[Eddieweeks]

A month a go I received a remanufacturing VMC 3016L and everything is fine
untill I got a job to cut 1018 steel. No problem right..

I wrote the program for a .319 depth of cut with a 3/4" 4 flt carbide endmill
and it chatter bad. Changed to .150 DOC.. Chattered... Moved all
the way to 0.043" DOC before it quit chattering... I am running 350 SFM
and 0.0015" per tooth.. Even at 0.043 DOC if I changed the RPMs it will
start chattering.

Put a brand new Kenametal 1" end mill with 2 flt inserts and ran 1000 SFM 0.006 per tooth, no problem but only could cut 0.050 DOC..

The tool saleman cam buy yesterday and put in a 1/2 4 flt super end mill
700 SFM.. 0.319 DOC and it cut, but chatterd at a very high frequency..
I changed it to 0.160 DOC (or 2 passes)... It cut ok.. still chattering..

Am I expecting to much from this machine.. ?..

I am cutting 1018 steel, 2.5 sqare bar sitting in the bottom a 6" kurt vise

Thanks for you help...

[carbidecraters]

Sounds like the spindle bore may need to be ground. It could be also your tool is sticking out of the holder too far. Generally though you should be able to take 3/4 of the diameter of the tool without any chatter. Was it sqeaking as well? Is it in format 2? I could write a small program that would test the chatter

[Ken_Shea]

Ther are many variables but here are a few things to consider from Niagra tool Cutter. They have extensive technical information.
http://www.niagaracutter.com/

Feed and speed too fast
Lack of rigidity (machine & holder)
Poor set up
Cut is too heavy
Overhang of tool is too much
Lack of relief
Decrease relief angle, make margin: (touch primary with oil stone)


Here is another very useful link for software that offers speeds and feeds and bunches of other useful machining, drilling, tapping information.
http://www.mrainey.freeservers.com/


Ken

[carbidecraters]

Reman'ed from Fadal means very little these days. Insiders say that they dont check all the things they say and they just once over and ship the machine.....its a sham!!

[carbidecraters]

Ther are many variables but here are a few things to consider from Niagra tool Cutter. They have extensive technical information.
http://www.niagaracutter.com/

Feed and speed too fast
Lack of rigidity (machine & holder)
Poor set up
Cut is too heavy
Overhang of tool is too much
Lack of relief
Decrease relief angle, make margin: (touch primary with oil stone)


Here is another very useful link for software that offers speeds and feeds and bunches of other useful machining, drilling, tapping information.
http://www.mrainey.freeservers.com/


Ken

Ken it seems like even the tool salesman couldnt get it right...hmmmm

[Eddieweeks]

It is difficult to describe the sound... you know when it drills, it makes
no sound.. When its cutting well. All I hear is a nice humm.. I am not sure
I heard sqeaking, each tool chattered / squalled differently. The 1" made
the most racket.. The 1/2 at 700 SFM was very high pitch and left a chattering finish.. We ran the 1/2" at 10 to 70 ipm and only the inensity
changed.

i am going to test the spindle bore with a blue marker..

Thanks

Sounds like the spindle bore may need to be ground. It could be also your tool is sticking out of the holder too far. Generally though you should be able to take 3/4 of the diameter of the tool without any chatter. Was it sqeaking as well? Is it in format 2? I could write a small program that would test the chatter

[HuFlungDung]

If the toolholder is good, and the spindle taper is good, you might have broken springs in the tool retension rod. When the tool gets enough bite on the work, the helix of the flute is able to pull the toolholder out of the spindle a wee bit. This would be visible after some extended period of time as a brown rust stain on the tool holder shank, called fretting corrosion.

[carbidecraters]

If the toolholder is good, and the spindle taper is good, you might have broken springs in the tool retension rod. When the tool gets enough bite on the work, the helix of the flute is able to pull the toolholder out of the spindle a wee bit. This would be visible after some extended period of time as a brown rust stain on the tool holder shank, called fretting corrosion.

yup yup yup

[Eddieweeks]

Does everyone agree, that this machine should be able to cut more than
0.050" with a 3/4 endmill.. I would be happy with 0.200" but 0.050" is unacceptable.

I will check on the spring. Thanks

Eddie

[HuFlungDung]

I vote, yes it should be able to cut .2" deep with a 3/4" endmill. I will qualify that statement by saying that a solid carbide endmill may want to scream a bit when its brand new, if the edges are really keen. A tad too much clearance is responsible, but usually after a break in period this noise will diminish.

An inserted tooth endmill, with typical honed inserts should behave itself right from the beginning.

[Geof]

I am not familiar with this machine but I have had chatter problems on big manual machines because the spindle bearing preload was not high enough. If the machine has been remanufactured this may be something to check.

