Jump to content

Welcome to eMastercam.com
Register now to gain access to all of our features. Once registered and logged in, you will be able to create topics, post replies to existing threads, give reputation to your fellow members, get your own private messenger, post status updates, manage your profile and so much more. This message will be removed once you have signed in.
Login to Account Create an Account
Photo

G68.2 *basic* explanation

- - - - -

  • Please log in to reply
46 replies to this topic

#1
newbeeee

newbeeee

    old but NOT grown up

  • Members
  • PipPipPip
  • 1,705 posts
  • Location:Where the Ind Revolution began
Hi all,

A friend of mine is working on a MAM72.
It has G68.2 and he can't get his head around how it works.
Can someone please explain in laymans basic terms how this works?
Many thanks as always.

#2
Guest_SAIPEM_*

Guest_SAIPEM_*
  • Guests
Fanuc 68.2 allows a user to define a WorkPlane by an X,Y,Z Coordinate Origin and the angular rotation about X,Y,Z axis centerlines(I,J,K Addresses)

The benefit of this for machines with a nutating head is that you can use all the canned cycles while the head is tilted.
You can also generate 2-1/2D toolpaths with arcs without having them linearized because of the plane orientation.

G68.2 performs the sames funtionality as the Fanuc 3-D Coordinate Conversion using G68 but simplifies it to a single line of code.
G68 3-D Coordinate Conversion required 2 lines of code to activate.

#3
marting

marting

    Advanced Member

  • Members
  • PipPipPip
  • 706 posts
  • Location:Trois-Rivières, Québec, Canada
OK, here it goes,

G68.2 X... Y... Z... I... J... K... R...

X, Y and Z define the center of rotation and will also be the work coordinate system origin.

I, J, K: Value is always 1 or 0. Only one address can be defined as 1 and the other 2 need to be 0. I1 means rotation around X. J1 means rotation around Y. K1 means rotation around Z.

R is the rotation angle. positive = CCW and negative = CW.

Hope this helps,

#4
newbeeee

newbeeee

    old but NOT grown up

  • Members
  • PipPipPip
  • 1,705 posts
  • Location:Where the Ind Revolution began
Thanks all,
I'll pass it on.
Cheers

#5
Joe788

Joe788

    Advanced Member

  • Members
  • PipPipPip
  • 3,482 posts
  • Location:California
Just curious, is there any real particular reason he wants/needs to use G68.2 on a trunnion machine?

#6
Guest_CNC Apps Guy 1_*

Guest_CNC Apps Guy 1_*
  • Guests
^^^

Maybe he's writing a program by hand (INSANE IMHO).

Just sayin... :D

Also, the function is called Tilted Working Plane.

I always thought I, J, K were the angles of pitch, roll, and yaw (or rotation around X, Y and Z respectively - See B-63944EN_03 pg 874,)

I didn;t know that right off the top of my head, but I was working with it this morning. :D

It's pretty involved to use it correctly. The pictures in the FANUC manual for a change actually are pretty decent and do help in understanding it... at least for me. Maybe my Jinglish is getting better.

#7
JMC

JMC

    Advanced Member

  • Members
  • PipPipPip
  • 935 posts
  • Location:All of North America
Basic explanation of TWP....wow. A couple of years ago I took an "advanced" class at Methods where they went through the theory of using G68.2 (Fanuc) and Cycle800 (Siemens)...they both work in a similar manner tho with the Siemens control you have about 5 different ways of using it....ugly words like Euler angles come to mind. A while ago I came across this site... http://bleiercnctrai...-machining.html . It is for the Siemens control but pretty much the same things apply for the Fanuc's.

Cycle800 does the transformation that calculates the orientation angles and actually commands the orientation axes to these angular positions. It also translates, rotates and translates again (if required) the G17 system so that when it is done the machine and control are ready to read-in and process G-code blocks that are identical to blocks for simple vertical bed mills.



#8
Colin Gilchrist - Eapprentice

Colin Gilchrist - Eapprentice

    Advanced Member

  • Members
  • PipPipPip
  • 4,562 posts
  • Location:Tolland, CT

OK, here it goes,

G68.2 X... Y... Z... I... J... K... R...

X, Y and Z define the center of rotation and will also be the work coordinate system origin.

I, J, K: Value is always 1 or 0. Only one address can be defined as 1 and the other 2 need to be 0. I1 means rotation around X. J1 means rotation around Y. K1 means rotation around Z.

R is the rotation angle. positive = CCW and negative = CW.

Hope this helps,


Martin,

This may be your particular Machine's implementation of G68.2, but many Fanuc controls will allow 3-dimensional rotation.

On these controls you will get a G68.2 X Y Z I J K (with no "R"). The I J K values will use Euler Angles for describing the Rotation about X,Y, and Z.

In these cases, I, J, and K will hold a rotation value from 0-90 degrees.

Most controls use G53.1 in conjunction with the G68.2 command. The G53.1 controls the Tool Axis direction (Z+ or Z- direction).

Wikipedia does a great job of explaining Euler's angles:
http://en.wikipedia....ki/Euler_angles

#9
Joe788

Joe788

    Advanced Member

  • Members
  • PipPipPip
  • 3,482 posts
  • Location:California

Wikipedia does a great job of explaining Euler's angles:
http://en.wikipedia....ki/Euler_angles


Good link Colin.

Posted Image

#10
Colin Gilchrist - Eapprentice

Colin Gilchrist - Eapprentice

    Advanced Member

  • Members
  • PipPipPip
  • 4,562 posts
  • Location:Tolland, CT
Thanks Joe.

I get that way when I start reading the Geometric derivation section. My eyes start to roll back in my head...


