Manufacture > Milling > 3D > Morph
The Morph Strategy will machine an area between 2 curves. The toolpath is guided by the basic shape of the curves. The chained curves can be open or closed boundaries. The system varies the toolpath to match the basic shape of the boundary curves.
Select the type of coolant used with the machine tool. Not all types will work with all machine postprocessors.
Spindle and Feedrate cutting parameters.
When enabled, this provides additional controls for collision handling. Collision detection can be done for both the tool shaft and holder, and they can be given separate clearances. Choose between several modes, depending on the machining strategy.
This function increases the number of calculations that need to be performed. This may effect the performance of your system on very large projects.
Select 2 or more curves to guide the toolpath. These can be edges from the model or sketch geometry. You can select Open or Closed boundaries to guide the toolpath.
Boundaries mode specifies how the toolpath boundary is confined. The following images are shown using a 3D Radial toolpath.
Example 1 Silhouette |
Example 2 Selection |
Bounding Box. |
Silhouette. |
Selection. |
Use tool containment to control the tools' position in relation to the selected boundary or boundaries.
Inside
The entire tool stays inside the boundary. As a result, the entire surface contained by the boundary might not be machined.
Center
The boundary limits the center of the tool. This setting ensures that the entire surface inside the boundary is machined. However, areas outside the boundary or boundaries might also be machined.
Outside
The toolpath is created inside the boundary, but the tool edge can move on the outside edge of the boundary.
Inside |
Center |
Outside |
Use the Additional Offset parameter, to overlap the boundary edge.
The additional offset is applied to the selected boundary/boundaries and tool containment.
A positive value offsets the boundary outwards unless the tool containment is Inside, in which case a positive value offsets inwards.
Negative offset with tool center on boundary |
No offset with tool center on boundary |
Positive offset with tool center on boundary |
To ensure that the edge of the tool overlaps the boundary, select the Outside tool containment method and specify a small positive value.
To ensure that the edge of the tool is completely clear of the boundary, select the Inside tool containment method and specify a small positive value.
When enabled, specifies that the boundary limits where the tool touches the part rather than the tool center location.
The difference is illustrated below on a Parallel toolpath using a ball end mill.
Toolpath driven by Tool Center. | Toolpath driven by Tool Contact Point |
Disabled |
Enabled |
Disabled |
Enabled |
Controls whether or not toolpaths are generated where the tool is not in contact with the machining surface. When disabled, toolpaths are extended to the limits of the containment boundary and across openings in the workpiece.
Enabled |
Disabled |
When selected, contains toolpaths based on a range of specified angles.
Only areas equal to or greater than the values in the From Slope Angle and To Slope Angle parameters are machined.
Most 3D finishing strategies support slope angle confinement. One use of slope confinement is to confine a selected toolpath strategy to angles where it works best. For example, Parallel Finish is better suited to shallow areas while Contour Finish is better suited to steep areas.
0° - 90° |
0° - 45° |
45° - 90° |
From Slope Angle is defined from the 0° (horizontal) plane. Only areas equal to or greater than this value are machined.
To Slope Angle is defined from the 0° (horizontal) plane. Only areas equal to or less than this value are machined.
Slope angle confinement is defined from 0° (horizontal) to 90° (vertical).
Slope angle from 0° |
Slope angle to 90° |
When checked this limits the operation to only remove material that a previous tool or operation could not remove.
Rest stands for REmaining STock.
|
Specifies the source from which the rest machining is to be calculated.
Uses the stock body as defined in the Setup
Specifies the diameter of the rest material tool.
Specifies the amount of stock from previous operations to ignore. Expressed in distance units. The parameter helps you avoid machining of minor rest material.
Specifies how the tool orientation is determined using a combination of triad orientation and origin options.
The Orientation drop-down menu provides the following options to set the orientation of the X, Y, and Z triad axes:
The Origin drop-down menu offers the following options for locating the triad origin:
Enable to override the model geometry (surfaces/bodies) defined in the setup. You can select a different model to apply the toolpath.
Enabled by default, the model selected in the setup is included in addition to the model surfaces selected in the operation. If you disable this checkbox, then the toolpath is generated only on the surfaces selected in the operation.
When enabled, you can select surfaces to avoid. The toolpath will stay away from the selected surfaces by a specified amount.
Disabled All surfaces are machined. |
Enabled Selected surfaces are avoided. |
The amount of clearance between the machined surfaces and the selected surfaces.
Inverts the meaning of the Avoid surfaces setting. When enabled, the avoid surfaces are the ones that must be touched within the given clearance while the remaining surfaces are avoided.
Touch surfaces
The Clearance height is the first height the tool rapids to on its way to the start of the tool path.
Clearance Height
The Clearance Height Offset is applied and is relative to the Clearance height selection in the above drop-down list.
