Okuma M560-V P300 rotary A axis limits

Does anyone know how to set soft limits for axis A (rotary axis)? I have a fixture that will hit the table if rotated too far. I already talked to Gosiger and they can't figure it out yet. I have already tried changing the user parameters and the system parameters but the machine still rotates wherever it wants.

riser so it don't hit?

WILLEO6709 said:

riser so it don't hit?

Click to expand...

That's what I did.

I wonder if it has anything to do with other 4th axis settings, like continuous wrap (can't remember what Okuma calls it)..or shortest path rotation vs directional...just wondering if you're in the right spot but something else is conflicting with it so it's ignoring your limits.

Gosiger finally got to me on this issue. changed NC Optional Parameter Bit N0. 70 bit 6 rotary axis with limit or without (check box)

They sent this .doc

SYNC SCALES: CAL X, Y, Z scales with encoders in System Parameters

************************************************************

Multi Turn Function (Do not use for simultaneous)

NC Optional Parameter Bit No 39

Bit 3 A-Axis to 1
Bit 4 B-Axis to 1
Bit 5 C-Axis to 1

************************************************************

* Short connection for rotation direction ( Replaces using M15 M16)

*NC Optional Parameter Bit No 69

*Bit 0 4th-Axis to 1 (B-Axis on HMC)
*Bit 1 5th-Axis to 1
Bit 2 6th-Axis to 1

After reset or Power on the rotary axis will always use shortest connection between 2 positions with M15 and M16 we can control CW or CCW.

Short cut by M-Code for MB-V form Jan 2005 and MA-100H from April 2005 Production.

M403 : 4th-axis
M404 : 5th-axis
M405 : 6th-axis

************************************************************

NC Optional Parameter Bit N0. 70 bit 6 rotary axis with limit or without

***********************************************************

*NC Optional Parameter Bit NO. 15 bit 7 (inch mode use F as feed rate for rotary axis)

***********************************************************

*For MU simultaneous machining, set A and C axis to modal in parameters. Stops automatic axis brake. (Uncheck boxes for brake modal and check boxes to use M code for brake). Parameter page-Additional Axis.

***********************************************************

NC Optional Parameter Bit No 54

Bit 2 - Inverse Time to 1

***********************************************************


NC Optional Parameter Bit No 67

Bit 5 – Accel Low Vibration Mode to 1

***********************************************************


NC Optional Parameter Bit No 46

Bit 0,1,2,3 – Rapid Interpolation for GOO, G30, G60, Home Movement to 1