Morph reference

morph strategy

Manufacture > Milling > 3D > Morph morph icon

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.

morph open chains example morph open chains example

morph closed chains example morph closed chains example

tool tab icon Tool tab settings

3d morph dialog tool tab

Coolant

Select the type of coolant used with the machine tool. Not all types will work with all machine postprocessors.

Feed & Speed

Spindle and Feedrate cutting parameters.

Shaft & Holder

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.

Shaft and Holder Modes

Settings

geometry tab icon Geometry tab settings

3d morph dialog geometry tab

Curve Selection

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.

morph open chains example morph open chains example

morph closed chains example morph closed chains example

Machining Boundary

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.

Tool Containment

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.

Additional Offset

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.

Contact Point Boundary

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

Contact Only

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

Slope

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

From Slope Angle is defined from the 0° (horizontal) plane. Only areas equal to or greater than this value are machined.

To Slope Angle

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°

Rest Machining

When checked this limits the operation to only remove material that a previous tool or operation could not remove.

Rest stands for REmaining STock.

  1. Area to Machine - Pocket shown in green.
  2. Previous Operation - Not all stock is removed.
  3. Rest Machining Off - All areas are machined.
  4. Rest Machining On - Previously un-cut areas are machined.

Source

Specifies the source from which the rest machining is to be calculated.

From Setup Stock

Uses the stock body as defined in the Setup

Tool Diameter

Specifies the diameter of the rest material tool.

Ignore Stock Less Than

Specifies the amount of stock from previous operations to ignore. Expressed in distance units. The parameter helps you avoid machining of minor rest material.

Tool Orientation

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:

Model

Enable to override the model geometry (surfaces/bodies) defined in the setup. You can select a different model to apply the toolpath.

Include Setup Model

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.

Avoid/Touch Surfaces

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.

Avoid/Touch Surface Clearance

The amount of clearance between the machined surfaces and the selected surfaces.

Touch 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 diagram

Touch surfaces

heights tab icon Heights tab settings

3d morph dialog heights tab

Clearance Height

The Clearance height is the first height the tool rapids to on its way to the start of the tool path.

clearance height diagram

Clearance Height

Clearance Height Offset

The Clearance Height Offset is applied and is relative to the Clearance height selection in the above drop-down list.

Retract Height

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 diagram

Retract Height

Retract Height Offset

Retract Height Offset is applied and is relative to the Retract height selection in the above drop-down list.

Top Height

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 diagram

Top Height

Top Offset

Top Offset is applied and is relative to the Top height selection in the above drop-down list.

Bottom Height

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 diagram Bottom Height

Bottom Offset

Bottom Offset is applied and is relative to the Bottom height selection in the above drop-down list.

passes tab icon Passes tab settings

3d morph dialog passes tab

Tolerance

The tolerance used when linearizing geometry such as splines and ellipses. The tolerance is taken as the maximum chord distance.

   
tolerance loose tolerance tight
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.

Contour Offset

Used to offset the center of the tool from the generated toolpath, by the specified distance.

contour offset

Dark Blue = Original path.

Light Blue = Offset path.

Morph Mode

Changes how the selected contours are blended together.

     
morph mode simple   morph mode closest
Simple:

Best when the selected chains have an equal number of segments.		   Closest:

Finds the closest distance between the selected chains.

Pass Extension

The distance to extend the passes beyond the machining boundary.

pass extension diagram

Use Stepover

When selected this allows you to specify a Stepover distance per cut.

Stepover

Specifies horizontal stepover between passes. By default, this value is 50% of the cutter diameter less the tool corner radius.

horizontal stepover diagram Horizontal stepover

Number of Offset Stepovers

Allows you to adjust the number of cuts to create between the selected curves.

  1. Selected containment curves.
  2. Zero Offset Stepovers.
  3. 2 Offset Stepovers - Cuts reduced
  4. -2 Offset Stepovers - Cuts extended

Number of Stepovers

Allows you to specify the number of cuts to create between the selected curves.

Direction

The direction option lets you control if Fusion should attempt to maintain either Climb or Conventional milling.

Related: Depending on the geometry, it is not always possible to maintain climb or conventional milling throughout the entire toolpath.

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

Multiple Depths

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

Maximum Stepdown

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.

stepdown max

Number of Stepdowns

Specifies the desired number of stepdowns.

Order by Depth

Specifies that the passes should be ordered top down.

Disabled

Enabled

Up/Down Milling

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

Stock to Leave

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

Radial (wall) Stock to Leave

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.

Axial (floor) Stock to Leave

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.

Fillets

Enable to enter a fillet radius.

Fillet Radius

Specify a fillet radius.

Smoothing

Smooths the toolpath by removing excessive points and fitting arcs where possible within the given filtering tolerance.

   
smoothing off smoothing on
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.

Smoothing Tolerance

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.

Note: Total tolerance, or the distance the toolpath can stray from the ideal spline or surface shape, is the sum of the cut Tolerance and Smoothing Tolerance. For example, setting a cut Tolerance of .0004 in and Smoothing Tolerance of .0004 in means the toolpath can vary from the original spline or surface by as much as .0008 in from the ideal path.

Feed Optimization

Specifies that the feed should be reduced at corners.

Maximum Directional Change

Specifies the maximum angular change allowed before the feedrate is reduced.

Reduced Feed Radius

Specifies the minimum radius allowed before the feed is reduced.

Reduced Feed Distance

Specifies the distance to reduce the feed before a corner.

Reduced Feedrate

Specifies the reduced feedrate to be used at corners.

Only Inner Corners

Enable to only reduce the feedrate on inner corners.

linking tab icon Linking tab settings

3d morph dialog linking tab

Retraction Policy

Controls how the tool moves between cutting passes. The following images are shown using the Flow strategy.

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.

High Feedrate Mode

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.

High Feedrate

The feedrate to use for rapids movements output as G1 instead of G0.

Allow Rapid Retract

When enabled, retracts are done as rapid movements (G0). Disable to force retracts at lead-out feedrate.

Safe Distance

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.

Maximum Stay-Down Distance

Specifies the maximum distance allowed for stay-down moves.

1" Maximum stay-down distance

2" Maximum stay-down distance

Horizontal Lead-In Radius

Specifies the radius for horizontal lead-in moves.

entry radius diagram

Horizontal lead-in radius

Vertical Lead-In Radius

The radius of the vertical arc smoothing the entry move as it goes from the entry move to the toolpath itself.

entry radius diagram - vertical

Vertical lead-in radius

Horizontal Lead-Out Radius

Specifies the radius for horizontal lead-out moves.

exit radius diagram

Horizontal lead-out radius

Vertical Lead-Out Radius

Specifies the radius of the vertical lead-out.

exit radius diagram - vertical

Vertical lead-out radius

Parent page: Morph milling strategy