Accuracy issues with my Makino...

[Joe788]

One thing that attracts me about a presetter is there is no thermal error added from the machine tool. It is a completely independent standard and that makes it much easier to isolate accuracy. If I were to set the tools as you describe then need to replace a tool after a few hours of running for whatever reason, that tool will be off in left field with respect to the others. A presetter eliminates that issue so all I really need to track on the machine is thermal drift and I'm not trying to keep tabs on thermal drift and tool accuracy. Part of the frustration of the last two days is that with a horizontal nothing is fixed, tombstone, spindle, anything... so determining where the root of the error is becomes a real challenge. A vertical is much easier to deal with in this case for sure. The table is always square to the spindle (hopefully) and it never leaves the machine. A presetter would help to lock down one of these sources of error, but at a cost, as always.

 

Some days I wonder if it would be worth investing in a pallet/tombstone and setting it up specifically for calibration routines of the probe and machine. If there is any hint of an issue bring in this tombstone and run the cycle which would have the reference geometry to calibrate the probe, find the axes and completely troubleshoot everything in a matter of minutes with a dozen or so probe touches. Anyone do this?

 

In the event you only need to replace one of the tools and you're satisfied with where everything else is - you skip the initial B90 facing, B270 facing/B0 measure portion of it. The routine only sets the tools relative to the "master" tool again. So whether the machine is hot or cold, any tool you replace is going to come out perfect matched with what you've already got.

 

The presetter is definitely a wonderful tool that's worth having - it just depends on how many other $20,000 items you need worse.

[GoetzInd]

it just depends on how many other $20,000 items you need worse.

 

Haha I know how you feel. I have to ration out my 10K+ requests to keep the boss from killing me. Pre-setter is def worth it though. Remember , measuring tools is only a small part of what they do.

 

Mike

[cincy k]

One of the problems I see with a tool setter is you cannot account for thermal changes of the spindle at operating speed. With the class of machine tool you have this shouldn't be much of any movement so you may be okay, I have issues with it having lower class machinery. This is where taper and face contact help as well (HSK). Also, this is where i see having something in the machine to measure the tool such as a laser is helpful. Call the mold and die guys at Makino and ask them which laser they use and see if you can apadt that to your horizontal. I believe you said you have a split rail system. Maybe that's the culprit. Food for thought.

 

In the end I would still go with the presetter for the reasons you mentioned. Vacuum or mechanical retention of the tool as it's being measured!!!! Oh and RFID chips too if you can swing it.

[Sticky]

When trouble shooting, start from base, and work your way out.

 

So, how square is your machine? Do you have values for YZ over 300-500MM? How about XZ? You only need to be 5 microns out or less for either of those to see the error you have.

 

Backlash?

 

The most likely cause of all of this, is the fact that you have a 40 taper holder with a 5" gage length. Depending on the part material and your S&F (cutting pressure) you could easily cut .002" deeper then programmed from deflection alone.

 

Deflection and thermal growth are the reason I haven't bought a presetter. Whenever you change your cutting parameters, or the tool losses sharpness your cutting pressure changes and this WILL affect your cut result, both for wall taper and floor/Z depths.

 

I do as Joe does, 9811 is your friend! The only thing I add to his method is I use (best I can anyways) the same cut parameters (S&F, ADOC, RDOC) that the tool will actually use in the program. This is the only way IMO to get it t1ts.

 

With a 40 taper, and 5" gage, even on a little 3/8 tool, I would PLAN on it cutting at least .001-.002" deep if you are taking any sort of healthy cut. I can actually get a 1/2" em to cut about .01" deeper then set and programmed without getting too crazy. Everything moves and deflects when you put force on it, how much is your responsibility to measure.

 

To prove this use the same tool and take varying depths of cuts, get more aggressive each cut and probe in between cuts. You will see you cut deeper then programmed, incrementally, on each cut. And your wall will have more taper too.

 

A presetter is not going to solve your problems.

[Sticky]

Oh and about your "calibration pallet", I wouldn't recommend it. Because then you have to throw pallet repeatability into the mix, and while its usually .0002" or less, its still going to add a lot of tail chasing, and likely for nothing.

[Mick]

One thing that attracts me about a presetter is there is no thermal error added from the machine tool. It is a completely independent standard and that makes it much easier to isolate accuracy. If I were to set the tools as you describe then need to replace a tool after a few hours of running for whatever reason, that tool will be off in left field with respect to the others. A presetter eliminates that issue so all I really need to track on the machine is thermal drift and I'm not trying to keep tabs on thermal drift and tool accuracy. Part of the frustration of the last two days is that with a horizontal nothing is fixed, tombstone, spindle, anything... so determining where the root of the error is becomes a real challenge. A vertical is much easier to deal with in this case for sure. The table is always square to the spindle (hopefully) and it never leaves the machine. A presetter would help to lock down one of these sources of error, but at a cost, as always.

 

Some days I wonder if it would be worth investing in a pallet/tombstone and setting it up specifically for calibration routines of the probe and machine. If there is any hint of an issue bring in this tombstone and run the cycle which would have the reference geometry to calibrate the probe, find the axes and completely troubleshoot everything in a matter of minutes with a dozen or so probe touches. Anyone do this?

