Project 4: Contour Square Step

This exercise teaches how to do the following:

The fixture offset is a point on the part that can be easily and accurately found by mechanical means. For example, in Figure A.12, the upper-left corner of the stock can be located using an edge finder. The fixture offset (G54) is located at this point. If it were not, the datum could be shifted from this reference point by changing the G54 XYZ-values on the machine control.

Figure A.12: Contour Block

It is common to choose the upper-left corner of the stock as the fixture offset for the first operation. If the stock is sawed, ensure there is sufficient stock allowance around the part so finish operations remove material all around.

For subsequent operations the fixture offset is set from features machined in previous operations.

1. Square Block

Begin with a finish machined 2x2x3in block (created in Project 3).

2. Find Fixture Offset XY

Use an edge finder to locate the upper-left corner of the block (shown by the black dot in Figure A.12).

3. Set Fixture Offset A

Set the fixture offset Z (G54) to the top of the block.

Figure A.13: Set G54

4. Program Contour Tool Path

Create a contour tool path to mill a .100x.100 step around the part as shown above. Use Wear compensation, line/arc lead in/out moves, and the correct cutting speed and feed for the tool. Use a finish pass of XY .010 in and Z .005 in to ensure the wall and floor are dimensionally accurate and have a good surface finish.

Contour Block: Job-1 Setup

G54 Datum: Upper-Left corner of previously finish machined 2x2x3 in block.

Tool (in)
.25 End Mill 4-Flute
Speed (rpm)
Feed XY (ipm)
Feed Z (ipm)

Rough and finish the OD contour using wear compensation. Make one roughing pass and then a finish pass that removes .010 in stock on walls, and .005 in on floor.

Table A.1: Contour Tool Path

5. Adjust CDC

After machining the contour, measure it with a dial indicator. The step should be exactly .100 in ±.001 in depth. If not, the G54 Z position or Tool Length Offset (TLO) was not set properly.

Check that the boss measures 1.800 x 1.800 in ±.001. If it is too large, it is likely because the tool is worn and thus not exactly .250 diameter. Adjust for this wear by changing the wear compensation (CDC) for this tool on the control, and then re-running the program.