Tool holder run out.

I can't think of any political contributions for the group right now, so I'll post something on topic.

I use set screw type tool holders. I have TG and ER type collet chucks but I don't use them much. A lot of people disagrees with me, but I have found them to often have worse run out than "standard" tool holders.

I have a job coming up where I'll be running small cutters (1/32") in a material (copper) that cuts best at high SFM (600+). So I'll be using a high speed air spindle in the main spindle to get the RPM I need.

The air spindle is mounted with a straight shank on one end and uses a tiny collet to hold the end mill. I measured the run out on a tool and it is close to .001", which is not real great on a .031" tool, but is workable. I then measured the total run out between the tool axis in the air spindle and the main machine spindle and found the TIR was .005" which is high enough to put features cut with that tool out of spec.

This got me thinking. So I measured the run out on a few set screw tool holders and they're all around .002 TIR. Makes sense, there is about .001" clearance between the tool and the holder, and it is all pushed to one side, hence .002 TIR. Not too good, but at least it doesn't effect positioning accuracy of features in a part because the developed tool diameter is still concentric to the axis of the mill. It just wobbles a bit.

The problem is when you're cutting something without turning the mill spindle, like when you're using a high speed air spindle attached to a tool holder with run out. Your coordinate system could be off a few thou, which, in this case, is enough to mater so must be compensated for either in a work offset or perhaps I'll turn an eccentric sleeve to get everything in line.

Anyway, I know a few of you use these high speed attachments, and perhaps hadn't considered that some may not be perfectly in line with your spindle axis. A good quality attachment on a dedicated tapered shank will probably not exhibit any problems, but my setup does.

I have three mills in my shop, all with different tapers, so a straight shank tool seamed like a good idea at the time, but now it is adding up to more unproductive work getting it in line.

Reply to
Polymer Man
Loading thread data ...

"Polymer Man" wrote in news:

Kennametal GmbH makes some hydraulic holders, which allow you to dial in the concentricity of the tool. You might look into these. They aren't cheap, but they are GOOD.

Reply to

Shrinkers would likely work well here also.

Reply to

If you think it's alright that a .031" diameter tool is running out .001", than being relative to the ratio, you are alright with a 5/16" tool running out .010". Or a 5/8" diameter tool running out .020".

How about going the other way in size. If you use a standard of acceptance of a 1/2" (.500) Tool running out .001" then that standard puts a .050" diameter tool running out .0001" .

To make sure this accuracy is met, the discipline of cleanliness of the spindle taper/collet/collet nut is an absolute must EVERY time you decide to change the tool. Torquing the nut at the suggested rating must be followed. And the thing everyone takes for granted is the shank of the tool running out to the cutting diameter. Most manufacturers of small tools understand this. Manufacturers of tools that are trying to get into making small tools may not. Be aware, all small tools are not alike.

Another thing is of course your air spindle must spin 75,000 RPM for the 600SFM. These are typically a Set RPM due to the pressure coming into the spindle itself. If you try to adjust the air flow to set the RPM you might lose some of the torque the spindle is rated at. They don't have much torque in the first place. Try to get the spindle rated at the RPM you wish to run the tool at is my suggestion.

For your thought of the machine spindle not turning but the Air Spindle running in it, sure I suppose an eccentric sleeve will make up for it. Check out Ceratip or Mitsubishi, they offer a nice graduated sleeve in their insertable drill sections. Different OD/ID combinations available. Works well in a lathe to geet the insertable drill on center, works well on a mill to get the outboard insert of an insertbale drill to cut smaller or larger like a boring head would do, limited range of about .008" if I remember.

These are simply issues Call them mistakes if you wish) from past experience with getting miniature tools to run properly.


Reply to


You mean heat cinch tooling? Yeah, I don't have any of that.

