Showing results for 
Search instead for 
Do you mean 
Reply

Multi-Axis Contour Profile

[ Edited ]

 

Hello there,

 

I ran into a problem when posting a multi-axis contour profile operation.

 

I set the Motion Output Type in the Machine Control section of the operation dialog as Arc (this doesn’t matter). The generated tool paths can be seen below. The work piece is hidden. You can see a bunch of points on the tool path, as I turned on the End Point in the Display Group.

MotionControl.PNG

Capture1.PNG

Then I post processed the operation with a multi-axis post. As it is a vector operation, in the post, you can see a bunch of points as follows:

 

LN X-14.428 Y6.0842 Z.005 TX0. TY0. TZ1.

 

These lines are generated from the Linear Move section of the post. From point A to point B, there are about 440 points in the NC program.

Post.PNG

The question is what in the post decides how many points should be generated to complete the tool path. (why are there 440 points between A and B)

 

Thanks,

Kai

10 REPLIES

Re: Multi-Axis Contour Profile

How much does the tool axis change between A and B?

What is the Max Tool Axis Change in the operation?

Mark Rief
Retired Siemens

Re: Multi-Axis Contour Profile

Hello Mark,

 

Thanks for your reply.

 

There is no tool axis change between points A and B. 

 

We set the Max Tool Axis Change as 180 Per Step in the dialog.

 

Thanks,

Kai

Re: Multi-Axis Contour Profile

[ Edited ]

I can't think of anything else obvious to check.

If the tool path listing matches the points shown in the picture, but the post adds a lot more without any tool axis changes, I suggest you contact GTAC, so that they can take a closer look at your post. 

Mark Rief
Retired Siemens

Re: Multi-Axis Contour Profile

1) Does the internal toolpath have arc output (CIRCLE records)? (right click on the operation -> Toolpath -> list) 2) If so, I'm guessing due to the variable axis operation type, or due to the arcs not being in the XY/XZ/YZ plane, the post is converting arcs to linear moves. If (2) is true, then the tolerance is coming from within the post. I am *guessing* it is the variable "mom_kin_linearization_tol" (set in "Machine tool" tab -> click on one of the rotary axes, then click on the "Configure" button) If this is too coarse, then you can do one or more of the following: - in the operation, change the arc output mode to "linear" (or whatever that optioni is named) - make the linearization tolerance smaller - make the post support arcs in non-principal planes Hope this helps...Ken
Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Multi-Axis Contour Profile

Thanks, Ken. The arc is on XY plane. 

 

I think the reason why there are only linear moves in the NC program is that it is a vector operation type.

 

Changing output mode from arc to line can certainly add more points, but we are still not sure what controls the number of points generated by the post.

 

I tried changing the Linearization Tolerance both for arc and line output mode, but nothing changed.

 

Thanks,

Kai

Re: Multi-Axis Contour Profile

If the tool axis is fixed and you are making a planar cut why are you using Contour Profile?
NX11.0.1

Re: Multi-Axis Contour Profile

Then we'll have to dig deeper into the tcl code.

Search the post's tcl file for mom_operation_type or mom_tool_axis_type.

See if it does anything based on variable axis.  Particularly to mom_kin_arc_output_mode or mom_kin_arc_valid_plane

 

Also (in arc move) check min radius & length (I didn't see a scale factor in you picture, are these really tiny arcs? I was assuming not)

 

Are you using Lock axis UDE?

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Multi-Axis Contour Profile

Thanks, Dstryr. Before Point A, there are many tool axis changes.

 

Kai

Re: Multi-Axis Contour Profile

Thanks, Ken.

 

There are several procedures that set the value of mom_kin_arc_output_mode.

 

#=============================================================
proc PB_CMD_detect_5axis_mode { } {
#=============================================================
  global mom_kin_arc_output_mode
......
  if {[DETECT_5AXIS_SIMULT]} {
    ......
     set mom_kin_arc_output_mode "LINEAR"   
  } else {
    ......
  }
}


#=============================================================
proc PB_CMD_reset_5axis_control_mode { } {
#=============================================================
#Cancel M128
if {[ info exists mom_tnc_5axis_control_mode ] && $mom_tnc_5axis_control_mode == "M128"} {
set mom_kin_arc_output_mode "FULL_CIRCLE"
......
}
}


#=============================================================
proc SET_LOCK { axis plane value } {
#=============================================================
# called by MOM_lock_axis
......
set mom_kin_arc_output_mode "LINEAR"
}

Do these control the number of points?

 

The minimum arc in the tool path is R 0.2, L 0.314.

 

We are not using Lock axis UDE.

 

Thanks,

Kai

Learn online





Solution Information