Contour parallel Finishing

The Surface Milling Contour Parallel cutting strategy is a finishing toolpath. It uses a pattern, similar to the Pocket-Contour Parallel, and projects this cutting pattern onto the selected surfaces.

The inputs to the function are a 3D surface, and optionally a start point, a closed chain contour restriction boundary, closed chain islands within the outer boundary, and a stock box. The contour rules are the same as for Contour parallel pocketing, non intersecting, closed contours. The restriction boundaries should be flat in the X-Y plane, but can be drawn at any Z height. Use a Stock box to restrict a toolpath without a surface underneath, such as when a restriction curve is larger than the selected surfaces.

If no restriction boundaries are defined, the toolpath will be a rectangular shape within the X and Y extents of the surfaces to be machined. If a start point is defined, the first plunge will be to the surface depth at that point, from which the cutter will profile along the surface toward the normal contour parallel pocket toolpath, which is projected onto the 3D surface.

Because it is often desired to cut a 3D surface in parallel contours to the outer edges, the Vector 3D curve and surface modeling tools provide powerful support in refining the finish toolpath.

Start with an irregular outline surface:

Select the surfaces, and then extract the surface edges with 3D-Extract Surface edges

3D-Curve-Project curve on Plane

Set Z depth to -.1, OK

Draw-Other Curves-Offset, distance = .5, OK. Note: use one-path option on the Offset dialog to create a single offset curve around multiple and complex surface edges.

Change-Break-Interpolate

Draw-Spline-Arc-Spline

Select the surfaces then NC-3D-Milling-Contour Parallel

Tool Section

Select Tool from the milling tool table, diameter D and E will be supplied from the tool library. They can be overridden after selection.

Tool Origin can be either tool tip or center of the radius on a ball end mill

NC Path Section

Sidestep distance based on the desired surface finish. After entering the Sidestep distance and pressing Tab, the theoretical scallop height is calculated from the tool size and the Side step distance values.

Set Interpolation errors according to the desired surface accuracy tolerances. Start with a relatively large value to reduce calculation times. Use Undo to return to the dialog and try different values. Set to a smaller value after the desired toolpath form has been achieved. Smaller values will dramatically increase the calculation times.

Click the Z-Connections button to change the default Z connect heights and settings.

Note the Z Incremental can be used to permit rapids close to the surface just prior to cutting. Unchecking, Z-Incremental results in rapids to the Z clearance plane, this is the safest condition, but may result in extended feeds at reduced rates through air as the tool feeds through the distance between the Z clearance plane and the 3D surface location.

Surfaces Section

Interpolation error – the approximate distance along the surfaces that will be used for evaluating the toolpath location. Start with a relatively large number when setting up the toolpath, and then reduce to the desired accuracy, after the desired pattern is achieved. Smaller values can cause a large increase in computation time, so do not use excessively small numbers, but rather reasonable for the cutting conditions, taking into consideration the tool flex, machine rigidity, etc.

Stockdistance is the minimum amount of material that will be left on the surface of the model, after machining.

Contour Parallel Section

Conventional- (Up) milling. By default the Contour parallel toolpath will climb mill. Check the box if conventional milling is desired.

From Outside to Inside. The default cutting pattern is from inside to outside, the same as a contour parallel pocket. Check the box if the reverse is desired, then the toolpath will be created from outside to inside.

Region Section

The region of cut is set by the selection.

Inside, the toolpath will be offset by the boundaries and the tool will not cross over into adjacent regions

On, the center of the cutter will follow the curve of the boundaries.

Outside, the toolpath is offset outside the boundaries to assure that there is a margin around the boundaries, equal to at lease one tool radius.

Options Section

Translate connections over dZ. The default value is 0. In this case the connections between the successive contour parallel paths will follow the surface. If any value greater than 0 is entered, each successive contour parallel ring will be connected by a Z lift, and there will be no cutting between the contours.

Jobs Tab

The Jobs tab permits changing of the tool, and the associated parameters for Feed, Feed Reduced, and Speed. The Job step can also be named/re-named.

Although the toolpaths appear to be flat, 2 axis, X-Y waterlines, this is dependant on the offset restriction boundary. If this boundary is not close to the same shape as the surface outline, and if the surface has a non-uniform cross section, the toolpaths will be more and more 3 axis motions. The side step distance used for this example is very coarse and would probably be sufficient for roughing, but would not produce a smooth finish surface. Use a much finer side step and a resulting smaller scallop height.