M-Series Operator’s Manual 4/9/15
5-2
Height Offset
This is the distance the control adjusts Z-axis positions when tool length compensation (G43 or G44) is used with a
particular H value. For example, if H001 is -1.0 and the job contains G43 H1, then the CNC software will shift all
Z-axis positions down 1.0 to compensate for the shorter tool.
To edit the Height Offset entries move to the desired height offset number with the arrow keys, Page Up, Page
Down, HOME, and END. You can choose to manually edit or automatically measure the value.
Height Offsets values are measured using the Z Reference position. The Z Reference position is the Z-axis position
when the tip of the reference tool is touching the work surface. The reference tool should always be the longest
tool.
The Height Offset value for end mills and drills is the difference between the Z-axis position when the tip of the
tool is touching the work surface and the Z Reference position. The Height offset value for ball nose and bull nose
cutters is the difference between the Z-axis position when the center of the tool is at the work surface and the Z
reference position. Because it is not possible to position the tool in this way, you must instead move the tip of the
tool to the work surface, and then manually edit the value to subtract the tool nose radius.
To manually edit a Height Offset value, simply type the desired value and press ENTER.
To manually measure Height Offset values, use the following procedure:
Establishing the Z reference position
Press F1 – Z Ref to select the Z Reference setting function.
Insert the longest tool into the tool holder (you can use the jog keys or the TOOL CHECK key to assist you).
Jog the tip of the tool down to the top of the work surface.
Press F10 - Save to save this Z Position as the Reference Position.
Measuring each tool height (Z position for tool minus Z position for Reference tool)
Insert the desired tool into the tool holder (Jog keys or the TOOL CHECK key can be used to assist you).
Jog the tip of the tool down to the top of the work surface.
If the tool is a drill or end mill, press F2 –Manual Measure to measure the height.
If the tool is a ball nose or bull nose cutter, press F2 – Manual Measure to measure the height, and then subtract
the tool nose radius.
After a tool height is measured, the next Height Offset entry is automatically selected.
When the edit is complete, press F10 - Save to save the Offset Library and Exit.
Examples (assuming Z Reference = -1.5):
If the tool position is -1.75, then the tool height = -0.25
If the tool position is -1.75 and nose radius is .25, then the tool height = -0.50
If the tool position is -2.25, then the tool height = -0.75
If the tool position is -2.75 and nose radius is .125, then the tool height = -1.375
Diameter
This field tells the control the distance to adjust when cutter diameter compensation (G41 or G42) is used with a
particular D value. For example, if D001 is 0.5 and the job contains G41 D1, the CNC software will adjust all X-Y
positions 0.25 (half the tool diameter) to the left of the programmed tool path.
To edit the Diameter entries move to the desired diameter offset number with the arrow keys, Page Up,
Page Down, HOME, and END. You must manually edit the Diameter Offset value. Type the desired value and
then press the ENTER key.
You can make small adjustments to Height Offsets and Diameters using F5 - +.001 and F6 - -.001. Use the arrow
keys to highlight the value to be adjusted. Press F5 - +.001 to increase the offset value by 0.001" (or 0.02 mm in
Metric mode). Press F6 - -.001 to decrease the offset by the same amount. If the cut parts are undersized, use F5 -
+.001 to cut less material. If the cut parts are oversized, use F6 - -.001 to cut more material.
To Next Page
Loading...
