The Contour strategy is designed to give you an optimal finish for steep regions in your geometry. It is typically applied to areas where the slope exceeds an angle of 30 degrees. The Contour algorithm virtually slices the geometry into horizontal layers. At every layer, the toolpath then machines along the edge of the two-dimensional geometry thus created. You can control the vertical distance between the toolpath layers with the stepdown parameter.
In addition, to traditional Contour cuts at constant depth, HSM Performance Pack supports the so-called spiral Contour, which continuously ramps down along the geometry. This completely removes transition marks from the surface of the final part.
As with all strategies in HSM Performance Pack, Contour is optimized for High Speed Machining by assuring maximum smoothness of the toolpath in particular at sharp corners of the geometry.
Full Control Over all Parameters
You can control exactly in which region of your geometry the Contour strategy should be applied by selecting a range of slope angles. Furthermore, Contour supports rest machining such that you only machine regions which were not machined by previous operations. You can freely configure the lead-in and lead-out moves of the operation. HSM Performance Pack generates lead arcs with optimal smoothness to minimize the tool wear. In addition, both the ramping and linking moves are freely configurable to match your tool, machine and part.
In the large area, the tool is selected, or a new tool can be created from the right click menu. The fields below are automatically updated from the tool selected above. The tool drawing to the right is updated each time a field is exited, to reflect the changed value. The right click menu is also used to access the HSM tool library, described below.
The flute length doesn't have an effect on the shape of the cutter paths unless a taper angle is applied. Tapered tools add the shape of a cone of the given taper angle from the vertical axis. The bottom of the (truncated) cone is tangential to the shape at the tip, and the top is at the flute length above the tip. For tapered tools, the tool definition is straightforward for ball nosed and flat bottomed tips, but for bull nosed tips the standard convention is more complicated: the shaft diameter refers to the diameter of the bottom of the conical surface and not the diameter of the virtual toroidal shape that would be within the tapered shape.
In the section Shaft and holder you can define holder and shaft collision checks and how the toolpath should respond to detected collisions. In particular, this is where you can define to tilt the tool in case of a collision, effectively creating a 5-Axis toolpath.
Note that these collision checks require additional calculation time when the toolpath is generated, but ensures that the shaft and holder do not collide with the part if used.
The following parameters can be set to control the collision detection (note that not all parameters are available for all strategies):
Collision detection policy
The dropdown menu lets you select how HSM Performance Pack should react to a detected holder collision. The following options are available (depending on the selected strategy):
With the option Ignore, collisions between the shoulder, shank, holder and the work piece are ignored.
When the trimming option is selected, toolpath will be trimmed away in areas of holder collisions.
Tilt to avoid collision
With this option, the tool is tilted far enough so that it can make the cut without having the holder collide with the part. Only toolpath with a ball nose mill can be tilted. This mode is supported for finishing strategies.
In the pull away mode, the kernel avoids shoulder/shank/holder collisions with the part by moving the tool away from the surface. It is important to notice that some stock might not be machined in this case and the toolpath may contain some air cuts. This mode is very useful when the “undercut” option is enabled for 3D Contour or Horizontal as it helps to avoid trimming and ensures that as much of the part as possible is machined.
With the option detect lenght, HSM Performance Pack checks toolpath and suggests a flute length to the user for which any holder collisions are avoided.
A warning such as the following will be provided to suggest a tool:
“Warning: Tool flute must be increased by 53.04 to avoid holder gouge.”
Fail on collision
With the option fail on collision, the toolpath generation fails in case the software detects a holder collision.
The following is an example error which is provided to help the user in removing the gouge:
“Error: Holder Gouge detected at point (37.7439,-57.5288,0), tool axis: (0,0,1), linking path #102”
The Holder clearance defines the safety distance between the holder and the stock. If the holder gets closer to the part (or stock) than this distance, it will be treated as a collision.
The Shank clearance defines the safety distance between the shank and the stock. If the shank gets closer to the part (or stock) than this distance, it will be treated as a collision.
The tilt angle is the angle at which the tool will be tilted at the beginning of the toolpath.
