OmniTurn New Generation CNC Control
Fast... Precise... Affordable...


C-Axis Plane Switching

Plane switching allows you to program parts using the C axis in combination with the X or Z axis as if you were programming a milling machine.

There are two plane-switched modes: XC and ZC :


XC Plane Image

XC Plane:

In the XC plane, the Omniturn’s X and C axes work together to trace an X-Y tool path on the face of a part. In this mode the live tool is oriented parallel to the Z axis. The live tool will do its cutting on the negative X side of the part centerline.


Live tool parallel with Z-Axis.






ZC Plane Image
ZC Plane:

In the ZC plane, the Omniturn’s X and C axes work together to trace an X-Y tool path on the side of a part. The OmniTurn Z axis becomes the milling machine’s X axis and the C axis emulates the mill’s Y axis. In the ZC mode, the live spindle is oriented parallel to the X axis on the negative X side of the part.

Live tool parallel with X-Axis





The programming details for plane switching are not yet finalized, so currently plane-switching commands need to be hidden from the error checking software by placing them in parentheses. The only commands permitted in the plane-switched part of the program are axis moves and feedrate commands. There is no cutter compensation, so it is up to you to write the program for the endmill you are using. All dimensions in the plane-switched mode are in absolute coordinates.

The commands are as follows:

(~PLXC): Start XC mode. The tilde character “~” in a (comment) alerts the Omniturn’s parsing program to scan for a plane switching command.

(~PLZC): Start ZC mode. The tilde character “~” in a (comment) alerts the Omniturn’s parsing program to scan for a plane switching command.

(Xnn): moves the X axis to the specified coordinate

(Ynn): moves the Y axis to the specified coordinate

(G02XnnYnnInnJnn): moves X and Y to the specified coordinates clockwise along a circular path with its center located at the I dimension in X and the J dimension in Y.

(G03): same as G02 but travels CCW along the arc.

(Fnnn): feedrate specified in inches per minute

(Znn): moves the virtual mill’s Z axis.
In the ZC plane, the Z dimension is specified as the diameter of the cylinder the tool’s tip would touch.
In the XC plane, the Z axis is the same as it would be if plane switching was not in effect.

(Dnn)(ZC plane only): specifies the part diameter at which the Y dimensions are translated to C axis rotation.

This value defaults to the virtual mill’s Z position (that is, the diameter at the tool’s tip) at the start of the plane-switched operation.

It should only be changed when the Y position is 0, since it causes a re-scaling of the Y dimensions on the first move after it is programmed.

The reason this parameter exists is that you may want the Y dimensions to be calculated at the surface of the part rather than at the depth of cut.

(END): cancel plane-switch mode

Note: if you copy the plane-switch programs, do not include comments in the plane switched section. Nothing is allowed in the plane-switched program except the program statements described above.





Back to Top          Back to CNC Info

OmniTurn
(541) 332-7004
(541) 332-1018 fax

email sales@omniturn.com
[ Home ] [ GT-75.htm ] [ CNC Control ] [ Custom X-Z Slides ] [ Repair Parts ] [ Rebuilding your OmniTurn ] [ Used OmniTurns ] [ Contact Us ] [ OmniTurn ZipLoader ] [ Repair Catalog (PDF) ]