5 axis milling, control does not include my pivot point distance

[kpq]

Dear experts
I have an issue with my pivot point distance when running 5 axis programming,
My pivot point is 83.17mm if I turn my 4th and 5th axis 180 degree (head head config) to mill with the side of my router the control does not include my pivot point distance of 83mm the coordinates from the program are correct but my tool center is off by 83mm in this case Y and Z axis 83mm exactly, is there a MD parameter or file that needs to be adjusted? Or is there a siemens code that needs to be given before it reads my pivot point?
when I run only G17 3 axis code all is good, but when I start to make 5 axis movement tool center is not where it should be.
Hope you can assist me with my issue

sinumerik 840D NCU 573.4 MMC103 With SW4.4

the g code is from my current issue, where it missing 83mm in z and y axis. maybe I'm missing a code,

N3050 ;Start of Path
N3060 ;
N3070 ;TECHNOLOGY: METHOD
N3080 ;TOOL NAME : MILL
N3090 ;TOOL TYPE : Milling Tool-5 Parameters
N3100 ;TOOL DIAMETER : 80.000000
N3110 ;TOOL LENGTH : 85.000000
N3120 ;TOOL CORNER RADIUS: 0.000000
N3130 ;
N3140 ;Intol : 0.030000
N3150 ;Outtol : 0.030000
N3160 ;Stock : 0.000000
N3170 _camtolerance=.06
N3180 $MA_COMPRESS_POS_TOL[X] = _camtolerance*1.2
N3190 $MA_COMPRESS_POS_TOL[Y] = _camtolerance*1.2
N3200 $MA_COMPRESS_POS_TOL[Z] = _camtolerance*1.2
N3210 $MA_COMPRESS_POS_TOL[C] = _camtolerance*12
N3220 $MA_COMPRESS_POS_TOL[B] = _camtolerance*12
N3230 NEWCONF
N3240 ;
N3250 ;Operation : CONTOUR_PROFILE_2
N3260 ;
N3270 MSG("80MM SHAPE TOP")
N3280 ;First Move
N3290 FFWON
N3300 UPATH
N3310 SOFT
N3320
N3330 G642
N3340 TRAORI
N3350 G54
N3360 ORIWKS
N3370 G0 C-148.51871 B168.24409
N3380 G0 X553.08425 Y52.56516 Z66.32606 D1
N3390 ;Engage Move
N3400 G1 X479.43822 Y21.38753 Z68.37979 F3000
N3410 ;Cutting
N3420 X470.30421 Y17.5207 Z68.6345 C-149.24668 B168.40099
N3430 X461.13448 Y13.73944 Z68.89017 C-149.97664 B168.56069
N3440 X451.92983 Y10.04409 Z69.14676 C-150.70866 B168.72331
N3450 X442.69106 Y6.43497 Z69.40426 C-151.44283 B168.88894

any help would be grateful
if anyone needs more information from my part just ask and ill post it asap


Regards
Flemming renaldi

Similar Threads:

• CadCam tool setup for 4 axis- Z gauge lenght or with pivot length
• Help wanted: milling around 4th axis when workpiece is not centerd rotating point
• Mazak 5 axis mill with tool center point control g43.4
• How to change the pivot point when using custom WCS's?

[kpq]

my machine dealer told me the pivot point , let me past what he wrote me.

****The parameter for the pivot point is stored as a basic* in the tool corrections T1,T2 ...
Here the value should be changed ****

can anyone tell me where I should input that from my attached picture of my tool offset parameter page?

regards
flemming

[CNCFr]

I don't think it is a good idea to introduce machine constants into tool data.
There is a set of 3 vectors in the machine data which are used to describe the kinemtics of the machine.
These are
MD24500 $MC_TRAFO5_PART_OFFSET_1 ; vector from zero point to 1st rotational axis
MD24550 $MC_TRAFO5_JOINT_OFFSET_1 ; vector which gives the distance between both rotational axes
MD24560 $MC_TRAFO5_BASE_TOOL_1 ; vector from 2nd rotational axis to pivot point for tool length 0

The suffix _1 is for machine data used by the first TRAORI-transformation (which is relevant for your case as you wrote just TRAORI in your prgramme).
For a first try I would recommend to experiment with the 3rd component of $MC_TRAFO5_BASE_TOOL_1 i.e. with $MC_TRAFO5_BASE_TOOL_1[2].

[kpq]

problem solved.

fix was to change these 2 MD settings from 0.0 to my pivot distance that is 83.17mm

MD 24500[2] = 83.17 ( pivot point plus)
MD 24550[2]= - 83.17 ( pivot point minus)
hope it helps