Tilt angle deviation +/-
The option tilt angle deviation +/- allows you to set the maximum allowed tilt angle in both directions away from the the vertical position.
Max segment length
Specifies maximum allowed distance between neighboring points in toolpath after tilt.
Max axis change
Specifies maximum allowed tool axis change between neighboring points in toolpath after tilt.
Specify the smoothing distance that should be applied in the tilt algorithm. Bigger value provide smother toolpath after tilt.
The Clearance height defines the first height to which the tool moves before the start of the toolpath. The height is relative to the top of the surface to be machined.
The field Absolute clearance height can be enabled to define an absolute Z value instead.
The Retract height defines the height to which the tool retracts between cutting passes. The linking moves at this height are carried out at rapid speed. The height is relative to the top of the surface to be machined.
The field Absolute retract height can be enabled to define an absolute Z value instead.
The Safe distance defines the minimum distance between the tool and the part surfaces during shortest path retract moves. This distance is measured after the stock to leave has been applied, so if a negative stock to leave is used, special care should be taken that the safe distance is large enough to ensure that no collisions occur.
The Retraction policy determines how moves between cutting passes are done. Shortest path is the shortest possible path (which often includes moves in all three axes), Minimum retraction is straight up to the lowest height where the tool will be clear of the part (by safe Z distance), and Full retraction is to the clearance plane.
Allow rapid retract
By enabling Allow rapid retract, vertical retract moves will be carried out at rapid speed. If this is not enabled, retracts will be carried out at the lead-out feedrate.
Explicit lead out
By enabling Explicit lead out you can define the lead out parameters independently from the lead in parameters. If not enabled, the lead out parameters will be identical to the lead in parameters.
By enabling Perpendicular lead you can define that a movement which is perpendicular to the lead-in/out arc should replace tangential extensions of arcs.
Perpendicular lead out
By enabling Perpendicular lead out you can define that a movement which is perpendicular to the lead out arc should replace tangential extensions of arcs.
Vertical lead radius
A lead-in or out movement generally consist of three components. The horizontal lead-in/out arcs which is located in the perpendicular plane to the tool start axis and leading smoothly into or away from the toolpath, followed by a linear segment in the same plane, and a vertical arc connecting the linear segment with the retract movement.
Vertical lead radius defines the radius of the vertical arc component of the lead-in/out movement. The radius can be specified as a percentage of the tool diameter or as an absolute value.
Vertical lead out radius
Vertical lead out radius defines the radius of the vertical arc component of the lead-out movement. The radius can be specified as a percentage of the tool diameter or as an absolute value. You need to enable Explicit lead out in order to specify a separate vertical lead out radius. Otherwise, the same radius will be used for lead-in and lead-out.
Horizontal lead radius
Horizontal lead radius defines the radius of the horizontal arc component of the lead-in/out movement. The radius can be specified as a percentage of the tool diameter or as an absolute value.
Horizontal lead out radius
Horizontal lead out radius defines the radius of the horizontal arc component of the lead out movement. The radius can be specified as a percentage of the tool diameter or as an absolute value. You need to enable Explicit lead out in order to specify a separate horizontal lead out radius. Otherwise, the same radius will be used for lead-in and lead-out.
Sweep defines the sweep angle between the linear segment component of the lead-in/out movement and the toolpath.
Sweep (lead out)
Sweep (lead out) defines the sweep angle between the linear segment component of the lead out movement and the toolpath. You need to enable Explicit lead out in order to specify a separate lead out sweep angle. Otherwise, the same angle will be used for lead-in and lead-out.
Linear lead distance
Linear lead distance defines the length of the linear segment component of the lead-in/out movement.
Linear lead out distance
Linear lead out distance defines the length of the linear segment component of the lead-in/out movement. You need to enable Explicit lead out in order to specify a separate linear lead out distance. Otherwise, the same distance will be used for lead-in and lead-out.
Keep down distance
The Keep down distance defines a length below which retracts are avoided. This means that lead-in and lead-out moves are still generated below this length, but the tool is only lifted up slightly.