[carbidecraters]

We run .75 endmills .310 deep at 200sfm in lasered edge 1018 all day with a little 3016 but the linear ways are something we dont have.

[Scott_bob]

eddiweeks,

Is the milling operation slotting? If you are slotting, and I assume you are, yes you are expecting way too much from your linear way CNC. Now if you are profiling and your engagement is less than 1/2 of the tool, then both speeds and feeds can be as fast as you're running in steel. No way, if you are slotting on this linear way machine.

High performance machining (Not HSM) would not cut as deep as you started with...
HSM would use even shallower depth of cut...

Slotting is always problematic, at least knock off 25% of your feeds for profiling, and depth of cut like you have discovered (1/4 of your depth of cut for profiling).

Linear way machines just don't have the vibration dampening qualities of a good box way machine, but they can be faster, and are definetly easier to build.

Good luck, and keep us informed, good discussion everyone...
BTW, Ken Shea, I like what I see on your link to the ME Consultant Professional software, I am trying it out right after I finish here.

[psychomill]

If you are slotting, and I assume you are, yes you are expecting way too much from your linear way CNC.

Linear way machines just don't have the vibration dampening qualities of a good box way machine, but they can be faster, and are definetly easier to build.

I wouln't attribute this problem to the fact that a machine has linear guides. This sounds like you're saying that all linear guide machines have this problem when taking the cut he's taking. His initial cut is not that tough. Something else is going on. It could just be the Fadal.

90% of the machines I have are linear. I for one can tell you that I can take way more cut than he is without chatter or extreme vibrations causing problems.

I'm more curious to your actual set up Eddie. What tool are you using? Brand? Tool holder? part set up? How much reach? etc etc. Your machine should be able to take the cut you were initially programming for.

[Eddieweeks]

Here are some of the tools I have tried... 3/4" carbide (no name) 4 flt...

1" Kennametal brand new with inserts that my friend is using to cut 316 SS
on a 4020 Fadal 0.012 at per tooth... When I saw that. I got the holder and
inserts... Didn't do me any good...

the results are

3/4 end mill.... 0.040 DOC.. anymore it chatters.. tried many speeds and feeds

1" end mill... Cound do 0.050 DOC at 0.006 per tooth no problem.. anymore chatter.

the tool man put in a crazy looking 1/2 inch 4 flute. 5380 RPM.. 700 SFM... 0.319 DOC.... Cut like butter.. at ~50 in/min ... He said it was chattering and when you
look at the part you can see it in the finish...

I changed it to 0.160 DOC... Took twice as long witch was still 10x faster than 0.040
but still chattered but still at a very high frequency..

I want to thank you guys for your help. I am just starting out and my ears are open..

Eddie Weeks
http://www.corpcomp.com/weeks1/

[Neal]

Just to show what can be done on this machine when everything is correct, I frequently make a cut of .750" deep, full 1" diameter, 5 flute corn cob M42 cobalt EM at 380 RPM at 5.0 IPM in 17-4ph stainless.
I would suggest that you verify the bellville washer stack. If that checks out ok (1650 to 2100 psi for a locking drawbar) then I would consider load the tool harder.

Neal

[Eddieweeks]

Yeah... See... I am not asking too much... Getting Irritated...

[Scott_bob]

Eddie,

Thanks for the photos, those pics are worth a couple thousand words...
Yeh, the 1st thing your want to change is that 2 set screw solid end mill holder.
I only use these for drilling, for the same reason you have shown. Chatter...

You need a good stub (single set screw) holder. These get the end mill shank up inside your taper, much better. This alone may solve your probs.
Ideal holder would be a shrink fit holder, but that's another story...

[alloyspec]

I run Fadal 4020s and a 6030 and I would say there is no way I would get tool life from 700 sfm with carbide in these machines and they have box ways. We find the published claims of the tool companies to be way off the charts. But sometimes they are off the other way too. In aluminum, yes by all means run 1200 or 1250 sfm, but have a lot of coolant. The supersonic high-speed machining only seams to works in the aircraft and the tool-and-die industry. You need a good toolholder to get a good finish. Use as short an endmill as possible and choke up on it in the holder. We find these machines work best with a ½ inch end mill, even 2” flute length. But you cannot run them at that kind of RPM. Slow the rpm and increase the chip per tooth to get your time down. Try a roughing mill first as you can really up the chip per tooth, but you have to slow the RPM even more with that. Or try an inserted mill as a rougher as you can crank up the RPM a lot more than a 4 flute. You have to find what works the best for your machine. I do not get near the tool life as the guy on the old Hitachi-Seiki next to me, as it is a much heavier built machine, but I find ways to work around it.

Alloyspec

[carbidecraters]

**** no you should be able to bury that end mill...get that guy who sold it to you and pull on his ear untill he fixes it