks/clamps to keep the indicator on "Zero." (It takes about 3x more pressure on the clamps to move the part the same distance, as it does the jack screws - go figure...)

dodgin · May 26, 2017

Jashley73 said:
If you're asking me specifically, I'd point you to our Double-Octomills. The small version gets you 3mm cutting depth. The big version gets you to 6mm cutting depth. Lots of grade & edge-prep options, especially in the large version. Our MP2500 grade would probably be a great place to start, and best of all - you could run dry! (I hate coolant with a passion...)

View attachment 199608 View attachment 199609

https://www.secotools.com/#article/m_6898
(And as of Monday, our website no longer sucks. )

I would definitely recommend the jack-screw, regardless of who's cutter it is. It doesn't take much pressure to provide support. Like finger pressure on the jack-screw.

It also doesn't take much more than finger pressure to move the part - that is, to bend/distort the part - with jack screws either. If you really need to crank down on the jacks to secure the part, then you'll have to toe-clamp over the jacks, and use an indicator on the part. Zero the indicator with the part sitting free, and then tighten the jacks/clamps to keep the indicator on "Zero." (It takes about 3x more pressure on the clamps to move the part the same distance, as it does the jack screws - go figure...)

16 cutting edges...that's certifiably badass. Thanks for the recommendation, I'm going to give our Seco rep a call today and see if we can't test one of these guys.

Mtndew · May 26, 2017

Jashley73 said:
https://www.secotools.com/#article/m_6898
(And as of Monday, our website no longer sucks. )

THANK YOU for pointing that out.
It was terrible before and so hard to navigate!

DMF_TomB · May 26, 2017

dodgin said:
Hey guys - looking for a new 6" face mill and some tough inserts for a certain application. Job is milling some cast steel - coming in about 300 BHN, believe it's also annealed. Between two operations we're milling off about 20 cubic inches of material total, and with the inserts we're running we're getting about 4 or 5 completed pieces before indexing. Hard to explain but there's a tricky part about the way the work sits on the fixture, there's two pads on either side getting milled down that are just kind of hanging out in space, and we're playing with the idea of some kind of jackscrew to put in there for some support. Anyways, for the time being we're fighting a bit of chatter on those surfaces.

Machinist hates indexing inserts and wants to know what else is out there for us to further limit the dead spindle time he's getting, and maybe run a bit faster while we're at it - currently running these (THLS130608R IN2530) about 350 RPM, 17 IPM. Tried out an OSG Phoenix already and it didn't go over particularly well.

Anyone have any good input for what to use in that kind of material (cough, Jashley, cough)?

.
i use 6" facemill often and it has big Widia inserts on it. Feed 20 to 60 ipm feed usually. if part vibrating real bad often better to add more passes. when down to 20 ipm with slower rpm of course. usually not better to go any slower but to add more passes so feed is back closer to recommended rate.
.
some part shapes are just not rigid enough for 6" facemill and you are better off going to 4" facemill. math often says its slower using too big a facemill and slowing way down cause of vibration. often feeds and speeds got nothing to do with what cutter can take but what the part can take. 0.2 depth full 6" width at over 50 ipm feed can literally shake a part loose in a fixture and all the hold down bolts and pushers just loosen up from vibration heard 200 feet away
.
tool life should be 45 to 120 minutes. usually if not lasting 45 minutes the feeds and speeds and depth and width of cut needs adjustment. if inserts last over 120 minutes its cause they are not being pushed hard enough
.
watch the load meter. you can easily need 40 hp if pushing to the max

huskermcdoogle · May 26, 2017

Kennametal Dodeka or Sandvik 745. Both are very capable. 745 is very quiet. Dodeka is louder, but gets better tool life. Used to run in structural steel, had about a 200 minute edge life. Ran them in 4", 6", and 8" diameters. Play with doc to find the machines sweet spot. You can push the feeds and speeds safely. 1500SFM and .020" per tooth is not unheard of in steel with the dodeka platform, done it many times in production at about .05" doc. (part rigidity, and spindle power problems keeping doc low)

michiganbuck · May 26, 2017

Good to run an indicator to insert tops and see most are in the cut +- .002 or so.. If not you can often shim under to make good..

Just running one part and looking at wear land can tell if most inserts are in the cut.

Smooth wear can tell you might go harder grade carbide..chipping can meal grade is too hard.

ridged set-up can help for longer life. Some times one can bump the part with a heavy solid block-in in an area to make the set-up more solid.

For early chipping some time a diamond honed small land can help..sometimes for chipping a rub on a steel with brush can help..For normal wear going to harder carbide is good.. and coating is good also.

Any thin area of the part should be braced.

adama · May 26, 2017

IMHO you don't want a new face mill, you want 2 with arbours so you can have one in the machine and one being indexed. No dead time like this.

DMF_TomB · May 26, 2017

salesman rarely mention with steel if you want to remove
.
10 cubic inch per minute you need 10 hp
20 cubic inch per minute 20 hp
50 cubic inch per minute 50 hp
.
just saying the obvious
.
depth, width of cut, feeds and speeds add up the cubic inches per minute.
.
be aware cutting forces can be over 2000 lbs. if part held with little bolts they often cannot hold the load. also lock nuts often needed cause of vibration

michiganbuck · May 26, 2017

QT:[Machinist hates indexing inserts and wants to know what else is out there.. grind cutters .. then you need a TC grinder.]

Yes you can grind indexable cutters.. you just make a bevel to the curtting corner that does not harm the set-to-pocket sides.

Likely you can double the life of inserts that way.. yes with a simple TC grinder and simple set-up perhaps 5 minuets to go around a 6 to 10" cutter.

Casting sand can be a bugger on such work..

