G68.2 *basic* explanation

[Colin Gilchrist]

2 hours ago, So not a Guru said:

Colin, what are the pros & cons of G53.1 vs G53.6?

 

Tim Markoski made an excellent post on LinkedIn, describing the pros and cons of both modes.

The real important thing to understand is that both G53.1 and G53.6 will cause Rotary Motion on the Machine, unless the rotary axes have already been positioned by the NC code, prior to calling G68.2.

G53.6 enables RTCP during the rotation. (If not pre-positioned.) This means the tool tip will remain stationary, while the Machine pivots around the tool tip. This potentially causes XYZ motion while the rotation occurs.

G53.6 cannot be used with G54.4 (Work Setting Error Correction), while G53.1 can.

You can think of G53.1 as a "rotate now, if the tool spindle is not already aligned to the Z axis of the TWP" command.

There is some danger with using G53.1, if your machine is not "pre-positioned" as it will simply engage and move the rotaries, when called. Since RTCP is not active with G53.1, you could potentially get a collision if the tool is close to the part, fixture, or table.

https://www.linkedin.com/pulse/fanuc-g682-5-axis-tilted-work-planes-tim-markoski

 

[So not a Guru]

45 minutes ago, Colin Gilchrist said:

Tim Markoski made an excellent post on LinkedIn, describing the pros and cons of both modes.

 

 

That was the post that brought me to ask this.

Thanks for your clarification. You are, as always, much appreciated.

[CEMENTHEAD]

lol @ 36,000 views

[[email protected]]

Hi,

Does anyone have any idea how would G68.2 work on 3axis machine?

I would like to use my touch probe to measure the part, and than rotate the coordinate system arround some refference point. So i would "allign" the part with virtual coordinate system.  The rotation angles would be very small, under 1deg..

Im working on Mori Seiki NV with G68.2 enabled, when i enter the G68.2 it doesnt follow the logic.

For example:

G0 G90 G54

X0.Y0.Z0.

G68.2 X0.Y0.Z0.I45.J0.K0. 

G1 Z-100.(it should move the Z and Y axes both at the same time for same amount, but instead goes only with Z but nothing with Y axe)

But if i write:

G68.2 X0.Y0.Z0.I.J45.K0. 

G1 Z-100.(than it moves Z and Y axes both at the same time for same amount)

Any ideas?

[crazy^millman]

On 2/6/2019 at 11:42 AM, [email protected] said:

Hi,

Does anyone have any idea how would G68.2 work on 3axis machine?

I would like to use my touch probe to measure the part, and than rotate the coordinate system arround some refference point. So i would "allign" the part with virtual coordinate system.  The rotation angles would be very small, under 1deg..

Im working on Mori Seiki NV with G68.2 enabled, when i enter the G68.2 it doesnt follow the logic.

For example:

G0 G90 G54

X0.Y0.Z0.

G68.2 X0.Y0.Z0.I45.J0.K0. 

G1 Z-100.(it should move the Z and Y axes both at the same time for same amount, but instead goes only with Z but nothing with Y axe)

But if i write:

G68.2 X0.Y0.Z0.I.J45.K0. 

G1 Z-100.(than it moves Z and Y axes both at the same time for same amount)

Any ideas?

G68.2 is tilted work planes. Are you sure you don't want G68.1 Coordinate System Rotation start or 3-dimensional coordinate system conversation on? 

G68.2 is normally for 4 and 5 axis work not sure how it is going to work on 3 axis when it is looking normally to 19700 parameter so the Axis Centerlines to know where and how to apply the Titled Work Plane.

From the Fanuc Manual it even mentions this.

 

For G68.1 I get this:

 

 

 

Edited August 20, 2020 by crazy^millman
Pictures removed to save space

[jlw™]

As Ron stated G68.2 is TWP.  However, most 3 axis controls support plain old G68 or have a theta on the offsets page.  Some have probing routines for this included.  If not, it's simple trig to get the rotation.  I've seen others where it is done through the scaling function.  My condolences if you have an Anilam control.  What control is it?

[[email protected]]

Not shure if the machine supports G68.1. I know it supports G68, and G68.2 but never tried G68.1.

I tried searching online but cant find much on G68.1. Do you know how to program it?

I know G68 is rotation arround one axis, and i need to rotate it arround two axes. G68.1 is capable of rotating two axes at the time? 

I will test it on the machine tomorrow morning..

[crazy^millman]

41 minutes ago, [email protected] said:

Not shure if the machine supports G68.1. I know it supports G68, and G68.2 but never tried G68.1.

I tried searching online but cant find much on G68.1. Do you know how to program it?

I know G68 is rotation arround one axis, and i need to rotate it arround two axes. G68.1 is capable of rotating two axes at the time? 

I will test it on the machine tomorrow morning..

G68.2 is not something I have ever tested on a 3 Axis machine. G68.1 is an option and does about the same thing as G68 from what I got out of the Fanuc Programming manual. You might be able to get it to work on a 3 Axis machine, but you need to make sure you understand what the I,J and K are doing and how they are going to impact your set up. From a programming stand point it should be able to take the originally programmed code and just adjust what is needed on the control to machine what you need.

[Leon82]

the Renishaw manual I have macro 9818 sets g68 coordinate rotation for a 3 axis

[[email protected]]

I made a macro program for measuring and calculation angles. But the problem is in rotation. G68.2 doesnt work like i thought. 

I supose your case is arround one axe only, right? 

[jlw™]

If this is a 3 axis machine, why are you rotating?  I'm curious here.  Can you post a file or a picture of the machine?  I mean, I get wanting to G68 to a fixture or an odd part on the table but I'm not seeing why use G68.2 at all on a 3 axis machine.

[Leon82]

You would rotate on the z. Anything else doesn't make sense if you have flat tools

[[email protected]]

Im programing finish 3d operations. The part is allmost done, only operation left is 3D operation in the cavity. Part has two pieces, a male and female half. Operator on the machine needs to allign the part physical, so the two halfes are alligned when put together.. Now he has to do it manually with measuring devices and difference between halfes must be under  0.02mm. 

So, the idea is to use renishaw probe and measure the part, calculate all angles differences between machine axes. Then rotate coordinate system to allign parts arround Z and X axes. 

With something like that operator dont need to center the parts manually. 

I allready made the measuring and calculation macros, offcourse if the measuring error is too big he has to allign it better, but if its in some tolerance, coordinate system rotation should do the job.. 

[crazy^millman]

37 minutes ago, [email protected] said:

Im programing finish 3d operations. The part is allmost done, only operation left is 3D operation in the cavity. Part has two pieces, a male and female half. Operator on the machine needs to allign the part physical, so the two halfes are alligned when put together.. Now he has to do it manually with measuring devices and difference between halfes must be under  0.02mm. 

So, the idea is to use renishaw probe and measure the part, calculate all angles differences between machine axes. Then rotate coordinate system to allign parts arround Z and X axes. 

With something like that operator dont need to center the parts manually. 

I allready made the measuring and calculation macros, offcourse if the measuring error is too big he has to allign it better, but if its in some tolerance, coordinate system rotation should do the job.. 

G68 and call it a day. That is exactly what that is for. G68.2 is for Multiaxis machines not 3 Axis.

[jlw™]

and unless I'm mistaken G68.1 is G68.  In the case of G68 the .1 is default and the .2 or .3 or .4 have to be specified.