Specifications

Southwestern Industries, Inc.

TRAK LPM Programming, Safety, & Operating Manual

Y3 POCKET: Y dimension for the opposite corner of the rectangular pocket that

surrounds the island.

CONRAD PCKT: the value of the tangential radius in the corners of the rectangular

pocket that surrounds the island.

FIN CUT PCKT: finish cut along the perimeter of the pocket. If 0 is input, there will be

no finish cut. See the previous section for a bottom finish cut.

RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous

event.

FIN RPM: is the spindle RPM for the finish cut.

Z FEEDRATE: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or

mm/min from 5 to 17780.

XYZ FEEDRATE: the milling feedrate in in/min from .1 to 800, or mm/min from 5 to

20320.

FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts.

TOOL #: is the tool number you assign.

When the initial screen is complete, you will define the perimeter of the island with a

series of A.G.E. Mills and A.G.E. Arcs. Programming with the Auto Geometry Engine is

explained in Section 9.0.

8.8 PROFILE Events

This event allows you to mill around the outside or inside of a circular or rectangular

frame or an irregular profile. The irregular profile may be closed or open. All profiles

are limited to the XY plane.

When the irregular profile event is started the ProtoTRAK PMX CNC will automatically

initiate the powerful Auto Geometry Engine. See Section 9.0 for programming with

A.G.E.

8.8.1 Circle Profile

Press the CIRCLE soft key if you wish to mill a circular frame.

Prompts in the Circle Profile event:

X Center: is the X dimension to the center of the circle

Y Center: is the Y dimension to the center of the circle

Z Rapid: is the Z dimension to transition from rapid to feed

Z End: is the Z dimension to the bottom of the frame; incremental is from the previous

event

Radius: is the finish radius of the circle

Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for milling

Tool Offset: is the selection of the tool offset to the right (input 1), offset to the left

(input 2), or tool center--no offset (input 0) relative to the programmed edge and direction

of the cutter movement

# Passes: is the number of cycles to machine to the final depth spaced equally from Z

Rapid to Z End (hint: keep Z Rapid small)

Fin Cut: is the width of the finish cut. If 0 is input, there will be no finish cut