 

I've done that. We manufactured a master tombstone that we kept on a pallet in a FMS. We had a probing routine that probed a set of features, and then dumped the results into a file, which was sent back to the cell controller, and then imported into a spreadsheet. The results were then plotted over the course of months to track any shifts in the machine.

 

We did this as our city was rocked by two major earthquakes, and we had to endure a number of aftershocks of varying sizes for months afterwards. We could track what was happening to the machine. It worked really well, and having it graphed, and coorelated to the dates of aftershocks allowed us to see if the aftershock(s) had affected the machine.

[Bob W.]

To prove this use the same tool and take varying depths of cuts, get more aggressive each cut and probe in between cuts. You will see you cut deeper then programmed, incrementally, on each cut. And your wall will have more taper too.

 

These facing passes had finishing depth cuts of .005" so there really wasn't any cutting force to speak of, certainly not enough to create that much error. I also do my best to maintain consistent parameters for side milling and finishing and I understand that when the wear comp is dialed in for the tool it is only valid for the cutting parameters that created the feature that was measured to set the comp. These are all really light cuts with no tool load whatsoever, finishing surfacing passes, facing passes, and contour passes. There is no doubt that the laser tool setter is measuring short because it varies from the PS95 values by .0005" for the same tool after both machines accurately measured the probe standards.

 

I definitely need to rethink how I am doing things and take a more systematic approach. It makes for stressful days when I have such a huge work backlog. I will take some time to measure the squareness of the machine this evening and see where that stands.

[Guest]

Working with a customer the last few days with a laser and they are trying to hold the stated ±1 micron number in Renishaw's manual.

 

They've got a greater than 1m span. It's not going well for me. They run the machine in metric so I don't have to try to split .0001", I already can; 3 ways as a matter of fact. But the machine's stated accuracy is ±2.5 microns so in reality the absolute very best we can expect is ±3.5 microns. Add into the mix tool coating wear (with a coating thickness range of 2~15 microns depending on the coating), built up edge on the tool. It just makes me want to pull my hair out.

[GoetzInd]

Working with a customer the last few days with a laser and they are trying to hold the stated ±1 micron number in Renishaw's manual.

 

Man that sucks. Personally I wouldn't rely on any conventional tool probe for under .0005 and not expect constant messing around . The vision based systems on the micro machines are a different story though. Never seen one that was retrofit-able though.

 

Mike

[Newbeeee™]

With a 40 taper, and 5" gage, even on a little 3/8 tool, I would PLAN on it cutting at least .001-.002" deep if you are taking any sort of healthy cut. I can actually get a 1/2" em to cut about .01" deeper then set and programmed without getting too crazy. Everything moves and deflects when you put force on it, how much is your responsibility to measure.

Sticky - how is this happening? Is this weak pull stud retention so the tool is pulling into the part?

[Joe788]

Working with a customer the last few days with a laser and they are trying to hold the stated ±1 micron number in Renishaw's manual.

 

They've got a greater than 1m span. It's not going well for me. They run the machine in metric so I don't have to try to split .0001", I already can; 3 ways as a matter of fact. But the machine's stated accuracy is ±2.5 microns so in reality the absolute very best we can expect is ±3.5 microns. Add into the mix tool coating wear (with a coating thickness range of 2~15 microns depending on the coating), built up edge on the tool. It just makes me want to pull my hair out.

 

Yikes. Might want to pull the eject handle on this one early. Even if you get it dialed in right now, next week they're going to run the thing hogging aluminum at 20K rpm for 12 hours straight, measure a tool .0002 too long, and then call you and rip you up one side and down the other for the machine not being in spec.

[Sticky]

These facing passes had finishing depth cuts of .005" so there really wasn't any cutting force to speak of, certainly not enough to create that much error. I also do my best to maintain consistent parameters for side milling and finishing and I understand that when the wear comp is dialed in for the tool it is only valid for the cutting parameters that created the feature that was measured to set the comp. These are all really light cuts with no tool load whatsoever, finishing surfacing passes, facing passes, and contour passes. There is no doubt that the laser tool setter is measuring short because it varies from the PS95 values by .0005" for the same tool after both machines accurately measured the probe standards.

 

I definitely need to rethink how I am doing things and take a more systematic approach. It makes for stressful days when I have such a huge work backlog. I will take some time to measure the squareness of the machine this evening and see where that stands.

 

Its a 5" gage length, there will be some deflection. But the cut parameters you are talking about have me thinking its more a squareness issue then anything. Do you have a large 5 sided square you can use to check the squareness of the machine?

 

Sticky - how is this happening? Is this weak pull stud retention so the tool is pulling into the part?

 

Retention is one potential and common cause, a worn taper is another. In this case, the long gage length and small diameter are going to be the largest causes of deflection, they just give/bend when force is applied to them. You might be surprised how much a 3/8 carbide end mill will bend before it snaps.

