The Global Parameters section allows you to set the tolerance value to be used in machining. A uniform thickness or stock that needs to be left around the part can be specified here.

Tolerance  

This is the allowable deviation from the actual part geometry plus the Stock allowance (if any).  In 2 Axis methods, this Tolerance is applied to XY motions only.

Tolerance

How to Increase Tool Path Accuracy

Stock

This is the thickness of the layer that will remain on top of the part after the toolpath is complete. Roughing operations generally leave a thin layer of stock.  For finishing operations this value is zero.

Stock

Compensation  

This enables cutter compensation.  The compensation direction, left or right, is determined by the Cut Direction selected (Climb or Conventional).

Island Offset

The tool will traverse in successive uniform offsets of the part shape

Island Offset

Linear Cuts

Select Linear and the tool will traverse in a Linear cut beginning at the Top or Bottom depending on the Start Point selection.

Linear

High Speed

Select High Speed to add progressive arc-shaped passes that reduces tool pressure and keeps chip load more consistent, allowing for higher cut feedrates.

High Speed

Cut Direction refers to the rotational cut direction of the tool in relation to the stock.  

Understanding Climb vs Conventional Milling

Climb (Down Cut)  

Select Climb (Down Cut) and the tool will be maintained in a downward motion into the stock.

Climb (Down Cut)

Conventional (Up Cut)  

Select Conventional (Up Cut) and the direction of the tool will be maintained in an upward motion out of the stock.

Conventional (Up Cut)

Mixed  

Select Mixed and the direction of cutting is alternated between each parallel plane.  This is a mixture of both Climb and Conventional cutting of the stock.  When Mixed is selected, zigzag motions are applied between step downs to eliminate tool retracts between z levels.  If Climb or Conventional is selected, retract between z levels are applied.

Mixed

Stepover Distance

Specify the stepover distance for the current operation as a percentage of the active tool diameter (% Tool Dia) and then enter the percentage value.

% Tool Dia.

Specify the stepover for the current operation as an exact Distance and then enter the distance value in the field provided.

Distance

Corner Cleanup

Automatically detect corners that the tool could not reach between cut level and add a toolpath based on the uncut area detected.  Either Linear or Offset cut patterns are used in these areas.

Cleanup Pass

No Cleanup Pass

Cleanup Pass

Automatically detect corners that the tool could not reach between cut level and add a toolpath based on the uncut area detected.  Either Linear or Offset cut patterns are used in these areas.

Cleanup Pass

No Cleanup Pass

Angle of Cuts

Specify the Angle of Cuts (0-360) measured from the X Axis.  This additional parameter is available for some operations when a linear cut pattern is used.

Start Point

For the Linear Cut Pattern, select the starting location for the cut.  This is not an exact point coordinate but a general location of Top or Bottom.

Start at Bottom

Select this option if you want the starting locating for the cut pattern to begin at the bottom of the cut pattern (i.e., min Y).

Start at Bottom

Start at Top

Select this option if you want the starting locating for the cut pattern to begin at the top of the cut pattern (i.e., maximum Y).

Start at Top

Transfer Cut Control (for High-Speed Cut Pattern Only)

Lift Cut

During the High Speed cut pattern use this parameter to lift the cutting tool during transfer motions.  0 (Zero) means that the tool will not list.  Enter a positive value and the tool will lift this amount in +Z prior to executing a cut transfer motion.

Feedrate Factor

During the High Speed cut pattern use this parameter to control the feed rate when the cutting tool is lifting and plunging before and after each cut transfer motion.  The value is a percentage of the Cut Feed (Cf) parameter for this operation (i.e., 50 = 50% of the (Cf) feed rate).