[PROGRAMERDAVE]

I OWN A JOB SHOP WHERE I CUT MOSTLY PRE-HARDENED 4140(28-32 HRC) AND SOFT TOOL STEELS. CURRENTLY I HAVE 2 VF2'S (2006) AND 2 OLDER THAN DIRT VFOE'S. THE TREND IM NOTICING IS THE BALL SCREWS TEND TO GO OUT OFFTEN ON HAAS. I PROGRAM WITH MASTERCAM X5 USING DYNAMIC MILLING ALOT. WITH LIGHT RADIAL CUTS IM FLYING AROUND THE PART, BUT AT CERTAINS SIDES I SUDDENTLY GET CHATTER. THE TOOLPATH CARIES A CONSTANT CHIPLOAD SO I CAN ONLY ASSUME IT THE BALL SCREWS. FOR 85% OF MY PART, THE CUT SOUNDS PERFECT.

MY NORMAL PARAMETERS ARE:
.625 VARIABLE 5 FLUTE ALTIN COATED (1.250 LOC--USUALLY ONLY GO .900 DEEP WITH IT), ER25 COLLET IN A SHORT PROJECTION CAT 40, .030 AXIAL, 500 SFM (3056 RPM), .006 IPT (91.6 IPM) AIR BLAST COOLED. PARTS ARE CLAMPED SECURELY.

IVE HEARD FROM A FEW OWNERS THAT HAVE THE NEWER GENERATION LATHES AND THEY SAY THE QUALITY IS NOTICABLE IN THE NEWER MACHINES. FOR THOSE THAT HAVE BOTH, IS THERE THE SAME DIFFERENCE IN THE MILLS OR WILL I JUST BE SETTING MYSELF UP FOR REPLACING BALL SCREWS IN A FEW YEARS.

I KNOW HAAS HAS GREAT CUSTOMER SERVICE AND THATS GREAT AND ALL, BUT ESSENTIALLY WHAT WE'RE DOING IS HAVING TO CREATE A BUDGET TO MAINTAIN/REPAIR ON A LARGER SCALE THAN THE OTHER BRANDS. I JUST HOPE THE NEWER HAAS ARE MORE RELIABLE THAN THE OLD SO I CAN STICK WITH THE SAME BRAND I'VE RAN FOR ALL THESE YEARS.

LET ME KNOW WHAT YOUR OPINIONS ARE ON "GENERATION THEN" VS. "GENERATION NOW"

[gizmo_454]

We are a job shop as well. While we do not have any of the latest and greatest Haas machines, we do have a Mini Mill from 2006. This thing had, at last count about 6-8 months ago, over 14,000 hours and over 850,000 tool changes. So it has seen a bit of running, to say the least. I have cut everything from mild steel, to 4140 @27-34HRc, to plastic, to brass, to aluminum, to carbide (not something I will ever do again, but that's another story). It will still hold 0.0005" total tolerance day in and day out. No chatter issues either.

Not that it means anything, because I know it will not take the cut (load) that a VF2 will, (we have a 2002 VF2SS as well). Please step back and really think about this logically before you answer the question:

Are you sure that is a ball screw issue?

I ask this because you mention that it only happens on "certain sides" of the part. If the X ball screw was truly wore out, you would have chatter at every X change of direction. Especially since we climb cut, we are always pulling the table with the tool in the same direction the ball screw is trying to push it. Any backlash in there will come out as chatter, digging in, or if the backlash is bad enough, broken tools. The same for the Y axis.

When you change the ball screws and nut, does it fix the problem? When you change the ball screws and nut, do you replace anything else like the bearings in the pillow blocks? If so, have you ever considered changing just the bearings in the pillow blocks? Our swiss screw machine was having problems holding size/shape last year. One of the bearings holding the ball screw went out. Replaced it and all was good.

Just some other things to consider besides the screws. Even though this does not answer your primary question, I hope it helps to at least consider some other possibilities that may be causing your chatter problems.