Retract height sets the height that the tool moves up to before the next cutting pass. Retract height should be set above the Feed height and Top. Retract height is used together with the subsequent offset to establish the height.
Retract Height
Retract Height Offset is applied and is relative to the Retract height selection in the above drop-down list.
Top height sets the height that describes the top of the cut. Top height should be set above the Bottom. Top height is used together with the subsequent offset to establish the height.
Top Height
Top Offset is applied and is relative to the Top height selection in the above drop-down list.
Bottom height determines the final machining height/depth and the lowest depth that the tool descends into the stock. Bottom height needs to be set below the Top. Bottom height is used together with the subsequent offset to establish the height.
Bottom Height
Bottom Offset is applied and is relative to the Bottom height selection in the above drop-down list.
The tolerance used when linearizing geometry such as splines and ellipses. The tolerance is taken as the maximum chord distance.
Loose Tolerance .100 | Tight Tolerance .001 |
CNC machine contouring motion is controlled using line G1 and arc G2 G3 commands. To accommodate this, Fusion approximates spline and surface toolpaths by linearizing them creating many short line segments to approximate the desired shape. How accurately the toolpath matches the desired shape depends largely on the number of lines used. More lines result in a toolpath that more closely approximates the nominal shape of the spline or surface.
Data Starving
It is tempting to always use very tight tolerances, but there are trade-offs including longer toolpath calculation times, large G-code files, and very short line moves. The first two are not much of a problem because Fusion calculates very quickly, and most modern controls have at least 1MB of RAM. However, short line moves, coupled with high feedrates, may result in a phenomenon known as data starving.
Data starving occurs when the control becomes so overwhelmed with data that it cannot keep up. CNC controls can only process a finite number of lines of code (blocks) per second. That can be as few as 40 blocks/second on older machines and 1,000 blocks/second or more on a newer machine like the Haas Automation control. Short line moves and high feedrates can force the processing rate beyond what the control can handle. When that happens, the machine must pause after each move and wait for the next servo command from the control.
Used to offset the center of the tool from the generated toolpath, by the specified distance.
Dark Blue = Original path.
Light Blue = Offset path.
Changes how the selected contours are blended together.
Simple: Best when the selected chains have an equal number of segments. |
Closest: Finds the closest distance between the selected chains. |
The distance to extend the passes beyond the machining boundary.
When selected this allows you to specify a Stepover distance per cut.
Specifies horizontal stepover between passes. By default, this value is 50% of the cutter diameter less the tool corner radius.
Horizontal stepover
Allows you to adjust the number of cuts to create between the selected curves.
|
Allows you to specify the number of cuts to create between the selected curves.
The direction option lets you control if Fusion should attempt to maintain either Climb or Conventional milling.
Climb
Select Climb to machine all the passes in a single direction. When this method is used, Fusion attempts to use climb milling relative to the selected boundaries.
Conventional
This reverses the direction of the toolpath compared to the Climb setting to generate a conventional milling toolpath.
Both Ways
When Both ways is selected, Fusion disregards the machining direction and links passes with the directions that result in the shortest toolpath.
Climb |
Both Ways |
Enable to do multiple depth cuts.
Multiple Depths are used to create multiple incremental Z offset passes in many of the 3D finishing strategies and are useful for removing a fixed amount of stock using several passes. The following images are shown with 3D Parallel.
Disabled |
Three stepdowns |
Specifies the distance for the maximum stepdown between Z-levels. The maximum stepdown is applied to the full depth, less any remaining stock and finish pass amounts.
Specifies the desired number of stepdowns.
Specifies that the passes should be ordered top down.
Disabled |
Enabled |
Use this option to break each pass into segments so that each piece is machined using either downward or upward moves only. This is useful when using insert cutters that are restricted to a specific cutting direction.
Both |
Down Milling |
Positive Stock to Leave - The amount of stock left after an operation to be removed by subsequent roughing or finishing operations. For roughing operations, the default is to leave a small amount of material.
No Stock to Leave - Remove all excess material up to the selected geometry.
Negative Stock to Leave - Removes material beyond the part surface or boundary. This technique is often used in Electrode Machining to allow for a spark gap, or to meet tolerance requirements of a part.
Positive |
None |
Negative |
The Radial Stock to Leave parameter controls the amount of material to leave in the radial (perpendicular to the tool axis) direction, i.e. at the side of the tool.
Radial stock to leave |
Radial and axial stock to leave |
Specifying a positive radial stock to leave results in material being left on the vertical walls and steep areas of the part.
For surfaces that are not exactly vertical, Fusion interpolates between the axial (floor) and radial stock to leave values, so the stock left in the radial direction on these surfaces might be different from the specified value, depending on surface slope and the axial stock to leave value.
