Accuracy issues with my Makino...

[Bob W.]

I am machining a mold on my A51 with the rotary installed and I am having some accuracy issues and I'm not sure where to start with the troubleshooting. I am trying to hold .0005" tolerances and I'm only able to hold ~.002" with indexing, etc... The shop is temperature controlled but varies by 5 degrees over the course of a day. The issue showed up when I faced the side of a part at B90 C0.0 then rotated the part 180 degrees and faced the other side at B90 C180. The part came out .0032" thin. This can either be caused by inaccurate locations of the B or C axes (B is off in Z direction or C is off in Y direction), or the tool length is incorrect. I have a thorough probing routine that takes a dozen or so measurements and verifies the axis locations and they are all within .0002"-.0003". I checked the accuracy of my laser tool setter by measuring the standard and it came in within .0002". I remeasured the tool and the new length came out SHORTER than the original length which is opposite of what it should have been given the measured results on the part. At this point I'm a little stumped and I don't want to move forward and waste a ton of time making scrap. Any ideas where I should be looking? Chips between the pallet and Z-axis?

 

What sort of probing or tool qualification procedures do people do to get into the tenths on more precise work? I have been fighting this for a while and it is getting frustrating. I do have my spindle probe working and setting DFO values during the program, I just tested and got that proven out tonight so I can run probing routines between tool changes pretty seamlessly. I'm not sure if I should have the offsets updated to reflect a change in the axis position (G54) or the fixture position (G54.1). If this is a thermal drift issue the axis positions would be moving and I would want to update G54.1, if it is related to pallet seating I would want to update G54. I'm not sure how I would tell the difference... Any thoughts?

 

So in a nutshell, here is how it went today:

 

1. Part came out .0032" thin.

2. Remeasured tool, new measurement was .001" shorter than original, should have been .0016" longer.

3. Verified laser by measuring standard, measured .00025" short

4. Removed fixture from rotary table and ran probing routine (multiple times). All axes were within .0002"-.0003" in X, Y, and Z

5. Sat down and scratched head.

6. Started typing...

 

Also, I have been tracking coolant temperatures and over the course of a day of hard running the coolant heats up 4-5 degrees. The ambient shop temperature is 73 degrees and the coolant starts at 70 degrees and ends up at 74-75 degrees. The shop temp generally varies from 69-75 degrees or so.

[cincy k]

How have you verified your spindle probe gage length and tool laser match?

[Greg Williams]

Was the machine setup accurate enough for this part in the past?

Basically did it work before?

Does the machine have face contact tooling HSK, bigplus?

Does the spindle temp vary?

Can you measure the spindle without a tool, then run it for a period with a tool so you do not damage the fingers then measure it again?

Can you do the same test with a master tool?

[DavidB]

Sounds like the machine needs the orientation point of the rotary axis set.

I ran a Makino D500 and had similiar issues. We then checked the positions of the centre of roation relative to the home position, which are set in parameters.

This made all the differance.

 

DMG are great for this as they use software called 3D Quick set. Still the most easiest and accurate way I have seen to set a 5-axis machines centre of rotation up.

 

I had a Japenese tech come out from Makino and he had to cut a block and measure it as he went, it took him half a day to recalibrate the rotary positions.

Once it was set though the machine was good.

 

If you machine a square about your X,Y zero datum (G54) from the Top. Then rotate it B90. Now using a dial indicator check the C-axis at 90 increments. Each side of the machined square should rotate around C axis the same. Also checking the top face with an indicator then rotate C axis 90 degrees, each side should read the same Z height.

 

HTH

[GoetzInd]

DMG are great for this as they use software called 3D Quick set. Still the most easiest and accurate way I have seen to set a 5-axis machines centre of rotation up.

 

Renishaw offers something very similar for most machines.

 

Mike

[betts]

Was the machine setup accurate enough for this part in the past?

Basically did it work before?

Does the machine have face contact tooling HSK, bigplus?

Does the spindle temp vary?

Can you measure the spindle without a tool, then run it for a period with a tool so you do not damage the fingers then measure it again?

Can you do the same test with a master tool?

 

I would agree that Greg's questions need answered, primarily "has it worked before?" as you are getting into SO many variables when pulling down to that tolerance, on a mill, that the list is quite long.

[gcode]

It could be as simple as a chip in the toolholder

The tool that made the thin part should have checked .0016" long.. but it didn't

(cause the chip wasn't there anymore???)

 

You didn't say what kind of tool it was... could it have been a face mill?

(with one insert not seated properly???)

