Okuma 5 axis program on a pyramid

[Brian B 74]

Has anyone run into trouble programming an Okuma M460-5ax with 2 parts on a pyramid?  Our CALL OO88 commands are coming up with some really crazy numbers.   I know for 1 part on the trunnion your WCS is set to top.  But what if your part is sitting at a 20 deg angle?  That's where I get a little lost.   I've created a plane on the top of my part and added values to the A and C rotary's to my WCS table in the osp to simulate a top plane but that made it even worse.

 Any help is greatly appreciated.

[crazy^millman]

On 11/29/2021 at 5:14 PM, Brian B 74 said:

Has anyone run into trouble programming an Okuma M460-5ax with 2 parts on a pyramid?  Our CALL OO88 commands are coming up with some really crazy numbers.   I know for 1 part on the trunnion your WCS is set to top.  But what if your part is sitting at a 20 deg angle?  That's where I get a little lost.   I've created a plane on the top of my part and added values to the A and C rotary's to my WCS table in the osp to simulate a top plane but that made it even worse.

 Any help is greatly appreciated.

The post should work out the solution from the center of your WCS to set the CALL OO88 values correctly. If not setup that way then you would need to make a WCS at each origin for each part with angles set in the work offsets in the machine and then the CALL OO88 will all be Zero. Where as if you have your WCS at the center and then your C and T Planes on the parts then the post should have that value in the CALL OO88 line. Now all your X,Y Z values will be Zero from the CALOO88 placement, but angle and such would still come from the original WCS. 

[Greg Williams]

I dont think CALL OO88 supports values in the A and C axis

[gcode]

7 hours ago, Greg Williams said:

I dont think CALL OO88 supports values in the A and C axis

That is correct

CALL 0088 works like Fanuc G68.2 

It positions the rotary axis, then outputs a 3axis toolpath 

[crazy^millman]

10 hours ago, Greg Williams said:

I dont think CALL OO88 supports values in the A and C axis

Not sure over there, but here is sample from a customer I did last year. I didn't put the plane at different places on the parts so that is why PX=0. PY=0. and PZ=0. This was on a Genos 460V 5 Axis an between CNC software, Hartwig, Okuma Think, and Postability to get the customer dialed in.

Gcode is correct it is DWO not TCP, but like a Fanuc you can use CALL OO88 to postilion the machine for full 5 axis toolpath just depends on how  the post configured to output the code is all.

 

(T5   - HELICAL - 81799 - END MILL FOR STEEL -  VARIABLE PITCH - 5 FLUTE X 0.5000 DIA X 0.6250 LOC X 0.0300 RADIUS X 2.7500 REA - H5   - D5   - D0.5000" - R0.0300")
G00 G17 G20 G40 G80 G90
G00 Z=VPPLZ
N1
(FINISH SIDE WALL OF FLUTE 2 BEFORE RAMP CUT)
(OPERATION NO - 76)
(OPERATION TYPE - CONTOUR)
G00 Z=VPPLZ
T5 M06 (HELICAL - 81799 - END MILL FOR STEEL -  VARIABLE PITCH - 5 FLUTE X 0.5000 DIA X 0.6250 LOC X 0.0300 RADIUS X 2.7500 REA)
G15 H10
M404
CALL OO88 PX=0. PY=0. PZ=0. PA=-44.5905 PC=4.2722 PH=10 PP=51
M11
M27
G00 G17 G90 A-44.5905 C4.2722 S2674 M03
M10
M26
G56 HA
X.16683 Y1.91403
Z3.
M08
M51
Z.66273
G94 G01 X-.09033 Y1.60765 F50.
G03 X-.11333 Y1.53469 Z.6627 I.07659 J-.06426
X-.08242 Y1.46254 I.12485 J.01088

(FINISH SIDE WALL OF FLUITE 5 BEFORE RAMP CUT)
(OPERATION NO - 82)
(OPERATION TYPE - CONTOUR)
CALL OO88 PX=0. PY=0. PZ=0. PA=-44.5905 PC=220.2722 PH=10 PP=51
M27
A-44.5905 C220.2722 S2674 M03
M26
X.16586 Y1.92515 Z3.
Z.66273
G01 X-.0913 Y1.61877
G03 X-.11435 Y1.54576 Z.6627 I.07659 J-.06426

Here is a CALL OO88 for positioning to do 5 Axis work.