Max transition distance
Use the parameter Max transition distance to define a maximum allowed length for transitions between cutting passes. If the distance between two passes is greater than the Max transition distance, the tool retracts or is lifted up and a lead-out and lead-in are generated.
Transition on surface
Activate the checkbox transition on surface to force the transitions to stay on the surface of the part. If the checkbox is not checked, the transitions will slightly move away from the geometry in order to avoid transition marks on the part. This option is available when curve or straight line transitions are used.
Allow 3D leads
Activate the option allow 3D leads to allow for lead-in and lead-out motions in 3D. This option is available when the contact ramp policy is set to loop.
Contact ramp policy
From the dropdown menu contact ramp policy you can select the method by which ramps should be carried out between different cutting depths. The available options are:
Straight line: This defines that the transitions are simple straight lines between two cutting passes.
Curve: In this mode, the transitions are smooth curves which are tangential to the cutting passes at both ends of the transition.
Loop: This creates a loop away from the surface of the part in order to maintain the machine dynamics when ramping down.
Disabled: This disables transition moves.
Contact ramp angle
The contact ramp angle is the angle which the ramp forms with the cutting passes. A smaller angle means that the ramp into the material is less steep.
Tolerance defines the maximum value the toolpath is allowed to deviate from the surface of the input geometry. A small tolerance value yields more precise toolpaths at the expense of longer computation times.
Minimum cutting radius
The minimum cutting radius is the smallest arc radius with which the tool is allowed to move. This means that sharp corners and tight radii are replaced with arcs of the specified minimum cutting radius. For high-speed toolpaths, it is recommendable to not have sharp corners in the toolpath to prevent peaks in tool engagement which could lead to tool breakage. With a reasonable minimum cutting radius, a smooth toolpath is guaranteed in corners, at the expense that the tool is moved away from corner vertices.
Stock to leave
Stock to leave is the stock to leave in the X/Y plane, i.e. in the plane vertical to the tool direction. Stock to leave offsets the tool away from walls and tilted surfaces by the specified distance.
Axial stock to leave
Axial stock to leave defines the stock to leave in the Z-direction, i.e. in the direction along the tool axis. Axial stock to leave lifts the tool up from the surface by the specified distance.
The stepdown is the maximum vertical distance between two cutting levels. Note that the actual stepdown may be less than the value specified in stepdown. This is because HSM Performance Pack will automatically reduce the stepdown to ensure that cuts are carried out at the minimum depth and maximum depth, and that all Z-level cuts are spaced evenly.
Example of the Stepdown. The Stepdown is indicated by the gab between the two cutting levels (the arrow), which are the two planes with pink paths.
The parameter can be used as a variable in formulas by entering MaximumStepdown.
Use the option allow undercut to perform undercuts, i.e. the tool is allowed to cut under some remaining material. This supported for lollipop, slot and dove tools.
Activate the option spiral to perform the contour operation in one continuous spiral. This means that the toolpath will spiral downwards continuously without any transitions for a superior surface finish. If spiral is not activated the toolpath will be carried out as a traditional contour with constant z-levels.
When fit arcs is selected HSM Performance Pack recreates arcs in the geometry. Arcs are linearized during the triangulation of the geometry prior to the toolpath generation and recreating them ensures that round geometry will be truly treated as round. Fitting arcs ensures a better toolpath smoothness.
Order by depth
When the option order by depth is activated, the cuts are ordered by the depth at which they are carried out. If the option is deactivated, the cuts are ordered by pocket, i.e. a single pocket is milled all the way at different depths before the tool moves to the next pocket.
Order from bottom
Machining will start from the bottom of the part. It is normally used for rest machining to avoid tool moving into chips.
Machine shallow areas
Activate machine shallow areas to add additional cuts in shallow regions of the geometry by dynamically reducing the stepdown in shallow regions.
The minimum stepdown is the smallest possible vertical spacing between two cutting levels. When machine shallow areas is used, the minimum stepdown ensures that HSM Performance Pack does not add extremely narrow cutting levels in almost flat regions of the geometry. HSM Performance Pack tries to ensure a stepover smaller than the stepover, but only as long as the stepdown is bigger than the minimum stepdown.
