G68.2 locations seem off.

[Carle387]

Hello everyone,

So I work in an environment where we do a lot of 3+2 machining on a Toyoda Fanuc 5-axis with a table/head configuration machine.  We've been utilizing G68.2 more and more instead of having to touch off a new work offset for every table or head rotation.  I am growing concerned that the center of rotation of my table is not accurately defined.  It seems to me the every time I rotate about the Z axis my locations in the X and Z seem to be off.  This last occurrence I had created a contour with an end mill that was my X0 location.  While still in on that plane I had a countersink run that was spot on.  I next had the part rotate 90 degrees around the Z axis.  Drilled and had a countersink on that plane.  The hole turned out to be off location and the countersink didn't even touch the part on a surface I created and should have been spot on. 

We have a sub pallet we added but at the time no center mark was made to go back and calibrate to.  I am looking for ideas on how I can check my center of rotation to confirm my suspicions.  The upper powers that be think I am all wet.  I thought I could go back and create an edge with an end mill.  Rotate about the Z axis and come back to the same profile with the same end mill and see if that is right on the money or if it too is off.  My thinking if all is as it should be my end mill should be right on that profile, anything else shows the center of rotation is off.

Is my methodology seem sound or am I not completely understanding the whole Tilted Work Plane process?  Any opinions are welcome.

Thanks

Carl

[crazy^millman]

Simple test block or anything you can get to from different angles. What some people do it mount a sphere on the machine. Sweep it in and then move it to many different places. If it doesn't repeat then that confirms your correct the machine's parameters for controlling the G68.2 position are wrong. When they are wrong your best programs will not make a good part. I have had this happen about a 1/2 dozen times over the years. Chase and chase parts and then they get the correct parameters in the machine and guess what programs originally made were good after all. What is really fun is when people think your time is free and all that chasing you had to do that was extra shouldn't be paid for.

If you suspect the machine is off then you stop everything and you make sure it is not off. You never keep running a machine with a problem, but like most places your place is doing what they do. Put their fingers in their ears and sing sounds to drown out the noise. Should start calling you a stinky head and arrogant know it all and many other choice names before the light bulb goes off. Well we always did it this way why are you trying to do it easier and faster? Just because we are losing customers and our quality is going down hill why would even suggest methods and processes to make us more productive? Your not a company person trying to make us more money. Quit and just do your job and be happy you have a job. Any of that sound familiar?

No your thinking is not off and that is the problem. Your thinking and when something is beyond someone else grasp to understand it always easier to call them names or pick on them or even threaten their jobs than try to get to the bottom of the problem and get it solved. We don't have time for this and got a good example over the last 2 weeks. Simple parts and found a major problem with a post. No one ever took time before to solve the post problem. Chase issues for 2 weeks that with a good post would have never came up. Cost them a late delivery and some scrapped parts. Now we are closer to getting the post issues solved, but if they had been solved originally then it wouldn't have cost me so much extra time and customer extra time and created such havoc, but this is what seems to be the normal course of action in Manufacturing. No time to get it right from the get, but plenty of time to keep doing it over and over and over.

Press on and hopefully you can get the machine rep to come in and talk some sense into management. Even then it normally takes a couple more failures before they stop and listen to what your really telling them. Please keep us posted.

[Carle387]

Yes, I have witnessed a lot of those scenarios in my current place of employment.  We like to stick our heads in the sand and hope the problem goes away.

 

I miss spoke in my initial post.  I am actually rotating about the Y axis, not the Z.

[Leon82]

+1 to a test part.

Even with our ez5 we still fine tune with the test part

[jlw™]

Nothing is perfect, honestly I've seen float of 0.002in - ish on our bigger machines... and I'm happy with that.

How much are you seeing?

[Carle387]

So I ran my test yesterday and as I suspected the end mill was off location.  I should have measured the error but didn't.  To my eye it was .030 or better.  Ran this up the flag pole and I met with some resistance but eventually I made them listen.  They had me check the table location in the X by measuring both sides of the table.  If this has any accuracy then I was only off about .0015 from center.  The other possibility is that the Z is off but still trying to figure how to measure this.

[Leon82]

Indicate the bore in that able and set relative to zero. Then go to 90 degrees and Indicate the face of the table.

This should roughly match the table half offset in the 19700 parameter area. 19703 or 4 I think

[Carle387]

Ah, therein is one of my challenges.  The table is 48" and has been covered with a home made sub-pallet.  No prior thought was put into having to verify the center of table position so I have no bore to indicate.  One of the other challenges, which is one of my greatest gripes with this machines capabilities is that I only have 18" of reach into the pallet when the spindle is vertical and my Y travel limits me to 2" above the pallet in a horizontal configuration which is the native mode.  This  makes any operation into the center on the pallet quite challenging to say the least.

