G68 for 3D coordinate conversion

[Doug Funny]

Good Morning/Evening Gurus,

I was flipping through the Fanuc 16/18/16i/18i programming manual and came across a section about using G68 for 3D coordinate conversion.  Anyone familiar with using G68 in this fashion? If you have programming examples you could share that would be great. We only have 4th axis' but, I think this could really simplify setups if we could use 1 coordinate system instead of multiple systems on a single part. I have a little experience (very little) with G68.2. The example in the book seems to assume the program origin is always at the center of rotation. Is does not mention any parameters to store center of rotation. I would imagine I need to use a work offset to establish COR then, use macros to calculate where the current work offset is in relation to the COR?

 

TIA,

Doug

[Tim Johnson]

6 hours ago, Doug Funny said:

Good Morning/Evening Gurus,

I was flipping through the Fanuc 16/18/16i/18i programming manual and came across a section about using G68 for 3D coordinate conversion.  Anyone familiar with using G68 in this fashion? If you have programming examples you could share that would be great. We only have 4th axis' but, I think this could really simplify setups if we could use 1 coordinate system instead of multiple systems on a single part. I have a little experience (very little) with G68.2. The example in the book seems to assume the program origin is always at the center of rotation. Is does not mention any parameters to store center of rotation. I would imagine I need to use a work offset to establish COR then, use macros to calculate where the current work offset is in relation to the COR?

 

TIA,

Doug

I don't know anything about the 3D coordinate conversion but once you find the COR you can set a variable for future use. We use #921 to hold our COR. Each machine is different but they all use #921 so the programs can be shared with the other same machines.

On a different subject , how did you get in to post your thread?

[Doug Funny]

1 hour ago, Tim Johnson said:

 

On a different subject , how did you get in to post your thread?

At the very top of the page where you can logout of your account, there's a pulldown menu that says "create".  Click it and select topic the select which forum you want to post in. Also, just under the title block of this thread there's a button to start a new topic

 

[cncappsjames]

G68 has nothing to do with Center Of Rotation per se and G68.2 allow you the ability to track and program nowhere near Center of Rotation. 

In G68, the X, Y, and Z on the function call are the point about which you are rotating your coordinates. The R is the rotation angle.

In G68.2 the X, Y, and Z are the relationship to the part origin the following program section beforenitnis canceled. The I, J, and K are Euler angles (if no P is specified) and they the rotations around  Original Orientation Z, Original Orientation X, new Orientation Z to calculate the new orientations. If there is a P (can't recall the number off hand) then you can specify the order of rotation Q123 would be rotation around X, Y, and Z. Q321 would be Z, Y,and X. etc...

 

G68.2 relies on parameters to define the machine kinematics. Combine that with a work offset and the control calculates every position in every orientation and rotation. 

 

HTH

[Tim Johnson]

15 hours ago, Doug Funny said:

At the very top of the page where you can logout of your account, there's a pulldown menu that says "create".  Click it and select topic the select which forum you want to post in. Also, just under the title block of this thread there's a button to start a new topic

 

Thanks. Emastercam is back to normal but I'll save your info for the next meltdown.

[Doug Funny]

10 hours ago, cncappsjames said:

G68 has nothing to do with Center Of Rotation per se and G68.2 allow you the ability to track and program nowhere near Center of Rotation. 

In G68, the X, Y, and Z on the function call are the point about which you are rotating your coordinates. The R is the rotation angle.

In G68.2 the X, Y, and Z are the relationship to the part origin the following program section beforenitnis canceled. The I, J, and K are Euler angles (if no P is specified) and they the rotations around  Original Orientation Z, Original Orientation X, new Orientation Z to calculate the new orientations. If there is a P (can't recall the number off hand) then you can specify the order of rotation Q123 would be rotation around X, Y, and Z. Q321 would be Z, Y,and X. etc...

 

G68.2 relies on parameters to define the machine kinematics. Combine that with a work offset and the control calculates every position in every orientation and rotation. 

 

HTH

Hi James, 

See the attached PDF. I copied it out of my manual to send to the applications engineers at the machine dealers. They sent info on G68.2 because they thought I was talking that code as well. This code seems to work in a similar fashion but, not exactly. I forgot to bring the manual home with me and I'm not back to the office until Wednesday. When I get back, I can scan the rest of the pages of this section. This seems like it may be a precursor to G68.2. The machine this manual is for is from early the 2k's. I believe you have to specify where COR is relative to current work coordinate, direction the tilt will be going in and the angle of tilt. You can only translate in one plane at a time (I think) if doing 3+2. We would only be doing 3+1 at this time since we don't have a 5-axis machine yet. The machine in question should be open next week or so, I hope to be able to experiment a little. I'm hoping someone has some knowledge on exactly how this code functions.

 

Thanks,

Doug

doc00574420221014123952.pdf

[Doug Funny]

FYI, the G68 code does work. It DOES NOT work like G68.2 however.  This would be a useful code if you had an angled milling head like in the picture. If you rotate the plane along the X axis and made a Y axis move, the machine would move both Y and Z.  X axis moves would move normally. We don't have any of these type of heads so, this code will not work how I'd like it to...

Hopefully this helps someone...

 

Doug

 

 

 

 

[BBprecise]

G68 is usually a paid option for Fanuc controls and requires the center of rotation be set up in certain parameters. If you "bump" the machine you have to verify the COR hasn't changed and change it if it has. Our Mazak 5x mills have a program that I use combined with an Excel sheet to tell me which parameters to change and to what as it's based on the previous values. Works slick.

