Circular interpolation problem with UGS NX 7.5

[wlamers]

Dear all,

I am facing the following problem with a Fanuc 6Mb control in combination with UGS NX CAM 7.5.

NX generates a 3d circular(helical?) path during the beginning of a cavity mill operation (to smoothly enter the blank). The post processor then converts this tool path to a G03 circular interpolation code for the Fanuc 6M control.

The problem is that the Fanuc control can not handle this command. It can handle in plane (2d) circular interpolation, but not combined with a 3rd axis. If have added an example below:

This goes wrong: G03 X100. Y54. Z38. I3.799 J2.412 K-1.206 F200.
This works: G03 X100. Y54. I3.799 J2.412 F200.

Maybe someone knows a way to adapat the control (via a parameter?) such that this will be possible to do this on the machine? A second option would be to let NX generate a toolpath which is not 3D circular. I cann't find a way to do this in NX. Can someone help me with this?


Thanks in advance and best regards,

W.Lamers

[jelmerra]

Helical interpolation is an option on fanuc controllers, I suppose you could get a quote from fanuc to solve the problem.

Another option would be to alter the postprocessor in such a way that it no longer outputs helicals.

Within NX you could choose not to generate helicals e.g. choose ramp on shape or something similar.

Jelmerra

[markrief]

If your conrtoller will not do helical, edit the post in Post Builder, go to custom commands, edit init_helix, and set the helical arc output mode to linear.

[1 Infinite Loop]

Also, even if a control can do helical, the K may be causing an issue. As Mark mentioned you can edit the custom command, but this time to get rid of the K edit mom_sys_helix_pitch_type to "none".

I, J and K are incremental swing points for an arc move but your K in question is probably being output as the pitch in Z which you don't need for your helical move. K is usually associated with G2 and G3 moves in XZ and YZ planes.

Just a thought; did you try the helical move using Z but without K? You may be surprised that your control may be able to do helical after all. That is a very common option to have, even on the old 6M and 11M controls.

[wlamers]

Thank you for your replies.

I'll try to find out if the machine can do helical by removing the k paramater. But how does the machine know what the z-axis pitch has to be then?

I've found out that the maxine is actualy a 2.5d machine. Only 2 axis's can be controlled at the same time. The strange thing is that i've made a 3d program (mold product) which does have 3d coordinates where the machine is told to move in three directions at the same time. The final product looks ok. I cannot check if it actually did mill in 3d since the movements where really small (0.01 mm). Whats happing here? Does the control move 2 axis's at the same time and when ready move the third one?


Best regards,

W.Lamers

[1 Infinite Loop]

Good question. It could be doing something bizarre like you described but I would think the control would alarm if it cannot execute the program as is. If it is moving in 3-axis, it can be true without having the option turned on to do helical movements. Helical is just another option like macro, extra offsets, number of programs, etc-.

A simple test you can perform is program the machine to move G01 X1. Y1. Z1. and see what it does. You can stop the feed somewhere in the middle of the move and your positions should be the same. This has to be performed with G01, not G00. Many older machines cannot do linear positioning in G00.

As far as your pitch question is concerned and assuming you are doing G2 or G3 with G17 in the XY plane, normally in older Fanuc controls the Z tells the machine where to go in absolute and is the destination as are the X and Y; at least that is how it works on our older machines which are 11M and 0M. If Postbuilder can output the pitch then there must be machines that take the pitch or perhaps the pitch is used in incremental programming; I'm not sure.