Mazak 410E integrex

[DODGERFAN]

I am having an issue with the C axis rotating during a milling operation. The C axis does not need to rotate and I have set the axis control to NO ROTATION. But it is rotating anyfrigginway.

Its just a simple cut from front view just going from right to left, no need to rotate at all.

What am I missing?

Ops 8-13 do it and makes no sense. Please advise. Thank you.

X7 MU2

M1187190.MCX-7

[DODGERFAN]

I should note that it does not rotate in mastercam verify but it posts a lot oc c axis moves.

I am also using an Icam post.

 

 

(T6 | 3/4 BULL ENDMILL 0.25 RAD | EIA SUFFIX - .00 | MAZATROL SUFFIX - .00)

G20 G10.9 X0

G91 G30 P3 X0.

G30 P3 Z0.

M200

T6 T7 M6

G91 G30 P3 X0. Z0.

G90

G54

M108

M212

G97 S1528 M3

G0 G43 X-.575 Y.937 Z5. B0. C0.

G17

M210

M107

Z.1

G94 G1 Z-.74 F8.56

X-.5 F15.28

X.5111

X.5861

G0 C31.949

G1 X0. Y1.0866

X.0636 Y1.0469

X.9216 Y.5119

X.9852 Y.4722

G0 C32.373

G1 X0. Y1.0739

X.0633 Y1.0337

X.9173 Y.4924

X.9806 Y.4522

G0 C32.807

G1 X0. Y1.0613

X.063 Y1.0206

X.9129 Y.4728

X.9759 Y.4322

G0 C32.953

G1 X0. Y1.0571

X.0629 Y1.0163

X.9113 Y.4663

X.9743 Y.4255

G0 C33.101

G1 X0. Y1.0529

X.0628 Y1.0119

X.9098 Y.4597

X.9726 Y.4188

G0 Z5.

G97 S713 M3

G54

G49 X-.9852 Y-.4584 Z5.0885

Z.1885

G1 Z-.75 F8.56

X-.9224 Y-.4993

X-.0754 Y-1.0515

X-.0126 Y-1.0924

G0 C0.

G1 X-.575 Y-.907

X-.5

X.5111

X.5861

G0 C-32.807

G1 X0. Y-1.0613

X.063 Y-1.0206

X.9129 Y-.4728

X.9759 Y-.4322

G0 C-33.251

G1 X0. Y-1.0487

X.0627 Y-1.0076

X.9083 Y-.4532

X.971 Y-.4121

G0 C-33.401

G1 X0. Y-1.0445

X.0626 Y-1.0032

X.9067 Y-.4466

X.9693 Y-.4053

G0 Z5.0885

M108

M212

M5

G91 G30 P3 X0.

G30 P3 Y0. Z0.

G90

[Mark@Joa]

Looking at the program you have I would say you are going to far below center on the X axis and the Icam post is trying to compensate by turning the C axis. I also do a lot of programming for a 410E and if I tried to post out the program you have I would get over travel alarms at the machine on the X. The 410 we have can only go .75" below center and this program is going .8996" below. Yours may be different but I would say you need to turn WCS "face" 90 degrees so the move would be a straight Y axis move.

[DODGERFAN]

Thank you Mark. I rotated everything 90° and re-chained it all, now it works much better.

This is my secong program for this machine, so I gots lots to learn. Thanks again.