This page gives you advanced settings for the Don't roll over the edge at all option.
There are two types of curves used by the Don't roll option. One type is a curve on the surfaces of the feature. This is called a part boundary and the points are the contact points where the tool stops at the edge of the feature. These curves do not depend on the tool. The second type of curve is a tool center (offset) curve. A tool center curve is a part boundary curve that has been offset by the tool edge radius. The Save combined boundary button on the Edges tab gives a preview of all the part boundary and tool center curves.
Part boundary tolerance — This controls the accuracy of the part boundaries. The default value is automatically computed. Smaller values give better results but take longer to compute. To reset to the default value, enter 0 and click OK, then click Apply on the Edges tab.
Use separate wall tolerance — The part boundaries use a tolerance to check for vertical surfaces (walls). By default it uses the Part boundary tolerance. Selecting this option enables you to enter a separate tolerance value for vertical walls. You may need to use this setting if you use the Cut to/from bottom of vertical walls option on the Edges tab. If you preview the part boundaries and they are not consistent at the bottom of vertical walls, select Use separate wall tolerance and enter a larger tolerance than the boundary tolerance above.
Offset boundary tolerance — This controls the accuracy of the tool center (offset) curves. The default value is the same as the Tolerance value on the Milling tab, but if you override it here it becomes a separate tolerance for the tool center curves.
Edge tolerance — This specifies the tolerance between the part boundaries and the surfaces. The default value of 0 means this tolerance is set automatically based on the boundary tolerance above. If the tool center curve is rolling over the edges of the feature you may need to set a larger edge tolerance (relative to the boundary tolerance).