[Jeremy Herron@DBS Solutions™]

My first guess would be what David suggests.

[Bob W.]

Okay, I'm back at it. I will answer some of these questions as I get the time. I ran the probing routine with no machine warm up and here are the axis shifts:

 

X offset of B-axis: +.00017

Z offset of B-axis: -.00021

X offset of C-axis: -.00021

Y offset of C-axis: .00037, easily changed by modifying work offset.

 

Standard true length: 5.00055

Standard measured length: 4.99945

 

These are all values without any machine warm up. The machine is running the warm up cycle right now, then I will redo these tests.

[Bob W.]

Another thing I should mention is the face of the rotary is not parallel to the XY plate, it is off by .004 degrees and I compensate for this by adjusting the B value of the work offset to .004. I'm not sure if this would affect how things run in DFO or not. The face of the rotary is normal to the C-axis though, so with the B-axis adjustment the C-axis is parallel to the spindle axis.

[Joe788]

How are you measuring the part to see that it's .0032 thin? Is it .0032 thin at the top of the part's Y, middle of it's Y, and bottom of it's Y? Also, is it .0032 thin at the bottom and top in the Z direction? If the two cut faces are perfectly square/parallel, you can rule out rotary problems for the most part.

 

What is the material, the tool, and gage length of the tool/holder assembly?

 

 

Also, measuring the master on the laser doesn't really do anything (unless your master is a nice sharp endmill that you can take a cut with.)

 

Face at B90, face at B270, then spin back to B0 and measure that width with the probe. Adjust that tool length until the width is DEAD NUTS, then use that as your master.

 

.0032 is a MILE. We don't see that much on 4 or 5 axis machines here, even with 25-30 degree temperature swings. I'm guessing it's going to be something simple.

[Bob W.]

It could be as simple as a chip in the toolholder

The tool that made the thin part should have checked .0016" long.. but it didn't

(cause the chip wasn't there anymore???)

 

You didn't say what kind of tool it was... could it have been a face mill?

(with one insert not seated properly???)

 

The tool was a 3/8" MA Ford end mill, 138 series and I was probing on the flute corner, not the tool center.

[Bob W.]

How are you measuring the part to see that it's .0032 thin? Is it .0032 thin at the top of the part's Y, middle of it's Y, and bottom of it's Y? Also, is it .0032 thin at the bottom and top in the Z direction? If the two cut faces are perfectly square/parallel, you can rule out rotary problems for the most part.

 

What is the material, the tool, and gage length of the tool/holder assembly?

 

 

Also, measuring the master on the laser doesn't really do anything (unless your master is a nice sharp endmill that you can take a cut with.)

 

Face at B90, face at B270, then spin back to B0 and measure that width with the probe. Adjust that tool length until the width is DEAD NUTS, then use that as your master.

 

.0032 is a MILE. We don't see that much on 4 or 5 axis machines here, even with 25-30 degree temperature swings. I'm guessing it's going to be something simple.

 

I hope you are right that it is something simple and I tend to agree. The machine repeats spot on. I used the standard because that is what is used to calibrate the laser. If I am ever unsure about the calibration state of any of my tool setters I just probe the standard to verify. It is quick and easy. I measured the part with micrometers that were just calibrated last week. I also verified the mic with the standard and it was dead on. The part is 3" tall and it has .0002" of taper from top to bottom which is well within what I would expect.

 

Material is aluminum

Gage length is ~5.0"

[Guest]

Have you tested the laser for straightness in Z?

[Joe957]

ive had issues with chips on the pallet seating cones on our a51's. they were thin enough to not throw the air gap alarm, but enough to cause some issues higher up on the tombstone. The sensitivity of the gap switch is adjustable. not sure how the nx is configured, but check under the shield that divides the two tables. Its a place that chips like to hide and this swings over the seating area during a pallet change. If you are comfortable in maintenance mode, raise the apc and bring the table forward and clean the cones to eliminate the possibility. (be sure you know where machine z was when you lifted the apc to bring it back when you are done) Also check under the tables in the 4 pockets and verify everything is clean....

[Bob W.]

Thanks Joe, I will check that. I am making some progress here. I am working Per DavidB's advice and cutting test samples. A few things I have found, the B and C axes are off, but not by much. The bottom of the tool was NOT flat so we are inserting a new cutter for more tests. Per James recommendation I checked the laser alignment and it was out but not by much, went ahead and re-calibrated. It looks like this is a stack up of several things that were out by .0002" here, .0005" there, etc... Tests with the new tool will give pretty good insight as to where the axes are to .0001" or so. Then I'll adjust my offsets to hit the middle and be off to the races.

