c axis jerk (lathe)

[ashok kumar]

Hii,

 

i am using Mastercam X8 lathe with c axis.  Machine name: Gildemeister ctx 800 (Sinumeric 840D ) machine

 

If we create a c axis face contour in Mastercam lathe and when we run that program in machine means. C axis will jerk as a result chattering mark has formed in the job. We have tried to fine-tune the machine but no use

 

N120 G71 G40 G18 G90

N122 G54

N124 T8

N126 TC(1)

N128 G17 M814

N130 G94

N132 L707

N134 SETMS(1)

N136 DIAMON

N138 G26 S4= 4000

N140 G0 C4=DC(129.806)

N142 G0 Z5

N144 G0 X78.102

N146 G97 S1=1909 M1=3

N148 X78.102 C4=DC(129.806)

N150 Z2 C4=DC(129.806)

N152 G1 Z-5 C4=DC(129.806) F190.9

N154 X75.879 C4=DC(127.746) F381.8

N156 X73.789 C4=DC(125.597)

N158 X71.835 C4=DC(123.358)

N160 X70.019 C4=DC(121.029)

N162 X68.346 C4=DC(118.612)

N164 X66.818 C4=DC(116.108)

N166 X65.438 C4=DC(113.522)

N168 X64.208 C4=DC(110.859)

N170 X63.132 C4=DC(108.123)

N172 X62.211 C4=DC(105.323)

N174 X61.449 C4=DC(102.466)

N176 X60.846 C4=DC(99.563)

N178 X60.403 C4=DC(96.624)

N180 X60.123 C4=DC(93.66)

N182 X60.004 C4=DC(90.683)

N184 X60.048 C4=DC(87.705)

 

 

 

Here c axis and x axis values are appeared with  certain tolerances

 

Is It possible to make the outputs with circular interpolation and linear interpolation  like 2d contour mill ( machine don’t have y axis  )

 

Please give the solution to solve this problem

[Watcher]

It´s likely it´s not a MC fault. It´s caused by the tuning of your axes.

 

Why are you using DC statements? These are shortest direction angular moves. Are you sure Mastercam and the control is properly aware and tuned to deal with it?

 

Where did you get the post from?

 

Two solutions for you: Call you dealer and/or call DMG.

[#Rekd™]

We have a DMG latte with a Siemens 840D control, the post is by In-House.

 

The c-axis paths work fine.

[JoshC]

There is a face interpolation mode you may need to turn on. If the post has been setup with this option you will find it on the Misc Values page. If you look up a G12.1 or G112 online you will find what I am referring to. The G12.1 or G112 is a Face Milling function for the lathe and will turn your choppy motion into nice smooth motion.

 

This is what I am talking about

 
image hosting without registration​ 

[The Cathedral]

If you don't have, or cannot use that function for some reason, a "poor mans" option to smooth out the motion is to go into your arc filter page, and set the Smoothing settings to "Use Fixed Segment Length" of .020 or so. This will smooth it out, at the expense of a very, very long program.

[#Rekd™]

Your code seems a lot different then ours.

 

This one is with Transmit/Tracyl On:

 

T=""END_MILL_.375""
TC(1)
G54
;MILL HEX
G94 S1=1500 M1=3
M413
SPOS[4]=0
M4=10
G0 X1.9914 Z1. M108
G17
TRANSMIT
STOPRE
G94 G1 X-1.4708 H-136.9377 F50.
Z.1
H0. F30.
Z-1.038
G41 X-1.2776 H.0259 F15.
G3 X-1.1561 H.0466 CR=.1
G2 X-.7101 H.1287 CR=.2575
G1 X.7101 H0.
G2 X1.1561 H-.1287 CR=.2575
G1 X1.8663 H-.615
G2 X1.9353 H-.1288 CR=.2575
X1.8663 CR=.2575
G1 X1.1561 H-.615
G2 X.7101 H-.1287 CR=.2575
G1 X-.7101 H0.
G2 X-1.1561 H.1287 CR=.2575
G1 X-1.8663 H.615
G2 X-1.9353 H.1288 CR=.2575
X-1.8663 CR=.2575
G1 X-1.1561 H.615
G2 X-1.0254 H.0748 CR=.2575
G3 X-.9495 H.0665 CR=.1
G1 G40 X-.9242 H.0992
X-1.3842 H-.338
G41 X-1.191 H.0259
G3 X-1.0695 H.0466 CR=.1
G2 X-.7101 H.1037 CR=.2075

 

 

 

This one is with Transmit/Tracyl Off:

 

T=""END_MILL_.375""
TC(1)
G54
M4=10
G0 X.9957 Z1. M108
G17
Z.1C4=IC(0.)
G1 Z-1.038C4=IC(0.) F30.
G41 X.9456C4=IC(5.111) F766.2735
X.9395C4=IC(.881) F842.087
X.9361C4=IC(.935) F894.1694
X.9354C4=IC(.96) F917.4407
X.9373C4=IC(.952)
X.942C4=IC(.914) F873.7662
X.9521C4=IC(1.706) F854.6022
X.9597C4=IC(1.736) F869.6139
X.9648C4=IC(1.758) F880.1542
X.9673C4=IC(1.769)
C4=IC(1.774)
X.9648C4=IC(1.769)
X.9597C4=IC(1.758)
X.9521C4=IC(1.736) F869.6132
X.942C4=IC(1.706) F854.59