G43.4 (TCP) on a OKK VP9000 5AX w ith Fanuc 310is-A5?

[Steve Landkamer]

Good Morning after a sleepless night trying to figure this one out.

 

I am dealing with an OKK VP9000 5-axis (trunion A&C) with a Fanuc 310is control using G43.4 (TCP).

 

In my output code below the first two sides cut fine and the machine moves where it should.

 

When it goes to Side 3 (C0. A-4. the table rotates correctly) the machine moves from Y- to Y+ even though the code is X- to X+!!!!

When it goes to Side 4 (A-6. no C needed) the machine moves from Y+ to Y- and the code again is X+ to X-!

 

My customer is telling me that the "G43.4" is causing this to happen which in this case it is cutting the same sides of the part.......

He does not want to turn off the G43.4 for the obvious reason but dang this is strange.

 

In the past I have not encountered this with G43.4 TCP in a post and having issues with the code at the machine.

 

Am I missing something here is there something set wrong in the machine?

Any ideas or suggestions are appreciated.

 

Thanks,

Steve

 

%
O3535
(MILLPOSTTEST)
(DATE - 10-11.-13.)
(MCX FILE - OKK_VP9)
(NC FILE - MILLPOSTTEST.NC)
(MATERIAL - STEEL INCH - 1010 - 200 BHN)
(T245| 2 INCH FLAT ENDMILL|H245|D245| DIA. - 2.|WEAR COMP)
G49 G17 G80 G90 G94 G40
G0 G28 G91 Z0.0
G0 G28 X0.0 Y0.0 A0.0 C0.0
( 2 INCH FLAT ENDMILL|TOOL - 245|DIA. OFF. - 245|LEN. - 245| DIA. - 2.)
(SIDE 1)
N245 T245
M06
M79
M11
S267 M3
G0 G90 G54 X10. Y8.9619 C90. A-5.
G5 P10000 R1
G43.4 H245 Z4.8716
Z.9716
G1 Z.8716 F6.42
X9.8758
X-2.4224
X-10.
G0 Z.9716
Z4.8716
(SIDE 2)
Z5.2187
Y-8.9255
A7.
Z1.3187
G1 Z1.2187
X-9.8758
X2.4224
X10.
G0 Z1.3187
Z5.2187
(SIDE 3)
C0. A-4.
X-10. Y10.9756
Z4.6976
Z.7976
G1 Z.6976
X-9.8758
X2.4224
X10.
G0 Z.7976
Z4.6976
(SIDE 4)
A-6.
Y-8.9452
Z2.9547
Z-.9453
G1 Z-1.0453
X9.8758
X-2.4224
X-10.
G0 Z-.9453
Z2.9547
G49
G5 P0
M5
G0 G28 G91 Z0.0
G0 G28 X0.0 Y0.0 A0.0 C0.0
G90
M30
%

[Chris McIntosh]

When using G43.4 with a trunnion table typically you would output all your coordinates unrotated, the machines internal kinematics will work out the motion. With a C90 for the first two operations and a C0 for the second two and all motion in tool paths being along the X-axis, I would expect that motion in one of the tool paths to be incorrrect, which you have identified as the second two operations.

 

So, without seeing exactly what you're cutting it looks like the calculated coordinates for your second two operations are incorrect and need to be changed in the post.

 

Chris

[Guest MTB Technical Services]

When using TCP it's important to remember that the X,Y,Z coordinates in the NC Code are table coordinates.

That is, they are actually the CL coordinates BEFORE rotation.

 

A & C will be the actual rotary angles calculated from the tool vector.

With TCP, it's the angles that are critical.

TCP will use the rotary angles to correctly position X,Y,Z on the machine based on the X,Y,Z Table (CL) coordinates.

 

Backplot the toolpaths and save the toolpaths as geometry.

Then you can query the end points to verify the X,Y,Z position relative to the global WCS.

If the positions don't match the output code in the post, you'll need to modify the post to get the original CL positions.

 

http://www.emastercam.com/board/index.php?showtopic=73020entry853339

[Steve Landkamer]

Thanks for the feed back!

Trying what has been suggested but I have uploaded a Z2G that has the MCX-7 and associated files along with a video of how the machine was moving on the code posted above.

5-AXIS_MILL_POST_TEST.Z2G

[MSL]

Thanks for the feed back!

Trying what has been suggested but I have uploaded a Z2G that has the MCX-7 and associated files along with a video of how the machine was moving on the code posted above.

 

Hi Steve,

How do you like your machine? any problems? We were looking at OKK VC-X350 last week. We are looking to buy a 5Axis machine and I'm doing some research.

 

Thanks.

[Steve Landkamer]

As a follow up on this machine, yes I should have done this earlier......but here we go.

The following is the important parts that needed to be set in the post and THE MACHINE for crying out loud.

 

#######
#	    IMPORTANT NOTE!!!!!!!!
# Parameter settings for a Fanuc 30i series controller.
# These settings must be set in the control for G43.4 (TCP) to work.
#				 Bits: (76543210)
# Parameter 19696 Bit 5 (xx0xxxxx) set to 0
# Parameter 19754 Bit 5 (xx1xxxxx) set to 1
#

mtype	    : 2
#Primary axis angle description (in machine base terms)
#With nutating (mtype 3-5) the nutating axis must be the XY plane
rotaxis1$ = vecy  #Zero    ##rotaxis1$ = vecy  #Zero  
rotdir1$  = -vecx #Direction  ##rotdir1$  = -vecx 
#Secondary axis angle description (in machine base terms)
#With nutating (mtype 3-5) the nutating axis and this plane normal
#are aligned to calculate the secondary angle
rotaxis2$ = vecz  #Zero    ##rotaxis2$ = vecz	 
rotdir2$  = -vecy  #Direction  ##rotdir2$  = vecy