[Leon82]

You can mount a sphere and Indicate 180 apart for x and y. Or triangulate if you want some more math

[Carle387]

We don't have one in our dept. but I think I seen our QC dept use one to calibrate our CMM.  I'll have to track this down.  Any web site that has a walk through on how to do this?

[dstryr]

Get an endmill and a block of material

Run G68.2 Cycle to A0C0

Position the tool in the +Y Axis

Side cut the block moving in X

Jump up and position back to the start X position

 

Use G68.2 to rotate the part 90* around Z. (A0 C90)

Repeat cut in X

Repeat this process until your block is cut

 

Go back to A0C0 and pick up center line using X

Then G68.2 the machine to A-90C0 and pick up the Z height of the block.

 

This should help you test your machine and find your problems.

 

[Carle387]

So still working with this issue.  I did get them to listen to me and we went as far as calling the Manufacture to come in re-level and adjust the rotational axis.  After they got the estimate the howling and screaming started about how unreasonable the price is and we that we can't fix the  machine.   I told them why invest $xxx,xxx.xx  in a machine and then not maintain it.  Anyone use any software solutions for calibrating a 5 axis?

[jlw™]

As bad as I hate to throw this out there, I have had to do it.  You can set an offset for every rotation and sneak up on it.  I used an Excel spreadsheet to trig out the deviations and then plugged the data in a file I had a ton of G10s in.  It got me close but if there was anything tight or critical I always snuck up on it.

Let them see the cost of that for a few months vs just having the machine dialed in.  You can likely get the procedure from the manufacturer to find center yourself.  If not, get them in, watch and take notes.  Then you can do it.

[civiceg]

Quote

 I told them why invest $xxx,xxx.xx  in a machine and then not maintain it.  Anyone use any software solutions for calibrating a 5 axis?

Renishaw AxiSet. It works really well but it's not exactly cheap.

http://www.renishaw.com/en/axiset-check-up--11353

[Carle387]

On ‎10‎/‎8‎/‎2018 at 12:45 PM, jlw™ said:

  You can set an offset for every rotation and sneak up on it.  I used an Excel spreadsheet to trig out the deviations and then plugged the data in a file I had a ton of G10s in.  It got me close but if there was anything tight or critical I always snuck up on it.

 

This too is currently what I am forced to do.  I create a work offset for every plane and then manually figure out what the deviation is.  I don't think they care that it takes a lot of work to not only proof a new tool path but also to dimple or just buzz a .005 profile cut to see where you are and what changes in your offset need to be. 

Oh, so anyone following this we are still sitting on the two bids I have a trying to decide what to do.  I did offer up the renishaw option but my supervisor didn't think it would make corrections to the rotational axis. 

[jlw™]

Renishaw does have a package that will tweak for COR deviation.

There is no substitution for mechanical accuracy though.

[Carle387]

So after 6 months of kicking and screaming and everyone telling me I didn't know what I was talking about it finally took my lead programmer actually having to deal with the error for someone to believe me.  They brought a proven program over from a sister machine and not to my surprise the part didn't come out.  Since they want to be able to use my machine as a back up should something go wrong on the other they realized that with this error that would not work.  The manufacture came out and found the X was off almost .070 and the Z was off too, I forget the amount but it was significant too.   So now I have a machine that works again although now I have to go through all my programs and reset my work offset values.  It is worth the work knowing I can count on an accurate machine again.

[Metallic]

6 hours ago, Carle387 said:

So after 6 months of kicking and screaming and everyone telling me I didn't know what I was talking about it finally took my lead programmer actually having to deal with the error for someone to believe me.  They brought a proven program over from a sister machine and not to my surprise the part didn't come out.  Since they want to be able to use my machine as a back up should something go wrong on the other they realized that with this error that would not work.  The manufacture came out and found the X was off almost .070 and the Z was off too, I forget the amount but it was significant too.   So now I have a machine that works again although now I have to go through all my programs and reset my work offset values.  It is worth the work knowing I can count on an accurate machine again.

Did you get the centerlines fixed i am assuming?

[?Mark]

I had a similar situation with a different brand (starts with O, head/table)). Took them forever to tweak it in and it would never really hold it well.

With DMGMORI we have zero issues...the 3d quickset takes care of it for checking and tweaking

[gcode]

We have a JOBs gantry mill with three different heads

a 3X head, a right angle head and a high torque 5X head.

Obviously, only the RA and 5X head require G68.2

It has a Fanuc 31i control and all this is handled by the control.

It took them a while to get it set up properly.

The issue was that each head had it's own parameters and the machine need to know the geometry of the heads

Once their lengths and pivot distances were sent properly in the control this works really well.

You can run the same tool with the same Tool Length Offset through all three heads without

have to make adjustments

[Carle387]

On ‎2‎/‎19‎/‎2019 at 1:59 PM, Metallic said:

Did you get the centerlines fixed i am assuming?

Yes, the centerline for the X and the Z distance are now both adjusted.  Ran a quick test and my location were spot on.  Everything is now copasetic in the world again.