Really annoying run out issue

ukkie · Jul 10, 2020

Hi Guys,

I'm wondering if anyone can shed any light on what could be going wrong with my run out...

I'm using shrink fit holders and new solid carbide cutters yet I'm reading runouts as high as 40 microns on the Renishaw OTS. I initially thought that might need calibrated but the OTS seems to repeat within 0-3 microns every time. If I use one of the old shrink fit holders with a coated tool I can get it to down to around 3-4 microns. If I use a carbide tool it a about 35 microns out. I have 2 new holders that are also 30 microns or so out and the tool manufacturer has told me that the cutters cant physically be out that far as their machine rejects bar that's out by 6 microns...

I'm very new to machining so there is a high possibility that I'm doing something daft. Can the reading on the diameter (rotating) give a different reading as its only touching off on 2 parts? or should it still read exact even on something like an endmill? Also is it likely that a holder could be out? I am making sure everything is well cleaned before I put the tool in the holder and I've cleaned the spindle also.

Any help guys would be much appreciated.. I've been stuck on this for days now!

Thanks in advance

sirAIG · Jul 10, 2020

What does an indicator tell you? Runout should be dialed in via indicator, the tool probe I don't believe is able to tell you runout, but merely rotating dimension. One feeds the other, but sometimes cutters are just over or under

Sent from my SM-G955U using Tapatalk

DMF_TomB · Jul 10, 2020

ukkie said:
Hi Guys,

I'm wondering if anyone can shed any light on what could be going wrong with my run out...

I'm using shrink fit holders and new solid carbide cutters yet I'm reading runouts as high as 40 microns on the Renishaw OTS. I initially thought that might need calibrated but the OTS seems to repeat within 0-3 microns every time. If I use one of the old shrink fit holders with a coated tool I can get it to down to around 3-4 microns. If I use a carbide tool it a about 35 microns out. I have 2 new holders that are also 30 microns or so out and the tool manufacturer has told me that the cutters cant physically be out that far as their machine rejects bar that's out by 6 microns...

I'm very new to machining so there is a high possibility that I'm doing something daft. Can the reading on the diameter (rotating) give a different reading as its only touching off on 2 parts? or should it still read exact even on something like an endmill? Also is it likely that a holder could be out? I am making sure everything is well cleaned before I put the tool in the holder and I've cleaned the spindle also.

Any help guys would be much appreciated.. I've been stuck on this for days now!

Thanks in advance

.
who said end mill was sharpened with zero runout of end cutting edges to the shank ?
.
record runout on 100,000 tools in tool holders and compare runout amounts to tools you know for sure had runout problems. been my experience of many decades, runout has to be a lot to really give actual problems.
,
plus each machine spindle has its own runout. put test shaft in spindle and measure that spindles runout. you might be surprised. same tool in 3 different machine spindles usually has 3 different runout amounts

litlerob1 · Jul 10, 2020

Use an Indicator. If you're still getting .04mm runout, then take everything apart. Start at the ID of the machine spindle with an Indicator, and start testing out from there.

You haven't said what equipment you're using. So if you're talking about a benchtop $200 mill/turn machine you got from the toy store. That's the problem.

R

michiganbuck · Jul 10, 2020

likely you will have to plate check your holders.
few tenths error in a holder can make a thow in a tool that is reaching out.
Some times rotating a holder/cutter in the spindle can take out some run out.
some times you just make do with .0013 run out...

13engines · Jul 10, 2020

I think sirAIG is on to the problem. You basically can't measure run-out on a tool setter, even if you're touching the spinning tool off on two opposite sides of the tool setter pendent and calculating your way back to some number. You would have to know the exact diameter and location of the pendent head and the diameter of the tool being measured. Add up all the errors and uncertainty in that setup, and let's not forget the errors inherent in the ball screws controlling the measurements, and you'll be well outside the window of any high accuracy runout measurements you're hoping to put your money on.

Like others have said, measure runout with a high-ish resolution fixed indicator. Start at the tool end, and if you don't like what you read, work your way piece by piece back to the spindle socket.

litlerob1 · Jul 10, 2020

I'm suspect of the Machinery. Antique maybe? Cheep maybe? POS in general maybe?

