What's new
What's new

help with checking 5 axis center of rotation

Jvizzi

Aluminum
Joined
Jun 15, 2011
Location
Florida
So I want to use a tooling ball method of finding center of A axis tilt,taking 3-6 YZ readings at various A axis angles. But what I'm not understanding from other posts about this process, is how the Z coordinate of the ball is measured. My assumption is the only way is with a test bar and feeler gage block, after you have indicated XY center of the ball?

I do have a probe on the machine, but as I understand it, the probe's height accuracy is also dependent on a test bar during the calibration process?

I noticed several have recommended Karlo Apro's book, which I have on order, so my apologies if I am asking anything that's already covered there.
 
You're correct, to set the Z to the center of the ball a test bar (or other tool of known length) is the best way. The Z distance is critical to A axis pivot, so the more accurately you can set it, the better results you'll get.

What kind of machine and control are you doing this on?
 
So I want to use a tooling ball method of finding center of A axis tilt,taking 3-6 YZ readings at various A axis angles. But what I'm not understanding from other posts about this process, is how the Z coordinate of the ball is measured. My assumption is the only way is with a test bar and feeler gage block, after you have indicated XY center of the ball?

I do have a probe on the machine, but as I understand it, the probe's height accuracy is also dependent on a test bar during the calibration process?

I noticed several have recommended Karlo Apro's book, which I have on order, so my apologies if I am asking anything that's already covered there.

Yes and no... If you put a gage pin in say an ER collet, enter the length, say 4.10" and use that to calibrate your tool (stationary on table) probe, then calibrate the spindle probe, your tools and work offset will match up (Haas machine btw). It might not be the actual gage length of the tool, but if touched in the machine it doesn't really matter. I don't fully understand the mechanics behind it, but it works...

I know this because when I started this job all the spindle probes had different length offsets, as much as .25" BUT everything matched up in work offsets. I eventually ordered a calibration tool, like this
CAT40 Tool Probe Calibrator - Made in USA MariTool

Now using this standard, with diameter and length marked on the tool, I could use one tool on all machines to calibrate. Now all the machines are less than .002" difference on the spindle probe length.

edit: this all done on 3 axis mills, not sure what happens if the probe is not correct on 5 axis. I ran an first gen UMC750 and it included a calibration kit, with ball and calibration tools so...?
 
edit: this all done on 3 axis mills, not sure what happens if the probe is not correct on 5 axis. I ran an first gen UMC750 and it included a calibration kit, with ball and calibration tools so...?

you are right, on a vertical the probe height can be arbitrary, but not on a 5 axis. The tilt axis center of rotation must be measured from the gage line.
 
This is a Matsuura MX520 with a Fanuc 31i

why arent you using the easy 5 program? all matsuura machines come with the 5 axis calibration software and hardware. its stupid easy, position the probe roughly above the ball, hit cycle start and let it do its thing.
 
To my knowledge, this particular machine does not have easy 5. It is a 2010 model, and the original purchaser requested absolute bare bones on options to save money. As such it has 2mb memory, no data server, no offsets beyond G59, no Tilted work planes, about the only option it does have that it should is Tool center point control
 
To my knowledge, this particular machine does not have easy 5. It is a 2010 model, and the original purchaser requested absolute bare bones on options to save money. As such it has 2mb memory, no data server, no offsets beyond G59, no Tilted work planes, about the only option it does have that it should is Tool center point control

i'd still reach out to matsuura, the guys are very helpful. we bought a used machine also(2011) and they gave us all new macro programs etc to reload since the original owner did a bunch of weird shit on it.
 
After getting close with probing I dial in my Z by laying the trunnion over 90 degrees and making two facing cuts 180 degrees from each other on a piece of scrap. When the Z is right the thickness matches what it's programmed for. For X/Y I indicate the bore of the platter, spin 180, indicate again, and split any difference.
 
After getting close with probing I dial in my Z by laying the trunnion over 90 degrees and making two facing cuts 180 degrees from each other on a piece of scrap. When the Z is right the thickness matches what it's programmed for. For X/Y I indicate the bore of the platter, spin 180, indicate again, and split any difference.

I thought about this as well, but that is still dependent on knowing that tool's gage length very accurately, otherwise the web dimension is also being influenced by error in the length of the tool.
 
i'd still reach out to matsuura, the guys are very helpful. we bought a used machine also(2011) and they gave us all new macro programs etc to reload since the original owner did a bunch of weird shit on it.