In that section they talk about how to derive the Euler angles by using Matrix calculus.

#11
newbeeee

newbeeee

    old but NOT grown up

  • Members
  • PipPipPip
  • 1,705 posts
  • Location:Where the Ind Revolution began
Haha Joe!

Joe/James: - I *think* the G68.2 is what is spat out by the delcam post and he wanted to get his head around what it was doing.
Notice the word *think* here....:unsure:

#12
MotorCityMinion

MotorCityMinion

    Advanced Member

  • eMC Learning Group
  • PipPipPip
  • 1,270 posts
Had to save that pic.

#13
Mick

Mick

    Poison Ivy

  • Members
  • PipPipPip
  • 1,791 posts
  • Location:Kicked in the corner
Out of curiosity, what is the difference between G68.1 and G68.2? We use G68.1 on our Mori Seiki MT's, and it is for the same reason, a tilted working plane. We cut keyways in tapered shafts, and it is a much cleaner method of programming. Ironically, most of our operators hate it, but I think that is because they dont understand it :)

#14
Colin Gilchrist - Eapprentice

Colin Gilchrist - Eapprentice

    Advanced Member

  • Members
  • PipPipPip
  • 4,562 posts
  • Location:Tolland, CT
I'll check my Fanuc manual later on the G68.1, but I remember that G68 with no decimal is Pinch Turning on a Lathe (at least according to my manual).

The whole point of using the transformed work plane command is that you can create a 'reference plane' that is rotated in 3D space, and program using standard 3 axis code. It is typically used to simplify 3+2 machining. Your controller will take the 3 axis code ( a pocket or canned tap cycle for example) and do the 5 axis motion calculations inside the control.

As others have mentioned, the Siemens CYCLE 800 is another example of using transformed work planes.

#15
Mic

Mic

    Member

  • Members
  • PipPip
  • 282 posts
  • Location:Denmark
Well I've worked with both MAM72 and the new MX-520.

XYZ of the G68.2 line is new origin and centre of the rotation.

IJK is Euler rotation angles. I rotates around the untransformed Z axis, value can be +/- 180 ( or 0-359.999 depending on machine ) J is then rotation around the new X axis, here the value can be from 0 and up to endstop of A( B ) axis. Finally K is rotation around the new Z axis to allow the user to position the X axis in the wanted direction.

Always use G53.1 after the G68.2 line.

You'll also need to apply G43 after G53.1 and cancel it again ( G49 ) before G69

As already mentioned Siemens CYCLE800 can do exactly the same. And so will Heidenhain CYCL DEF 7 + CYCL DEF19 ( PLANE )

#16
Joe788

Joe788

    Advanced Member

  • Members
  • PipPipPip
  • 3,482 posts
  • Location:California

Well I've worked with both MAM72 and the new MX-520.

XYZ of the G68.2 line is new origin and centre of the rotation.

IJK is Euler rotation angles. I rotates around the untransformed Z axis, value can be +/- 180 ( or 0-359.999 depending on machine ) J is then rotation around the new X axis, here the value can be from 0 and up to endstop of A( B ) axis. Finally K is rotation around the new Z axis to allow the user to position the X axis in the wanted direction.

Always use G53.1 after the G68.2 line.

You'll also need to apply G43 after G53.1 and cancel it again ( G49 ) before G69

As already mentioned Siemens CYCLE800 can do exactly the same. And so will Heidenhain CYCL DEF 7 + CYCL DEF19 ( PLANE )


Mic, is there any particular reason you're using G68.2? I know why people use it on nutating head machines, but I haven't come across a need to use it on a trunnion machine. Are you using a right angle?

#17
Dave.L

Dave.L

    Advanced Member

  • Members
  • PipPipPip
  • 1,974 posts
Joe, did you rob that pic from Evil? Or are you his protégé ? :P

#18
Joe788

Joe788

    Advanced Member

  • Members
  • PipPipPip
  • 3,482 posts
  • Location:California

Joe, did you rob that pic from Evil? Or are you his protégé ? :P


I robbed it randomly off of the web, and spliced in the Euler's angles part. If you do a google image search for "at first I was like", you'll find lots of hilarious stuff!

#19
Mic

Mic

    Member

  • Members
  • PipPip
  • 282 posts
  • Location:Denmark

Mic, is there any particular reason you're using G68.2? I know why people use it on nutating head machines, but I haven't come across a need to use it on a trunnion machine. Are you using a right angle?


Yes there is. To be able to use the same program with different datum locations you either need to use G54.2(DFO) or G68.2(TWP). Dynamic Fixture Offset has one limitation. All machines I've seen has a small offset between A( B ) axis and C axis centre line measured in the XY plane, normally below 20 micron's. This small offset isn't compensated by G54.2 while G68.2 also takes care about this.

Maybe it's possible to compensate this in the postprocessor, but I've found it easier to use G68.2 because this works with most cam systems and posts.

#20
Joe788

Joe788

    Advanced Member

  • Members
  • PipPipPip
  • 3,482 posts
  • Location:California

Yes there is. To be able to use the same program with different datum locations you either need to use G54.2(DFO) or G68.2(TWP). Dynamic Fixture Offset has one limitation. All machines I've seen has a small offset between A( B ) axis and C axis centre line measured in the XY plane, normally below 20 micron's. This small offset isn't compensated by G54.2 while G68.2 also takes care about this.

Maybe it's possible to compensate this in the postprocessor, but I've found it easier to use G68.2 because this works with most cam systems and posts.


Ahhhh I see. I've only used G54.2 on a Matrix control, and it comps for the tiny mismatch between A and C. I didn't realize there were machines that didn't. Good knowledge!