Good luck!

Mike :cheers:

[txcncman]

Are you sure that is a ball screw issue?

I ask this because you mention that it only happens on "certain sides" of the part. If the X ball screw was truly wore out, you would have chatter at every X change of direction. Especially since we climb cut, we are always pulling the table with the tool in the same direction the ball screw is trying to push it. Any backlash in there will come out as chatter, digging in, or if the backlash is bad enough, broken tools. The same for the Y axis.

When you change the ball screws and nut, does it fix the problem? When you change the ball screws and nut, do you replace anything else like the bearings in the pillow blocks? If so, have you ever considered changing just the bearings in the pillow blocks? Our swiss screw machine was having problems holding size/shape last year. One of the bearings holding the ball screw went out. Replaced it and all was good.

Just some other things to consider besides the screws. Even though this does not answer your primary question, I hope it helps to at least consider some other possibilities that may be causing your chatter problems.

Good luck!

Mike :cheers:

+1

[Machineit]

THE TOOLPATH CARIES A CONSTANT CHIPLOAD SO I CAN ONLY ASSUME IT THE BALL SCREWS. FOR 85% OF MY PART, THE CUT SOUNDS PERFECT.

You say you use Mastercam, but unless you are using something much much more expensive, I don't believe that you are getting a consistent cutting, chipload or not.

Chipload is only one way to look at the cutting. The other is engagement. Making a pass at .05" deep on a side is totally different than running into a corner or such where engagement goes from .05" to 3/4 cutter width. You may be cutting .006" per tooth, but you are doing it for a much much broader area of the end mill, requiring more power and making it more difficult to evacuate chips.

Look at your procedure at the point of chatter.

And, I have never had to replace a ballscrew in 15 years of cutting with a Haas. They may not be the most rigid machine out there, but they are no light weight.

Mike

[Edster]

So your running a 5/8" end mill in an ER25 collet? Thats where I would start.

Try a Schunk Tendo hydraulic holder, or at the least a sidelock.

[murphdog]

We machine a fair amount of pre hard 4140 28-32 RC. Typically cutting .94-1.25 depth of cut using 5 flute 3/4" varibale pitch carbide. We do this on a VF4 using ER32 stubby holders. A link follows for a BT holder of the style we use. BT40 ER32 Short Collet Arbor + 8 Collets | eBay
I have only saw a handful of these in Cat 40 on eBay & I think I bought 4 of them.
Murph

[Machineit]

So your running a 5/8" end mill in an ER25 collet? Thats where I would start.

Try a Schunk Tendo hydraulic holder, or at the least a sidelock.

I agree with this post about the holder. I would not use a collet chuck for milling of that size. Use a standard endmill holder, as short as your job will accommodate.

4140 28-32 RC is sweet to machine compared to many things I do like 304 and 17-4 stainless and to mention exotics!

Mike

[mishikwest]

The er 25 is the first thing that caught my mind. IMHO that is your weak link. Your certainly using quality tools and the best programming strategy around . You should invest in a good milling chuck. And a set screw holder is NOT a good holder. Cheap, but not good. It inherinely pushes the cutter off center giving you runnout of some degree. A heat shrinker is a good alternative (however you need a inductive machine to go with it). Milling chuck is good too.

IMHO.

You say you use Mastercam, but unless you are using something much much more expensive, I don't believe that you are getting a consistent cutting, chipload or not.

Chipload is only one way to look at the cutting. The other is engagement. Making a pass at .05" deep on a side is totally different than running into a corner or such where engagement goes from .05" to 3/4 cutter width. You may be cutting .006" per tooth, but you are doing it for a much much broader area of the end mill, requiring more power and making it more difficult to evacuate chips.

Mastercam handles all of that. It will never, ever, ever violate your programmed radial engagement.

I am a Mastercam instructor and specialize in dynamic milling.