Changing the radial stock to leave automatically sets the axial stock to leave to the same amount, unless you manually enter the axial stock to leave.
For finishing operations, the default value is 0 mm / 0 in, i.e. no material is left.
For roughing operations, the default is to leave a small amount of material that can then be removed later by one or more finishing operations.
Negative stock to leave
When using a negative stock to leave, the machining operation removes more material from your stock than your model shape. This can be used to machine electrodes with a spark gap, where the size of the spark gap is equal to the negative stock to leave.
Both the radial and axial stock to leave can be negative numbers. However, the negative radial stock to leave must be less than the tool radius.
When using a ball or radius cutter with a negative radial stock to leave that is greater than the corner radius, the negative axial stock to leave must be less than or equal to the corner radius.
The Axial Stock to Leave parameter controls the amount of material to leave in the axial (along the Z-axis) direction, i.e. at the end of the tool.
Axial stock to leave |
Both radial and axial stock to leave |
Specifying a positive axial stock to leave results in material being left on the shallow areas of the part.
For surfaces that are not exactly horizontal, Fusion interpolates between the axial and radial (wall) stock to leave values, so the stock left in the axial direction on these surfaces might be different from the specified value depending on surface slope and the radial stock to leave value.
Changing the radial stock to leave automatically sets the axial stock to leave to the same amount, unless you manually enter the axial stock to leave.
For finishing operations, the default value is 0 mm / 0 in, i.e. no material is left.
For roughing operations, the default is to leave a small amount of material that can then be removed later by one or more finishing operations.
Negative stock to leave
When using a negative stock to leave the machining operation removes more material from your stock than your model shape. This can be used to machine electrodes with a spark gap, where the size of the spark gap is equal to the negative stock to leave.
Both the radial and axial stock to leave can be negative numbers. However, when using a ball or radius cutter with a negative radial stock to leave that is greater than the corner radius, the negative axial stock to leave must be less than or equal to the corner radius.
Enable to enter a fillet radius.
Specify a fillet radius.
Smooths the toolpath by removing excessive points and fitting arcs where possible within the given filtering tolerance.
Smoothing Off | Smoothing On |
Smoothing is used to reduce code size without sacrificing accuracy. Smoothing works by replacing collinear lines with one line and tangent arcs to replace multiple lines in curved areas.
The effects of smoothing can be dramatic. G-code file size may be reduced by as much as 50% or more. The machine will run faster and more smoothly and surface finish improves. The amount of code reduction depends on how well the toolpath lends itself to smoothing. Toolpaths that lay primarily in a major plane (XY, XZ, YZ), like parallel paths, filter well. Those that do not, such as 3D Scallop, are reduced less.
Specifies the smoothing filter tolerance.
Smoothing works best when the tolerance (the accuracy with which the original linearized path is generated) is equal to or greater than the Smoothing (line arc fitting) tolerance.
Specifies that the feed should be reduced at corners.
Specifies the maximum angular change allowed before the feedrate is reduced.
Specifies the minimum radius allowed before the feed is reduced.
Specifies the distance to reduce the feed before a corner.
Specifies the reduced feedrate to be used at corners.
Enable to only reduce the feedrate on inner corners.
Controls how the tool moves between cutting passes. The following images are shown using the Flow strategy.
Full retraction - completely retracts the tool to the Retract Height at the end of the pass before moving above the start of the next pass.
Minimum retraction - moves straight up to the lowest height where the tool clears the workpiece, plus any specified safe distance.
Shortest path - moves the tool the shortest possible distance in a straight line between paths.
For CNC machines that do not support linearized rapid moves, the post processor can be modified to convert all G0 moves to high-feed G1 moves. Contact technical support for more information or instructions how to modify post processors as described.
Specifies when rapid movements should be output as true rapids (G0) and when they should be output as high feedrate movements (G1).
This parameter is usually set to avoid collisions at rapids on machines which perform "dog-leg" movements at rapid.
The feedrate to use for rapids movements output as G1 instead of G0.
When enabled, retracts are done as rapid movements (G0). Disable to force retracts at lead-out feedrate.
Minimum distance between the tool and the part surfaces during retract moves. The distance is measured after stock to leave has been applied, so if a negative stock to leave is used, special care should be taken to ensure that safe distance is large enough to prevent any collisions.
Specifies the maximum distance allowed for stay-down moves.
1" Maximum stay-down distance |
2" Maximum stay-down distance |
Specifies the radius for horizontal lead-in moves.
Horizontal lead-in radius
The radius of the vertical arc smoothing the entry move as it goes from the entry move to the toolpath itself.
Vertical lead-in radius
Specifies the radius for horizontal lead-out moves.
Horizontal lead-out radius
Specifies the radius of the vertical lead-out.
Vertical lead-out radius