Original machine supplied parameters are very different than purchased control options. Control options are not just supplied by the builder but control manufacturer. Also, certain ones need license from the Japanese government before they can be supplied.
 
check me if I'm wrong, but this is a trunnion style machine, right? The center of rotation has nothing to do with the gage length of the tool.

if it were a gimble style machine, the gage length would have everything to do with it.
 
check me if I'm wrong, but this is a trunnion style machine, right? The center of rotation has nothing to do with the gage length of the tool.

if it were a gimble style machine, the gage length would have everything to do with it.

In the above example, it would matter. As I am understanding it.

Suppose you tilt to A-90. then face your block at C0 , then without moving the tool in Zrotate and face at C180. Now, center of that web is center of rotation for A, assuming there is no error in the intersection of A/C axis. Now, the next issue is, you have to measure to the center of that web in machine coordinates, from the gage line, so unless you know that tool's gage length very accurately, your measurement will be wrong. Hence the test bar.
 
In the above example, it would matter. As I am understanding it.

Suppose you tilt to A-90. then face your block at C0 , then without moving the tool in Zrotate and face at C180. Now, center of that web is center of rotation for A, assuming there is no error in the intersection of A/C axis. Now, the next issue is, you have to measure to the center of that web in machine coordinates, from the gage line, so unless you know that tool's gage length very accurately, your measurement will be wrong. Hence the test bar.

no, not really. It's all relative. If your test bar is off, your tool setter will be off the same amount. The cal parameters for your probe will be off the same amount. All your tools will be off the same amount. It all comes out even.

Consider this, your spindle is going to contract and expand during the day. This will effect your tool heights, but has no effect on your rotary centerline.
 
Original machine supplied parameters are very different than purchased control options. Control options are not just supplied by the builder but control manufacturer. Also, certain ones need license from the Japanese government before they can be supplied.

i can tell you thats not the case with matsuura. they were able to supply us with everything we needed to get our machine running without any issues.
 
i can tell you thats not the case with matsuura. they were able to supply us with everything we needed to get our machine running without any issues.

I can tell you that is the case with Matsuura. If the machine was not originally supplied with the options, they have to be purchased and some options need to be approved before they can be supplied.

Your machine was shipped to the US with the options on it. If the previous user, screwed them up, than it is easy for Matsuura to get you the original settings for the machine. If the machine was imported with the options, it is a different scenario.

Andy Dukes
Yamazen
 
no, not really. It's all relative. If your test bar is off, your tool setter will be off the same amount. The cal parameters for your probe will be off the same amount. All your tools will be off the same amount. It all comes out even.

Consider this, your spindle is going to contract and expand during the day. This will effect your tool heights, but has no effect on your rotary centerline.

Right, I understand that the tool's lengths don't "move" the center of rotation, and that error in the length of the test bar will also be reflected in the tool setter, spindle probe etc. Perhaps it would be better to say, in the above method, your check of the A/Z center will only be as accurate as the tool's gage length measurement is accurate.

For example, if you program a cut at A-90.C0. , then A-90.C180. at the same depth you could still have error in the A/Z center measurement yet make the tool cut "correct" by fudging it's height offset.

no?
 
Right, I understand that the tool's lengths don't "move" the center of rotation, and that error in the length of the test bar will also be reflected in the tool setter, spindle probe etc. Perhaps it would be better to say, in the above method, your check of the A/Z center will only be as accurate as the tool's gage length measurement is accurate.

For example, if you program a cut at A-90.C0. , then A-90.C180. at the same depth you could still have error in the A/Z center measurement yet make the tool cut "correct" by fudging it's height offset.

no?

Yep, you should definitely set up the machine that way. Just use a tape measure to measure center points and fudge tool lengths until the part comes out right.


Why are you so bent on assuming a test bar will be incorrect length and therefore impossible to accurately find the center of rotation? That's ridiculous.

Measure 3 points. Use math to find center. It's not rocket surgery.

Here you go - stupid simple calculator for ya to use:
Circle defined by 3 points
 
You've gotta touch your tools off relative to something. So decide what that is and lock it down. Then with the facing method you get the COR relative to how you touch off your tools. It'll stay there until you change where you touch off tools from. I then store COR in G59 and it stays there forever. Sometimes I'll put 3 axis parts on the trunnion to save setup time since I don't have to pick up a work offset.
 
I think you would correct it by changing your Z offset, not your tool offset. But then you would need to verify that by probing the cut on another plane, like with A at 0 deg.
 








 
Back
Top