The stepover is the maximum horizontal spacing between cuts of two next cutting levels. This criterion is used to add additional cutting levels when machine shallow areas is activated: HSM Performance Pack reduces the stepdown to ensure that the stepover does not exceed the stepover. Note that the stepdown will never be reduced to less than the minimum stepdown.
Trim shallow passes
Activate trim shallow passes to trim additional toolpath that was created in steep areas due to the option machine shallow areas. For large parts where there are shallow and steep walls in the same cutting depth, shallow area machining can lead to many excessive cuts in steep areas of the part. Activating trim shallow passes adds additional cuts in shallow areas, whereas cuts in steep areas at the same depth are trimmed away.
With the dropdown menu direction you can specify in which direction the tool will move along the surface. You can select climb milling, conventional milling or both ways.
Climb milling means that the direction of the work piece relative to the tool is in the same direction as the tool rotation.
In conventional milling, the work piece motion relative to the tool is in the opposite direction of the tool rotation.
Selecting both ways specifies that there is no preference between climb and conventional milling. In this case, HSM Performance Pack will choose the cutting direction such that the toolpath length is minimized.
In general climb milling is commonly used since the chips are thrown away from the tool. For conventional milling, they land in front of the tool. Due to this, climb milling leads to better surface finishes and less to wear. However, there may be cases when conventional milling is the better choice due to backlash in climb milling.
Activate confine depth to specify depth limits for the toolpath, useful for machining deep pockets, where the upper areas are to be machined with a shorter tool, and the lower areas with a longer tool.
The minimum depth is the height at which the cuts begin.
The maximum depth is the final cutting depth of the operation.
From slope angle
In the selection box from slope angle you can specify the lower limit of slope angles below which no toolpath will be generated.
To slope angle
In the selection box to slope angle you can specify the upper limit of slope angles above which no toolpath will be generated.
Machine flat areas
Machine flat areas ensures that flat regions in the geometry are machined by adding additional Z-level cuts between the regularly spaced cutting levels. When machine flat areas is not activated, HSM Performance Pack will create the cutting levels with constant spacing.
Instead of machining the flat areas completely, enabling this options generates a single pass exactly above flat area.
Maximum smoothing is an additional horizontal offset of the generated toolpath. This offset is used to smoothen the toolpath by rounding off corners without creating islands in narrow regions.
Using maximum smoothing allows for much faster tool movements since sharp corners are prevented. It may however lead to a longer toolpath since additional passes may be required to compensate for the offset toolpaths.
The minimum stepover is the smallest allowed distance between two horizontal passes. The minimum stepover can be specified as a percentage of the tool diameter or as an absolute value.
The maximum stepover is the largest allowed distance between two horizontal passes. Note that the maximum stepover must be less than the tool diameter to prevent upstands between the passes. The maximum stepover can be specified as a percentage of the tool diameter or as an absolute value.
Example of the Stepover. The Stepover is the distance between two cutting passes, indicated by the arrow.
Rest material source
The dropdown menu rest material source lets you select the method for calculating the rest material to be removed by this operation. The following options are available:
Disabled: Defines that the current operation is not a rest machining operation. Choose this to carry out a regular operation.
Rest material operation: The rest material is calculated as the material left behind by one or more earlier operations. This is the most accurate method to use, as it works from where the tool actually went in the earlier operation, taking into account the space needed for lead in/out motions, as well as any other limitations of the earlier operations. This is also the only way to take more than one operation into account. Due to the increased precision, this method may take longer than other options to calculate. The operations which should be included in the rest material calculation are selected below.
Rest material STL file: The remaining material is calculated from a STL file, defining a pre-roughed or cast part, for example. The STL file must be specified below.
Rest material tool: Uses a theoretical tool to calculate the rest area, left by this tool, and uses it as basis for the rest material calculation. The theoretical tool is specified by its diameter and corner radius.
Rest material operation
Use the dropdown menu rest material operation to select the operation to be used as basis for the rest material calculation. Use the last of the operations if the result of more than one operation is to be used as basis.
Union of all dependent operations
Selecting the option union of all dependent operations will use the selected operation and any operations the selected operation depends on as basis for the rest material calculation.
