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.

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.

Compensation

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

Climb (Down Cut)  

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

Conventional (Up Cut)  

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

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.

Understanding Climb vs Conventional Milling

For Z Level Cuts:
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.  Refer to the images below:

Check this box to move the cut start point to the mid-point of the longest side of a closed curve.

Specify

Select this option to activate the Cutting Side parameters in this dialog.

Right of Curve / Left of Curve

Right or Left determines the side of the curve to cut.  This can be set for both open and closed curves. Right or Left is determined by the start point and direction.

Use Inside/Outside for Closed Curves

Select this option if you have a closed curve region.  Then select Inside or Outside to have the tool cut on that side.

Alternate using Nesting

If your control geometry has nested curves, check this box to alternate the cut side (i.e., Outside/Inside or Inside/Outside). You can use the Sort Parameters tab to sort clustered profiles.

Total Cut Width

This is how wide your cut should be and the stepover amount for each cutting pass beginning at your total cut width and ending at your control geometry. For example if Total Cut Width is set to 1.0 and Step/Cut is set to 0.25, there will be 4 passes created. You can use the Measure button to select two points to determine the Total Cut Width.

Step per Cut

This will determine the stepover for each cutting pass beginning at your total cut width and ending at your control geometry.

Checking the Corner Cleanup box will cause automatic detection of all the corners that the tool could not reach between each pass. It will then add a toolpath based on the uncut area detected; either a linear cut in case of smaller areas or a cut that travels along the shape of the uncut area, when the area is large.

With this parameter checked, the cutter will not violate any of the selected control geometry. This option only works with closed curves as shown in the illustration below.