DMF_TomB · May 26, 2017

tool life if over 120 minutes you aint pushing hard enough.
.
it is what it is. 60 to 120 minutes of heavy cutting you need to change inserts. as old timers use to say if throwing sparks inserts are going dull. sparks often seen even using coolant. some inserts always throw sparks cutting dry especially if on the high end of max recommendations
.
not many machines got the hp to push a 6" facemill that hard.might want to check whether your machine can even handle it

Mtndew · May 26, 2017

DMF_TomB said:
salesman rarely mention with steel if you want to remove
.
10 cubic inch per minute you need 10 hp
20 cubic inch per minute 20 hp
50 cubic inch per minute 50 hp
.
just saying the obvious
.
depth, width of cut, feeds and speeds add up the cubic inches per minute.
.
be aware cutting forces can be over 2000 lbs. if part held with little bolts they often cannot hold the load. also lock nuts often needed cause of vibration

He is removing 20 Cubic inches of material total. Not per minute. :rolleyes5:

DMF_TomB · May 26, 2017

Mtndew said:
He is removing 20 Cubic inches of material total. Not per minute.

20 cubic inches total then he should be done in less than 1 minute. machine wont even have time to get warmed up
.
in machinist apprenticeship they teach
.
1) how long should it take to machine if using a different cutter
2) does machine have the hp to run cutter
3) can i hold the part to take cutting forces
4) how much does new tooling or facemill cost and what is my expected return on investment time.
.
like boss aint going to be happy buying $1000. facemill and machine dont have hp to run, part cant take cutting forces. job be done in a minute so if i save $1 or $2 labor cost but new facemill cost $1000 that dont seem worth it
.
just saying salesman aint going to mention it but will gladly take your money selling a tool to you. standard salesman tactic say you need the tool to keep up with the competition. or make you feel superior in deciding to buy the super duper tool.
.
do the math first and maybe you make some money on the job

dodgin · May 26, 2017

Just so you guys can see what we're working with. The pads on each end are what get milled down on the first op, then on the second it's the surface with numerous bolt holes that's visible at the bottom of the piece. Obviously you guys can tell where we're getting the chatter. The Ingersoll runs decent and leaves a good finish at 350 and 17 IPM, .06 DOC, but we imagine there's something out there that can do more than 4 or 5 pieces before an index.

The OSG Phoenix we had running about 300 RPM, 30 IPM to get the chatter out, anything lower than that feed wise and those pads were rattling a bit. At 30 IPM the inserts lasted only 1 piece.

Got a hold of Seco...gonna test drive the Double Octo in a couple weeks and see what we get.

DMF_TomB · May 26, 2017

dodgin said:
View attachment 199752

Just so you guys can see what we're working with. The pads on each end are what get milled down on the first op, then on the second it's the surface with numerous bolt holes that's visible at the bottom of the piece. Obviously you guys can tell where we're getting the chatter. The Ingersoll runs decent and leaves a good finish at 350 and 17 IPM, .06 DOC, but we imagine there's something out there that can do more than 4 or 5 pieces before an index.

The OSG Phoenix we had running about 300 RPM, 30 IPM to get the chatter out, anything lower than that feed wise and those pads were rattling a bit. At 30 IPM the inserts lasted only 1 piece.

Got a hold of Seco...gonna test drive the Double Octo in a couple weeks and see what we get.

.
my experience at only .06 depth of cut i would use smaller dia facemill at much higher depth of cut cause of part chatter vibration
.
most facemills designed for .150 to .200 depth of cut. sure some high feed ones run less depth of cut at higher feed but regular facemill i always take at least .125 DOC
.
if part vibrating often have to slow rpm. got nothing to do with tool its got to do with part only taking some much hp cutting forces with vibration. quite normal not using the biggest tool as the part cant take the cutting forces and end up finding a smaller tool is faster
.
i dont measure tool life per piece but how many minutes. 60 minutes is normal tool life
.
60 minutes at 20 cubic inches per minute is 1200 cubic inches tool life and 339 lbs of chips

dodgin · May 26, 2017

DMF_TomB said:
.
my experience at only .06 depth of cut i would use smaller dia facemill at much higher depth of cut cause of part chatter vibration
.
most facemills designed for .150 to .200 depth of cut. sure some high feed ones run less depth of cut at higher feed but regular facemill i always take at least .125 DOC
.
if part vibrating often have to slow rpm. got nothing to do with tool its got to do with part only taking some much hp cutting forces with vibration. quite normal not using the biggest tool as the part cant take the cutting forces and end up finding a smaller tool is faster
.
i dont measure tool life per piece but how many minutes. 60 minutes is normal tool life

Yeah, .06 depth isn't any good. I'm hoping to change that when we get a new set up. The program was definitely drawn up with inconsistent castings in mind though.

DMF_TomB · May 26, 2017

dodgin said:
Yeah, .06 depth isn't any good. I'm hoping to change that when we get a new set up. The program was definitely drawn up with inconsistent castings in mind though.

.
normal to have extra what if big passes in case casting is big. so what if 1st pass cutting air at 30 ipm it be done with soon.
.
picture shows facemill tool comp adjusted it should have been 1/2" away. facemill choked trying to take 1/2 depth. foundry apologized the casting being 1/2" big. machine was down for repairs took 6 weeks
.
tool came out of spindle drive keys disengaged and spun on spindle taper. machine pushed a 11 ton casting that was bolted in a fixture so guessing over 11 tons of push. it tripped the overloads and it takes a lot to do that

Need some 6" face mill recommendations

Hot Rolled

Stainless

Hot Rolled

Diamond

Titanium

Hot Rolled

Diamond

Diamond

Attachments

Stainless

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Hot Rolled

Diamond

Hot Rolled

Diamond

Attachments

Similar threads