But .04mm runout in a shrink fit holder---c'mon. Unless you're Tom, and your Tool is sticking out 15", that's more than is acceptable. Were it me, I'd almost automatically ask for my money back from the supplier (assuming it's on my Machine).

R

DMF_TomB · Jul 11, 2020

point is runout can be

1) from end mill itself not made with zero runout

2) from each machine spindle or each machine has runout in theory measure with a test bar AND of course when runout measured with 2 different test bars usually get some difference in runout measurements even with test bars

3) measure runout 1000's times and determine whats average or normal and what actually causes problems not somebody's opinion
.
.
i usually find 1% of worst tool holders and get then reground (taper reground) and all come back with much less runout but rarely perfect. yes and even brand new tool holders are often not perfect runout but usually better than old ones

ukkie · Jul 11, 2020

Hi Litlerob1,

Its a brand new VF4SS Haas I have. I had a Haas engineer out setting up the probe and checking the spindle aligment with the table only 3 weeks ago and Ive barely cut anything since as I was only doing test blocks. I was getting pretty poor join lines on contour cuts from tool runout, hence why I switched to shrink fit holders.

I've tried the indicator on the shank of the tool and it is showing about 3-4 microns but not 30 odd...

ukkie · Jul 11, 2020

Thankyou for the response sirAIG,

There will be a good level of incompetence on my part as ive only just started machining a month or two ago. I always thought that the ots diameter should tell you the tool diameter and if its reading a bigger size than the tool, that surely should indicate the tool is running out? So if I'm understanding correctly, rotating dimension and tool run out in this case will be two separate things? The figures are pretty high though, 30 odd microns surely cant be right? the indicator is showing around 2 microns on the shank.

If this is what to expect, how should I compensate for the cut? Im using fusion360. Do I set it to compensate from the machine or the software if its indicating this on the machine offsets?

sorry for all the questions... ive been getting nowhere with this!

ukkie · Jul 11, 2020

michiganbuck said:
likely you will have to plate check your holders.
few tenths error in a holder can make a thow in a tool that is reaching out.
Some times rotating a holder/cutter in the spindle can take out some run out.
some times you just make do with .0013 run out...

Hi yes we had basic ER collet holders when the machine arrived ( brand new Haas VF4SS) and the cuts had a huge step on the contour passes on the second op (.1 in some cases) so we diagnosed that the cutters weren't up for the job so we switched to shrink fit tooling and holders. Brand new tools from a well known brand and the same for the holders and I'm still getting this reading.

I cant help but think I'm doing something stupid as the WIPS was only calibrated a few weeks ago by a HAAS engineer and the spindle alignment checked and they said it was within 1-2 microns.

ukkie · Jul 11, 2020

litlerob1 said:
I'm suspect of the Machinery. Antique maybe? Cheep maybe? POS in general maybe?

But .04mm runout in a shrink fit holder---c'mon. Unless you're Tom, and your Tool is sticking out 15", that's more than is acceptable. Were it me, I'd almost automatically ask for my money back from the supplier (assuming it's on my Machine).

R

Hi its a brand new VF4SS Haas and all brand new tooling and holders. The strange thing is the ots is repeating within a few microns but its repeating miles out. If I use one holder and one tool I can get it within a micron or two of what I would expect the tool ) to be, but if I change the tool (even 2-3 tool changes in the same holder) then its miles out. If I use the other holders its also miles out but in line with the first holder (say 35-37 microns). Could I have repeat accuracy but the precision is out? or could it be that the tool I touched off with good precision had a completely different cut pattern than the endmills and me edge measure point is wrong?

ukkie · Jul 11, 2020

13engines said:
I think sirAIG is on to the problem. You basically can't measure run-out on a tool setter, even if you're touching the spinning tool off on two opposite sides of the tool setter pendent and calculating your way back to some number. You would have to know the exact diameter and location of the pendent head and the diameter of the tool being measured. Add up all the errors and uncertainty in that setup, and let's not forget the errors inherent in the ball screws controlling the measurements, and you'll be well outside the window of any high accuracy runout measurements you're hoping to put your money on.

Like others have said, measure runout with a high-ish resolution fixed indicator. Start at the tool end, and if you don't like what you read, work your way piece by piece back to the spindle socket.

