Z Level Roughing (Superseded) dialog - General tab

Strategy - Specifies a roughing strategy:

Pocket - Generates a roughing areaclear cycle using a concentric toolpath strategy.

External Boss - Generates a series of offset toolpaths from the inner shape clipped to the outer shape. The toolpaths always start from the outside.

Lace - Generates a roughing cycle using a laced toolpath strategy.

Mill Type - The cutter can move along a profile on the left or right hand side. This, combined with the spindle direction, gives the type of cutting to be either Climb or Conventional.

Climb - Tool cuts on the left of the profile (i.e. material is on the right).

Conventional - Tool cuts on right of the profile

Optimised - Cycle is optimised to reduce link moves. The tool may cut on the left or right side.

Direction - There are two possible ways for a series of concentric toolpaths to be cut:

Inside Out - Start the cycle with the innermost toolpath first. The tool plunges into material unless start holes are pre-drilled. This is the most commonly used method, and should be used if any parameters are set on the Approach tab.

Outside In - Start the cycle with the outermost path first. This should only be used when the Approach Strategy is set to Plunge, as the tool cannot perform a helical or zigzag approach starting from the boundary.

Link Control - Specifies a link move strategy between islands (only available if strategy is Pocket) :

Retract - The tool rapids to the clearance plane, rapids in the workplane to the start of the next toolpath element and then feeds down to depth.

Shortest - The tool feeds directly (using the shortest route, avoiding islands) to the next toolpath element, remaining at depth the whole time.

Mill Type - Similar to the Shortest link strategy, but the link is controlled by the Mill Type for the cycle.

% Stepover - Specifies the tool stepover distance between each pass as a percentage of the tool diameter.

Cut Increment - Specifies the depth of each successive cut. This must be a positive value. The cut increment value sets the vertical distance between successive planes.

Offset - Specifies the toolpath offset from the surface. Note that this is a three dimensional offset from the surface. The offset can be positive, but if negative, the offset must be smaller than the tool corner radius.

Using a Negative Offset
A negative offset cannot be equal or greater than the tool radius. When machining with a negative offset this produces the same results as reducing the tool radius by the offset, e.g. a 4mm ballnose tool used on a cycle with a -1.5 offset means the part is calculated using a 1mm ballnose tool. If the resultant tool size is very small please be aware that the tool could fall between small gaps in the model and the calculation time increases.

Tolerance - Controls the accuracy to which the surface is machined. A small value results in a more accurate surface finish but takes longer to generate the toolpath.

Lace Angle - (Only available if strategy is Lace) Specifies the angle between each pass and the X axis of the Initial CPL.

Feature Name - Enter a name here to allow labelling of digitised information for this cycle to enable "pickup" of this information in another (similar) cycle.

Feedrate - Specifies the rate of movement in the workplane.

Plunge Feed - Specifies the rate of movement in the direction of the tool axis.

Speed - Specifies the tool spindle speed.