I was in a shop a few weeks ago that had moved to heat cinch tooling for their new 40,000 RPM Makino. It was mesmerizing watching that mill put a finish pass on a big trode. He said the induction heating system and some other stuff added up to $20,000. That is quite a bit of an investment for tool holders, though a necessary one when your tool holder is spinning at nearly half the speed of sound.

Reply to
Polymer Man

I got a set of three NSK's in a nice mahogony box,,,same thing. The least eccentric one is .005". I don't use em anymore. These were purchased before I started working here, and weren't intended to be used this way. They do, however, make a line of electric, and pneumatic, spindles that are "VERY" concentric, I tested a couple. The electric ones had alot more torque, were dead-on concentric, and about $4,500.00 a pop.


Reply to

The first thing I'd do is try one of the collet holders (no collet). Mount it and then do a TIR on the collet taper. If it's out, reverse mount it. Try again. Then after the best mount, try the collet. TIR it and rotate it for the best concentricity. Work the holder and the collet a few times to see if you can get the concentricity you want. When you do, mark the holder and the collet so you can repeat the "line up."

Assuming you can attain a close enough runout, mount the endmill.

Surface Feet per Minute is only a recommendation. You can run lower if you want.

I use three flute Robbjack endmills. I take the endmill diameter and divide by 120 to devlope the chip load per flute. That 'times' three flutes 'times' the rpm gives the feed rate. Sink the endmill into the work no more than one half the endmill diameter per pass. I like stubby end mills. I plunge the endmill at about 25% of the sideways feed rate. Endmills don't come with enough end relief to plunge very well. Also this approach is for stubby endmills. A bit slower feeds will feel better with standard length tools.

** .031 diameter / 120 = .000258 chip load/flute 'times' 3 flutes = .00077 'times' 3000 = 2.33 inches/minute.

What ever rpm you use, feel the machine to check for abnormal vibration.

*Smile Use the fastest rpm which is smooth. Substitute that rpm for the one (3000rpm) in the formula.

The 120 is for slot cuts (full diameter cutting). If you are just roughing at no more than 70% cutter diameter then substitute 85 for the 120. This will give you about 1.5 times the feed rate.

This is the way I do it. Very few broken tools.

The material type doesn't matter too much. What matters, is rpm (for the surface feet per min.) and vertical depth of cut for tougher materials (as in steel etc.). When cutting annealed ofhc copper, the material isn't stiff enough to support the cutting. So we ease up on the sideways feed until the burrs go away.

I hope this helps.

Best regards,


Reply to
Stan Dornfeld

Don't be discouraged by the cost of the heating system. I have a dozen shrink fit holders, and I don't use anything but an oxy/acetalyne torch. I rarely change my heat shrink tools, so it's a very small inconvenience.

If I were you, I'd definitely buy a shrink fit holder from Command ($150-$180), heat it with a torch, and slip your air spindle in. As long as the taper on your spindle is good, you're not going to have any measurable runout.

If your spindle isn't in great shape, Lyndex makes a line of holders with a runout adjuster, similar to what Anthony already mentioned.

Reply to


Yeah, I'd had that same thought myself. I tried it, but gave up in frustration after about 10 minuets of screwing with it. Probably the best advice was to order an adjustable eccentric sleeve or an adjustable tool holder. But it didn't take very long to turn out a brass sleeve for a 1 1/8" tool holder and just make a permanent assembly out of it. Seriously, when is the last time you needed a 1

1/8" tool holder. So I used a cheater bar and ran it down tight, and the thing can just live in there from now on. It took a bit of fiddling with it, but I have the run out between the air spindle and the main spindle to around .0003" which is an order of magnitude better than it had been and is fine for me.

Yeah, I'm not sure but I think the theory is to prevent copper welding to the tool, which goes away above a certain SFM. I'm using ZrN coated tooling, so welding shouldn't be too bad regardless.

I'm about to zero out the fixtures and prove out the program, so I let you know how it goes.

Reply to
Polymer Man

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.