 

 

Yikes. Might want to pull the eject handle on this one early. Even if you get it dialed in right now, next week they're going to run the thing hogging aluminum at 20K rpm for 12 hours straight, measure a tool .0002 too long, and then call you and rip you up one side and down the other for the machine not being in spec.

 

I was thinking the same thing, this has long term stress written all over it.

[Newbeeee™]

Yikes. Might want to pull the eject handle on this one early. Even if you get it dialed in right now, next week they're going to run the thing hogging aluminum at 20K rpm for 12 hours straight, measure a tool .0002 too long, and then call you and rip you up one side and down the other for the machine not being in spec.

But sales have done the hard thing Joe - getting the purchase order.

'Yeh yeh yeh of course it can hold a micron - The readout shows .001mm and the rotary is 3600000000 of a degree'......

 

Taxi!

[Guest]

The machine is already installed and been running for probably 6 months now. They are going to run some "really close tolerance" parts and need more accuracy/repeatability on the tool measurement front. Too late to eject. Nobody will be able to do much better. I mean we're talking a few microns here. .0001" I WISH I was only worrying about .0001", 1 micron for the uninitiated is .00003"

 

I think I'm going to go pass out now.

 

I'm SO glad this is a quality machine tool. At least that variable isn't something I have to worry about.

 

Remember that discussion about taking engineers out behind the woodshed and beating them like a rented mule... I'm thinking that applies here.

[Newbeeee™]

The machine is already installed and been running for probably 6 months now. They are going to run some "really close tolerance" parts and need more accuracy/repeatability on the tool measurement front. Too late to eject. Nobody will be able to do much better. I mean we're talking a few microns here. .0001" I WISH I was only worrying about .0001", 1 micron for the uninitiated is .00003"

 

I think I'm going to go pass out now.

 

I'm SO glad this is a quality machine tool. At least that variable isn't something I have to worry about.

 

Remember that discussion about taking engineers out behind the woodshed and beating them like a rented mule... I'm thinking that applies here.

Foggy - being curious. What are they doing and what tolerances (ie is it bores to a diametric tolerance or hole positions to a positional tolerance).

Just curious as to what the cartoonist has specified.

 

And how are they checking this off the machine....RandR etc?

[Guest]

Foggy - being curious. What are they doing and what tolerances (ie is it bores to a diametric tolerance or hole positions to a positional tolerance).

Just curious as to what the cartoonist has specified.

 

And how are they checking this off the machine....RandR etc?

They are making prototype parts.

 

Chew on this for a bit to see what that word "micron" that gets thrown around in such a cavalier way really is.

[tozmaster]

Oh Boy the proverbial RCH goes from fable to fact.

[Newbeeee™]

I know what one is 'cus I work in metrico all day long, but I've never seen one

It's funny - a couple of tenths (5microns) used to be a real tight tolerance. but that's nothing nowadays in a lot of peoples heads. But the overwhelming majority are kidding themselves.

As we have beaten to death before, CAD and standard 2 decimals and position tolerance etc dimension templates have a lot to answer for.

[Guest]

I'm I the process of accounting for every micron, coolant temp, ambient temp fluctuations, tool growth/shrinkage, spindle growth, machine growth, laser bracket growth, tool wear/coating wear, etc...

 

It's a living.

[tozmaster]

. I think I found one you missed

[Guest]

. I think I found one you missed

I'm sure there's a bunch I missed.

 

My head hurts already.

 

[Newbeeee™]

I'm I the process of accounting for every micron, coolant temp, ambient temp fluctuations, tool growth/shrinkage, spindle growth, machine growth, laser bracket growth, tool wear/coating wear, etc...

 

It's a living.

Hmmmm, so you probably have hair like the guy who presents Ancient Aliens soon to be followed by hair like Elmer Fudd

[Zoffen]

IT MUST HAVE BEEN ALIENS!!!! DUR!!!!!

[Bob W.]

I think I have found the culprit. My spindle chiller unit isn't working correctly... This evening I ran a tool at 12k rpm for 20 minutes. Before running the tool I measured the standard and it measured at 5.00001". After running 20 minutes the standard measured 4.99919", or SHORTER by .00082". This is in only 20 minutes. After running surfacing toolpaths for several hours it is probably much worse. The chiller unit cools the spindle AND ball screws and if it is running cold things will shrink and parts will be cut small, which is exactly what I have been experiencing. If I measured a tool at the beginning of a program and did extended cutting with indexing and rotary moves and tool shrinkage would be amplified resulting in things being off by a mile, like .0032" I will be calling Makino service first thing in the morning.

[Newbeeee™]

Bob,

Which way does your chiller work? Is it absolute temperature or does it track and adjust to ambient?

Reason I say is we had a 10krpm Leadwell that popped a spindle. Tech said wow that chiller is set too high at 15degrees. It should be set for 5 degrees so it chills the spindle 5 degrees less than shop/ambient temperature.

New spindle went in with chiller set to 5 degrees. End of the day we realised the spindle was wringing wet with condensation and freezing to touch, because it was set for 5deg absolute temp. Damage was done and spindle only lasted a few weeks after this.

Leadwell had both types of chillers and you needed to know what type...

Just a tale from the dim and distant past