Since none of our machines came with G68 option, I created a macro that can mimick G68. You just need to set the COR (X&Z on a horizontal mill) in a fixture offset you typically don't use and my macro can calculate the new X,Y,Z origin of any B rotation at store it in any fixture offset you want. I currently have it set up so it increments the work offset by 1 for every rotation and each rotation is programmed with it's own fixture offset.

[BBprecise]

17 minutes ago, BBprecise said:

G68 is usually a paid option for Fanuc controls and requires the center of rotation be set up in certain parameters. If you "bump" the machine you have to verify the COR hasn't changed and change it if it has. Our Mazak 5x mills have a program that I use combined with an Excel sheet to tell me which parameters to change and to what as it's based on the previous values. Works slick.

Since none of our machines came with G68 option, I created a macro that can mimick G68. You just need to set the COR (X&Z on a horizontal mill) in a fixture offset you typically don't use and my macro can calculate the new X,Y,Z origin of any B rotation at store it in any fixture offset you want. I currently have it set up so it increments the work offset by 1 for every rotation and each rotation is programmed with it's own fixture offset.

I will add that it is absolutely crucial that your COR and your primary work offset has to be as good as possible. As if either is off everything after that is off. So typically it's best if you cut a feature at "B0" then measure it and adjust until you get it right.

We don't program off machine COR and no need to. We pick a feature on the part to set our origin and program off that point at every rotation. Before we used my macro, the operators had to set the individual work offsets, so usually what we would do is pick a feature at each rotation that the operators could tram or edgefind and program from that point. If there was nothing the operators would put a hole for a tooling ball in the fixture and tell me where it is in relation to the programs primary work offset,  then I would tell them how much to move each axis to get to the program origin for a particular rotation.

[Doug Funny]

7 hours ago, BBprecise said:

G68 is usually a paid option for Fanuc controls and requires the center of rotation be set up in certain parameters. If you "bump" the machine you have to verify the COR hasn't changed and change it if it has. Our Mazak 5x mills have a program that I use combined with an Excel sheet to tell me which parameters to change and to what as it's based on the previous values. Works slick.

Since none of our machines came with G68 option, I created a macro that can mimick G68. You just need to set the COR (X&Z on a horizontal mill) in a fixture offset you typically don't use and my macro can calculate the new X,Y,Z origin of any B rotation at store it in any fixture offset you want. I currently have it set up so it increments the work offset by 1 for every rotation and each rotation is programmed with it's own fixture offset.

Thanks, you've inspired me to write a macro to handle this. I've been thinking about it all day and have a few thoughts in my head...

[cncappsjames]

10 hours ago, BBprecise said:

G68 is usually a paid option for Fanuc controls and requires the center of rotation be set up in certain parameters.

That is G68.2 not G68 (on a FANUC) Two completely different options and functions. 

G68 is coordinate rotation/3D Coordinate Conversion. G68.2 is Tilted Work Plane. G68 does not require the configuration of machine kinematic parameters. G68.2 does require the kinematic parameters (#19700-#19705 for table/table machines).

[BBprecise]

9 hours ago, cncappsjames said:

That is G68.2 not G68 (on a FANUC) Two completely different options and functions. 

G68 is coordinate rotation/3D Coordinate Conversion. G68.2 is Tilted Work Plane. G68 does not require the configuration of machine kinematic parameters. G68.2 does require the kinematic parameters (#19700-#19705 for table/table machines).

Now you have me wondering James, I'll have to go back and try it again, but I'm pretty sure I was getting an invalid G code when I tried it. Granted it was a couple years ago.

We use G68.2 on our 5x Mazaks exclusively and as long as you keep the machine calibrated it's the best thing since sliced bread.

[cncappsjames]

Indeed. 

Honestly, I'd never own a 4-Axis OR 5-Axis without G68.2

It is WAY too powerful a function to not have. 

[CEMENTHEAD]

On 10/20/2022 at 11:20 AM, Doug Funny said:

We own a few of these. collecting dust since 2002. 5 axis killed the need.

[PAnderson]

Question to you guys. especially James. I have a clear understanding of G68.2 and G68. We have someone that is purchasing a large bridge mill but is cheap and won't purchase an integrated 4th and 5th. Instead, they will purchase a manual 4th and 5th, rotated by hand.

My question is, will either of these options work in this scenario?

[cncappsjames]

Theoretically G68.2 should work as long as the parameters are set correctly for the type of machine.

[PAnderson]

On 1/22/2023 at 12:30 AM, cncappsjames said:

Theoretically G68.2 should work as long as the parameters are set correctly for the type of machine.

Thanks James. Remember, this is a manually rotated head. How would you even find the numbers to populate 19700-19705? Can't run any kind of kinematics checking program. This would be a head/head machine but not really. The control is oblivious to this head.

They are dead set on using G68 anyhow.

[Leon82]

I would think it would be fine as long as they remember to rotate it. It's still a mechanical number

It would have to omit the rotary moves to prevent an alarm for non existent axia

[cncappsjames]

Bridge mill..... set it up in the parameters as a head/head type machine. Pplus set #19696.5 (WKP) as 1 for "workpiece coordinate system" instead of the normally 0 for a table/table. You may need to get some help from FANUC as there may be some other parameters involved in.

I really lack recent parameter setup experience on head/head machines. Been a while. Too long.