Include all previous operations
Selecting the option include all dependent operations will use the selected operation and any operations above the selected operation in the operations manager as basis for the rest material calculation.
Only include operations within the same group
Selecting the option only include operations within the same group will use the selected operation and any operation above the selected operation which is in the same toolpath group as the selected operation.
Rest material STL file
Use the field rest material STL file to select the STL file to be used as basis for the rest material calculation. Right click to browse for a file or select it from a “recent files” list.
It is possible to adjust the rest material model for a better result:
Use as computed means no adjustment is used.
Ignore small cusps causes any areas of rest material smaller than the adjustment specified below to be ignored.
The adjustment is the size of the adjustment used when machine small cusps is used.
In the field on the right, all operations for the part created with HSM Performance Pack can be seen. The listing for each operation shows the operation type and the tool used, and can be expanded to also show the comment and stock to leave. The listings for each operation can be expanded or collapsed by clicking the plus or minus sign next to it. By right-clicking on an operation, it is also possible to view (but not change) all parameters for the operation, or expanding or collapsing all operations. When the rest material source is set to rest material operation, then it is possible to select the source operation by right-clicking it here and selecting Select. When the rest material source is set to Rest material tool, then it is possible to fill in the tool shape parameters by right-clicking an operation using the relevant tool, and selecting Fill-in tool parameters.
Click the Add... button to select the specific surfaces that should be machined by this operation.
Click the Add all button to select all surfaces to be machined by this operation.
Click the Remove all button to remove all surfaces from the selection and so they are not machined by this operation.
Boundaries and points
The list Boundaries and points shows the boundaries and points for the operation. Boundaries and points can be added or removed by using the buttons Add boundaries... or Remove all.
The Add boundaries... button allows the user to add one or more points or boundaries to the operation.
The Remove all button removes all boundaries and points from the operation.
The Remove button only removes the selected boundary or point from the operation.
The Manager... button enables you to switch to the Mastercam chain manager, and allows the boundaries or points to be edited there.
Select by entities...
The Select by entities... button changes to the graphics window, where the user can select an entity. The boundary containing that entity (if any) is then selected.
From the dropdown menu type the type of boundary can be selected. The available options are:
The available options for points are:
From the dropdown menu Geometry source, the source of the geometry can be selected. The following options are available:
Use selected geometry
The option Use selected geometry generates the triangulation model for the toolpath generation from the selected geometry.
Use STL file
The option STL file lets you select an STL file which will be used for the toolpath generation. This can be particularly powerful when very large files are used, for which triangulation takes a long time. In this case a pre-generated STL file avoids lengthy re-calcuations. Note however, that it may be dangerous to use an external STL file since this will not automatically reflect any changes made to the CAD model.
The field Size contains the file size of the STL file.
The field Date contains the creation date of the STL file.
Use the field Path to select the location of the STL file in your file system or define where the temporary STL file should be stored.
Geometry tolerance ratio
The Geometry tolerance ratio (%) defines the fraction of the operation tolerance (specified in the toolpath tab) used for generating the STL. The remainder is used for generating the toolpaths from the STL. This setting is ignored when using an external STL file. If the tool is very small, this value should be lowered to ensure that filets are represented correctly by the STL, and for complex parts, it is sometimes possible to reduce the calculation time by reducing this value.
The Invalidate button causes a new STL file to be recalculated at the next regeneration, regardless of the file policy setting.
The Export button exports the current STL file to an external STL file for use in other programs or for comparison in verification.
Use the radio buttons under tool containment to define the which part of the tool should be contained by the defined boundary. The following options are available:
Tool inside boundary
Using this option, the tool will be completely contained within the boundary.
Tool center on boundary
Using this option, the center of the tool will be contained by the boundary.
Tool outside boundary
Using this option, the tool may go over the boundary until the outside of the tool touches the boundary.
The additional offset defines an offset by which the previously defined tool containment is offset from the selected contour.
The fillets tab lets you apply toolpath fillets without the need to add these fillets to the CAD model.