[Guest]

A 20mm sharp e/m on a beam that is off in Z .1 Deg will give you .003mm error. The larger the tool,the larger the error.

[DavidB]

If your using a laser to measure tool length don't measure endmills on there centre line. Only measure ballnose cutters and drills on their centreline.

[Bob W.]

A 20mm sharp e/m on a beam that is off in Z .1 Deg will give you .003mm error. The larger the tool,the larger the error.

 

The beam was aligned to .00008".

 

If your using a laser to measure tool length don't measure endmills on there centre line. Only measure ballnose cutters and drills on their centreline.

 

End mills are always measured right on the flute.

 

I'm still perplexed about this. I can measure my standard and it is consistently within .0002" but the end mill is consistently measuring .0005" short. I got the axes dialed in right on the money via test cuts etc, but the tool always probes short. I went so far as to probe the standard in my PS95 with a touch probe (perfect), then probe the tool and record the value. Then I put the tool back into the A51 and it is .0005" short.

[gcode]

I'd check the taper on the tool holder next

[Guest]

One of the dirty little secrets that "laser guys" don't like to admit (out loud anyway) is that the polish on an endmmill can have an affect on the point at which the measurement is taken. High Polish inserts on shell-mills are theeeeeeeee worst culprits, but endmills are not immune.

 

Each measurement system has it's own set of strengths and it's own set of weaknesses and you have to look at the application and accept the drawbacks of each. Now, that being said, both systems are pretty reliable and the manufacturers of these systems do a pretty good job of mitigating the issues at hand but the closer you want to measure the more magnified the issues become. It's just the nature of the deal.

[GoetzInd]

One of the dirty little secrets that "laser guys" don't like to admit (out loud anyway) is that the polish on an endmmill can have an affect on the point at which the measurement is taken. High Polish inserts on shell-mills are theeeeeeeee worst culprits, but endmills are not immune.

 

+1. I've seen repeatable different results with the exact same tool with different coatings. That's what's nice about having a presetter. A lot more accurate IMO.

 

Mike

[Bob W.]

It isn't often when I really need to hit better than .001" true position but this is one of those times unfortunately and this laser is making it damn near impossible. This is for a small mold that has a 3D parting line and if the gap is bigger than .002" there will be flash. The gap of .002" is with a stack up of several parts so if each is off by more than a few tenths it will be a mess when they are all assembled. Pretty frustrating but it is looking like a presetter is a necessity right now. I don't know how I can make these molds effectively without one at this point. The probing is really working well in tracking thermal movement but then the tool length is out .0005" or so...

 

On another note, my B and C axes are misaligned by .00035". Is that worth trying to tap in to better than .0002"?

[Joe788]

Pretty frustrating but it is looking like a presetter is a necessity right now. I don't know how I can make these molds effectively without one at this point.

 

As bad as I want to purchase a new presetter - I can't justify it because the following process works so damn well:

 

Pick a tool that you want to use as your "master" - preferably something that the other tools for that program are going to need to match perfectly with.

 

Do the same B90 facing, B270 facing, B0 X measurement I described earlier, and dial in that length offset.

 

Presumably you have at least .010 or so extra stock in the Z direction, on the material you're using for this job.

 

Take a little test facing cuts with each of the tools at B0, starting with the "master" tool. With ball mills, you'll need to do a very fine zig zag to get a flat/accurate enough surface to probe.

 

Write a probe routine that probes the master tool's B0 test cut, and set's that as Z0.

 

Then probe each spot from your other tools' test cuts, and let the Renishaw 9811 macro update the tool length of each tool.

 

Throw in a new piece of stock, and run the program again. The second time, every tool should be under .0001

 

Here's a screen capture of one that I run right now, that blends .5, .375, .25, .156, .125, .0937, .0625, and .019 endmills all to perfection.

 

If you're doing this on a daily basis with tons of different tools, obviously the presetter will pay for itself fairly quickly. But if you have a pretty standard set of tools that need to be blended - you'll find yourself having a hard time parting with $30K to get the exact same results. (Although, I do have a crappy old TMM900 that I use to get tools within .0006 or so - which might be part of why I can't justify dropping the coin on a brand new one)

 

 

It takes 5-10 minutes to make the cutting and probing program, but then it's saved with the actual part program, and it can just run with the push of a button the next time that job is being set up, or the next time you need to change one of the tools on that job.

[Bob W.]

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?