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...

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

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

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!!

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

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

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.

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

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

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.

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.

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.

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.

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.

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/

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

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

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...

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

**** 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

oops after seeing that holder its no wonder...when you take for instance a 5 inch long endmill and cut 2 inches of the end off you drmatically and expidentially decreased the chatter and harmonics by greater than 4 times

this is starting to come together now... The tool guy installed a 1/2 endmill
in a fairly short holder.. Its still chattered but not near as bad as anything else...
I have run about 14 parts with this and now it hardly chatters at all any more..

The one inch cutter is a little shorter and it does ok.. The 3/4 is the longest
and it is the worst...

BTW.. that 1/2 inch cutter is doing all my steel work now.... 700 SFM.. 50 IPM
it cuts both Jaws in 1.5 min... 0.160 DOC... the tool guy told me to run 0.319
and I did and it worked... but I put it at 0.160 after he left.. hahah... I asked him
at 700 SFM how long will it last... He looked around and said there is not enough steel
in here to wear it out, and if you do you get a new one free.. I purched a bunch on the spot... hahah..

I want to thank you guys for your help.. I was pulling my hair out...
Can someone point me in the direction for CAT 40 holders.. SHORT.. hahah

Thanks again..

I will make a video of the 1/2 endmill... I want to know if this is the kind of
cutting you all do....

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

Eddie you may want to take a look at your machining ...reason I say this is because alot of salesmen are told and will tell that small cuts and rapid feed rates are the way of the future....this isnt true as they have always been around and it is just in the last ten years it has become more affordable. In alot of cases these small cuts will eat the inserts or tooling you are using faster...and in alot they wont. Watch those guys carefully.....this is coming from a shop owner who has 2 good friends in rapid machining tool sales

I think this supplier is a great value, is American made, and they have all the good stuff...

http://www.parlec.com/images/pdf/tol__60_83.pdf

Check out the really stub length solid end mill holders, they are inexpensive, and perform way, way better than a regular holder. The shank of your end mill will be up inside the spindle taper...

Just an update.... .. All chattering quit after 4-6 parts.. Just finished all parts.
Now its just a nice hummmm... Still running 1/2" end mill 700 SFM 0.160 DOC..
Doing sloting and 0.65 x D cutting. I just order 3 brand new stuby tool holders 1",3/4",1/2".. I want to thank every one for there help... Save me a lot of
time..

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

350 SFM for standard carbide emill in 1018 is too fast. Four flute in slot is wrong tool. The chatter may be from combination. Try 150sfm and no more than 3 flutes for full engagement.

The fact that you can run indexable and get good results tells me the machine is probably ok. The forces exerted by indexables are greater than from standard emills.

After talking to my good friend (machine shop owner), He said that 700 SFM was
really fast. I reminded him that Justin (Tool salesman) said if you wear or damage
this tool do this job, I will give you another one free. He was right. I finished the
job and it was fine. Tool guy it has some supercoating and the 4 flutes were
at odd angles not 90,180 ect... Also he said turn off the coolent, and I did.. ???
The part was large and the cuts were small so the part never got hot.

ctate2000... can you explain "that you can run indexable"

Thanks
Eddie Weeks

Do you have a locking drawbar or non-locking drawbar? The difference is 1650 to 2011 psi fopr the locking and 800 to 1000 psi for the non-locking in retention force. Also the bellville stack should be checked to insure that the correct retention pressure is there.
Next would be to look at the tool diameter vs tool length to get the best stability available.
Just food for thought.

Neal

Indexable tools are also known as "inserted". I suppose either term is correct. I used to run the family shop and recently left to take position as Mfg Eng. We had three Fadals two 15xt (now 3016L) and one 4020A. I could take heavier cuts on the small machines than on the larger one. Never figured out why. Probably the compactness of the 15xt. They are good machines and I never once had any complaints about them. We used to mill some 303 SS impellars from solid bar. They were 3.5 to 4.0 in dia 1.25 long and had 5 veins. The tool was a carboloy micro turbo mill single flute indexable with .125 R on the corner. Cutting speed was 6500 rpm and feed rate was 35 ipm. Radial depth of cut was full engagement and axial depth of cut was .0625. Took 15 mins to mill one complete and I got three parts per cutting edge. The reason it works is because the radius on the corner was half the axial DOC and it was like using a full round tool.Chip thinning due to radius allows you up the feed rate to maintain proper chip thickness. I would highly recommend the micro turbo mill for your machine. They are very free cutting and perform well in all materials.

Your chatter may be a result of the spindle bearings not having sufficient preload.
If the cutter chatters more in the morning (when the spindle is cold) than at the end of the day (when the spindle is warm) that is an indication of a bearing preload problem. If it chatters LESS with the spindle chiller OFF then it is a preload problem as the spindle will be warmer than spindle housing and the spindle will expand and increase preload on the bearings.

You can check the spindle for axial freeplay (in the Z direction) to determine if the spindle bearings have lost their preload. Place a dial indicator base on the spindle housing (not on the table) with the indicator on the spindle nose. Use a bar pivoting on a block to provide an upward force to load the spindle bearings. Use a block of wood on the spindle nose. Don't overdo it with force on the bar, as you should see a deflection with a couple hundred pounds of force on the spindle. You should not see even a .0001 of axial movement in the spindle.

. You should not see even a .0001 of axial movement in the spindle.
I have to clear somthing
in about 1000 PSI you should read 0.02mm to 0.04 mm this for 10K spindle
for 15K spindle it 0.05 mm
to calculate 0.02mm it about 0.0008

Do you mean 1000 pounds of force? That is a lot of force for a shop guy to exert on the nose of a spindle without force measurment and a means of insuring that the Z axis ball screw brake is not damaged.

If you are using a force/deflection method of setting spindle bearing preload, the total tolerance on bearing deflection (at about 1000 lbf.) should be around .00005 inch or 1.5 micron. The range of deflection values between .02mm and .04mm (.0008 inch) is an ENORMOUS variation in preload.

Sorry I mean 1000 lbf but if you will have spindle that the preload is 1.5 micron
It will not turn by the hand and not sure that it can turn by the motor I will try to post here Fadal paper that talk about it

Eddie,

does it chatter in bouth the X and Y direction.If not then try a convenional cut vrs. climb on the axis that chatters see if that changes much.

Have you check the lash in the ball srcews and or the thrust bearings?

what size it the spindle tapper? From here it looks to be a 30.


Just thought I would ask
John

Try using a shorter style hard body tool holder. Also try using a rougher endmill and then come back though with a three flute finishing mill.

Try using a shorter style hard body tool holder. Also try using a rougher endmill and then come back though with a three flute finishing mill.

That is what I did.. And I have not had any chatter. It seems the problem
was in the tool holder the whole time. I have also changed to stubby endmills
when I can (Hanita) and have been cutting alot of material.

Eddie Weeks