Apply toolpath fillets
Apply toolpath fillets activates the toolpath filleting function. The toolpath filleting function modifies the toolpaths to prevent sharp corners in the toolpath by making the toolpath machine the area where a specified virtual tool would fit, instead of the machining surfaces. This causes fillets to be added at sharp corners and small radii.
The diameter is the diameter of the virtual tool used to calculate the filleting.
The corner radius is the corner radius of the virtual tool used to calculate the filleting.
The toolpath tab contains various parameters which are needed to configure the toolpath and properly execute it on the CNC machine, such as arc filtering and other toolpath filters.
The checkboxes under Arc filtering let you configure in which planes (XY-plane, XZ-plane, YZ-plane or helical arcs) arcs should be output to the machine as actual arcs (i.e. G2/G3), instead of being output as line segments (G1).
The Minimum radius defines the radius below which an arc is output as line segments.
The Maximum radius defines the radius above which an arc is output as line segments.
Minimum chord length
The Minimum chord length defines the arc chord length below which an arc is output as line segments.
The Linearization tolerance is the tolerance used when arcs are to be converted to line segments, either because arcs are disallowed in that plane, or because the arc is too large or too small.
Use the option Arc fitting to fit arcs where it is possible.
Defines the maximum error (distance) of the arc fitting to the geometry.
Rapid filtering defines when rapid moves should be converted to linear moves (G1 in ISO code) at a high feed rate. The following filtering policies are available:
Preserve rapid movement: Rapid moves are always output as rapid moves (G0 in ISO code), even if they are in all three axes simultaneously. This option should only be selected if rapid moves on the machine are synchronized as linear moves.
Preserve Z-axis and XY-plane rapid movement: Rapid moves are output as rapid moves (G0 in ISO code) if they are along the Z axis or in the XY plane, but are converted to linear moves (G1 in ISO code) at a high feed rate if they are in all three axes.
Preserve vertical rapid movement: Rapid moves are output as rapid moves (G0 in ISO code) if they are vertical (i.e. along the Z axis), and are otherwise converted to linear moves (G1 in ISO code) at a high feed rate.
Preserve horizontal rapid movement: Rapid moves are output as rapid moves (G0 in ISO code) if they are horizontal (i.e. in the XY plane), and are otherwise converted to linear moves (G1 in ISO code) at a high feed rate.
Preserve one axis rapid movement: Rapid moves are output as rapid moves (G0 in ISO code) if they are in one axis only, and are otherwise converted to linear moves (G1 in ISO code) at a high feed rate.
Map to high feed cutting: All rapid moves are converted to linear
moves (G1 in ISO code) at a high feed rate.
High feed rate
High feed rate defines the feed rate used when rapid moves (G0 in ISO code) are converted to linear moves (G1 in ISO code).
Depth compensation lets you choose in which way the toolpath should be vertically adjusted to the tool radius. The following options are available:
The output toolpath corresponds to the path of the tool center.
The output toolpath corresponds to the path of the tool tip.
The Settings button opens up the Mastercam dialog for setting the miscellaneous values.
The operation tab lets you define important parameters for the execution of the toolpath on the machine. For example, here you can set the file name of the output NC file, define the working coordinate system, or configure the line numbering of the output file.
In the Title field you can define the name of the operation as it will be displayed in the Operation manager of Mastercam.
The Comment field lets you add an additional description of your machining strategy, and can be used to further document parameters, purpose etc. of the operation.
The field Program number lets you give the output NC program a number.
Sequence start defines the starting line number of the output NC program.
The Sequence increment defines the increments in the line numbering of the output NC program.
In the field NCI path you can define the name and path under which the output file should be saved. Click the icon [...] in the field to browse your file system for a desired directory.
The parameters under Tool view define the tool plane and origin for 5 axis positioning.
You can define the X, Y and Z coordinate of the tool view through the respective fields. Furthermore, you can select the origin and select the tool plane by clicking on the respective buttons.
Working coordinate system
The parameters under Working coordinate system defines the working coordinate system used in the operation.
You can define the X, Y and Z coordinate of the working coordinate system through the respective fields. Furthermore, you can select the origin by clicking on the respective button.