Thanks for the advice 13engines.

Based on that, what should I then take my cutter comp from? If my machine is indicating a huge run out yet the true figure might only be a few microns, do I still use the machine offset as that will be the true rotating diameter?

Milland · Jul 11, 2020

Post a picture showing us how you're taking measurements (i.e. your indicator, your stand, etc.). Also, have you taken TIR readings of the spindle at different heights into the taper? If/when you do, you need to mark a "0" orientation point on the spindle such that you can watch for synchronous errors (are any deviations at the same rotation, or do they come at different values?).

Really, the machine taper should be "0" at any point you measure it, but after you confirm that the next thing I'd want to check is whether the Z axis is truly square to the Z travel, and to the X-Y plane. For this, you should have a "Lab Grade" granite right angle, on the order of 1-2 micron over 150mm accuracy. Then you can sweep (carefully, don't run into the granite) the indicator over the vertical granite face and look for deviations - do this at the four quadrants (0, 90, 180, 270) and record errors.

Deviations here mean adjustment of the leveling feet is needed, or more robust fixes if that doesn't get the column/travel square to the table.

Once the machine is certified good, you can properly review toolholder errors. At the least, you need to be certain about the spindle TIR at different heights, the granite square sweep will help you eliminate blend lines when cutting at different heights.

michiganbuck · Jul 11, 2020

Holders checked for run out and wobble.
Take a deep and shallow reading with marking where high and low occurs .so the runout is not compounded by the radial location of the error.

Check end mills out of a v block or turning in a close siza bushing.

13engines · Jul 11, 2020

ukkie said:
Based on that, what should I then take my cutter comp from? If my machine is indicating a huge run out yet the true figure might only be a few microns, do I still use the machine offset as that will be the true rotating diameter?

The easiest thing to do is start with the nominal radius of the tool and enter that. If you like, measure the tool with a micrometer or caliper and enter the radius of that reading. Especially if using reground tools. Then take a test cut. Every tool under varying cutting conditions in terms of depth of cut and radial engagement is going to finish at a different reading in both size and squareness do to flex in the machine, spindle, and tool under load. So try not to get the idea in your head that what you enter is going to be good as gold. Most comps need tweaking. Luckily the machine builders have giving us easy ways to do that.

As a rule, try to include cutter compensation in all your finishing passes. That way you can easily dial in your sizes by simply making small changes to comp at the control screen. What could be easier?

As far as not being able to get cuts to overlap perfectly, without seeing the entire setup and programming, it would be hard to figure where that problem is coming from.

On yet another note - have you checked your draw bar force? I know the machine is new but...

vmipacman · Jul 11, 2020

FWIW, .1 step deviation in contour passes between ops would not be attributed to toolholder type. There is another problem(s). If it was me, I’d drive what you have until you have a better knowledge base to pull from. Then invest in high end stuff. Nothing wrong with ER tooling.

pmack · Jul 11, 2020

Make sure your spindle taper and tool holder are absolutely clean.
Indicate your current tool with a very sensitive test indicator, mark a flute, record differences for each flute.
Remove the tool holder from the spindle, rotate it 180 degrees, and re-install into the spindle.
Do the indicator readings repeat for each flute? I'd bet not.
What you will likely find is the spindle has a few microns of run out, the holder has a few, and the tool has a few.
I would expect 5-10 microns run out in the spindle alone from the factory, you should have an inspection report for your machine showing what that is.
Even with shrink fit holders, we end up playing with tool holder orientation, and rotating the tool within the shrink to get minimal run out.
ER collet run out can actually help you get a better total runout by clocking the tool or collet for the best values for your spindle.

pmack · Jul 11, 2020

Your machine inspection report should be inside the electrical panel on your Haas. I just looked at my VF2SS report. 0.0001 at the taper, .0003 at base of test bar, and .0004 at far end of test bar.

Really annoying run out issue

Plastic

Aluminum

Diamond

Diamond

Diamond

Stainless

Diamond

Diamond

Plastic

Plastic

Plastic

Plastic

Plastic

Diamond

Diamond

Stainless

Cast Iron

Cast Iron

Cast Iron

Similar threads