(T4   - 1/4 BALL ENDMILL     - H4   - D4   - D0.2500" - R0.1250")
(T2   - 1/4 BALL ENDMILL     - H2   - D2   - D0.2500" - R0.1250")
G00 G17 G20 G40 G80 G90
G00 Z=VPPLZ
N1
(FINISH WALL SECTION TOOTH 1A)
(OPERATION NO - 52)
(OPERATION TYPE - SWARF 5AX)
G00 Z=VPPLZ
T4 M06 (1/4 BALL ENDMILL)
G15 H10
M404
CALL OO88 PX=0. PY=0. PZ=0. PA=-96.0845 PC=323.0572 PH=10 PP=51
G00 G17 G90 X.89187 Y3.22605 (TOP MAPPED)
G15 H10
M11
M27
A-96.0845 C323.0572 S5348 M03
G56 HA
M510
G00 G169 X2.11649 Y1.33059 Z-3.49328 A-96.0845 C323.0572 T2
Z-3.49328 A-96.0845 C323.0572
M08
M51
G94 G01 X2.01361 Y1.19377 Z-3.47504 F60.
X2.01296 Y1.19031 Z-3.47414
X2.01018 Y1.17293 Z-3.4721
X2.00848 Y1.15538 Z-3.47388
X2.00839 Y1.1385 Z-3.47926
X2.0103 Y1.12307 Z-3.48775
X2.01452 Y1.10978 Z-3.49869
X2.02086 Y1.09881 Z-3.51117
X2.01958 Y1.10268 Z-3.49839 A-93.3087 C323.7743
X2.01849 Y1.1068 Z-3.48563 A-90.5325 C324.4874
X2.01759 Y1.11118 Z-3.47287 A-87.7561 C325.1999
X2.01686 Y1.11581 Z-3.4601 A-84.9801 C325.915
X2.0163 Y1.1207 Z-3.4473 A-82.2049 C326.6363
X2.01592 Y1.12585 Z-3.43446 A-79.4309 C327.3673
X2.01589 Y1.12586 Z-3.43435 A-79.4323 C327.367
X2.01586 Y1.12587 Z-3.43424 A-79.4336 C327.3667
X2.01584 Y1.12588 Z-3.43413 A-79.435 C327.3664
X2.0158 Y1.12589 Z-3.43398 A-79.4368 C327.3661
X2.01577 Y1.12591 Z-3.43386 A-79.4383 C327.3658
X2.01574 Y1.12592 Z-3.43371 A-79.4401 C327.3654
X2.01569 Y1.12594 Z-3.43353 A-79.4424 C327.365
X2.01567 Y1.12595 Z-3.43342 A-79.4436 C327.3647
X2.01564 Y1.12596 Z-3.43331 A-79.445 C327.3644

Again if I had put planes at different places on the part like in the topic then I would expect to see different values in the CALL OO88 line for X - Y - Z, but since I programmed everything from one Zero point I got them all at Zero. The operations in Mastercam all shared the same TOP WCS and then had different T-C Plane,s but they all shared the same origin.

[gcode]

On 11/29/2021 at 5:14 PM, Brian B 74 said:

But what if your part is sitting at a 20 deg angle? 

your WCS should be TOP

then program your toolpaths using 20° tool and construction planes

[Greg Williams]

A and C need to be zero in the machine work offset page

[Chally72]

This is possible if you only have one rotation value in one rotary axis work offset field of the controller. IE, this would work for the zero degree C clocking position of the pyramid with a B (or A) of 20. As soon as you have a compound angle in the work offset, it will still run on machines like Haas and Doosan, but the resultant motion is no good. When doing multi-station pyramids, Gcode's solution of WCS being the top orientation, or along the spindle vector, has to be used- so you unfortunately can't use the work offset XYZ's to move your origin square to the orientation of the part to say, shift its pocket location.

[cncappsjames]

When using G68.2, you can have a value in your rotary axis fixture offset but not in your tilt axis offset... on a FANUC control anyway.

[Brian B 74]

Sorry for the late response.  We did get this worked out.  I had the A at -20 and C and 180 when I was probing the top of the part (setting workoffset H10).  Once I had this point set I ran the following command:

CALL OO88 PCA=-20 PCC=180 PH=10 PP=1

This calculated the point back to where it would be if the rotaries are at A0 and C0.  Once this was done everything fell into place.

Thanks for the help.  It was greatly appreciated.

[Greg Williams]

I think this error is fixed by using  G469/G467

 

G21
G00 G90 G17 G94 G40 G80
M05
G00 Z=VPPLZ
M01

( OPERATION 4 )
( EM-12-FINISH-FACE-PLANE-1 )
( EM-12X75X32_FINISHER | TOOL - 54 | DIA. OFF. - 54 | LEN. - 54 | TOOL DIA. - 12. )
T54 M06
S2000 M03
G00 G90 G17 G15 H1
G469 P1 X10. Y0. Z0. I90. J45. K0.
M11
M27
G00 A-45. C-90.
G467 P1
M10
M26
G56 HA
X15.531 Y52.091
Z50.