Adaptive Clearing



Access:

Ribbon: CAM tab 3D Milling panel Adaptive

Adaptive Clearing is a roughing strategy available for clearing large quantities of material effectively. It is unique in that it guarantees a maximum tool load at all stages of the machining cycle, and makes it possible to cut deep and with the flank of the tool without risk of breakage.

The strategy first makes a series of constant Z-layers through the part, and then clears them in stages from the bottom upwards. Because it can cut so deeply, the first step down at each stage should be the effective cutting length of the tool. Then clearing of the intermediate layers proceeds into the shallower layers to maximize the efficiency of the tool use.

This strategy is extremely effective for machining cores because it uses the shape of the original stock to maximum effect when machining from the outside inwards towards the finished shape of the part.

Adaptive Clearing can also be used to great effect for rest machining where a previous larger tool has removed the majority of the material, but a smaller tool is necessary for accessing the finer details. When a previous toolpath is selected, this strategy takes account of the state of the stock after the selected machining operations and limits itself to the yet non-machined areas.



Retract levels in an Adaptive Clearing toolpath. The numbers indicate the order in which the Z levels are machined.

Guidelines for Cutting Conditions

Steel

The depth of a cut can be the same as the tool's flute length; up to 20% of the tool diameter can be used for sideways step.

Hardened steel

The depth of cut can be up to the tool's flute length, and sideways step should be limited to 5% of the tool diameter.

Aluminum

The depth of cut is recommended to be 1.5 to 2 times the tool diameter (but can be up to the flute length). A sideways step of 30% of the tool diameter is recommended, and up to 50% of the tool diameter is in some circumstances achievable.

These values are for cutters suited for roughing. Multi flute cutters should only be set to half or less of the above sideways steps.

Tool tab settings



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 using a tool with a holder, you can choose between one of five different shaft and holder modes, depending on the machining strategy. Collision handling can be done for both the tool shaft and holder, and they can be given separate clearances.

Use shaft

Specifies that the shaft of the selected tool will be used in the toolpath calculation to avoid collisions.

Shaft clearance:

The tool shaft always stays this distance from the part.

Use holder

Specifies that the holder of the selected tool will be used in the toolpath calculation to avoid collisions.

Holder clearance:

The tool holder always stays this distance from the part.

Geometry tab settings



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.

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

File:

Specifies the rest material file.

Adjustment:

Selects the rest material adjustment for respectively ignoring or ensuring milling of small cusps.

Adjustment offset:

This parameter specifies the amount of stock to be ignored, or additionally removed, depending on the Rest Material Adjustment setting. The parameter is primarily used to avoid machining of minor rest material with the Ignore cusps setting.

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.

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 check box, then the toolpath is generated only on the surfaces selected in the operation.

Heights tab settings



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

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

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

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

Bottom offset:

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

Passes tab settings



Tolerance

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, CAM 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 Inventor CAM 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.

Machine shallow areas

Specifies that additional Z-levels should be cuts at shallow areas. The following two images are shown with 3D Contour.


Disabled



Enabled

Minimum shallow stepdown:

This parameter controls the minimum allowed stepdown between the extra Z-levels. This parameter takes precedence over the maximum shallow stepover.

Maximum shallow stepover:

This parameter controls the stepover used to detect areas where extra Z-levels should be inserted. If the normal stepdown results in a stepover of more than this value extra levels will be inserted until the stepover or the minimum stepdown is reached.

Optimal load:

Specifies the amount of engagement the adaptive strategies should maintain.

Note: Legacy clearing toolpaths produce uneven cutter engagement throughout the clearing operation. Using an Adaptive Clearing strategy results in 40% faster material removal rates because larger depth cuts can be taken with full confidence that the cutter will never see spikes in tool engagement that would break cutters.


High Speed Clearing Toolpath



Legacy Clearing Toolpath

Minimum cutting radius:



With Minimum cutting radius set

Sharp corners in the toolpath are avoided minimizing chatter in finished parts.



Without Minimum cutting radius set

The toolpath attempts to remove material anywhere the selected tool can reach. This produces sharp corners in the toolpath that often leads to chatter in the machined part.

Note: Setting this parameter leaves more material in internal corners requiring subsequent rest machining operations with a smaller tool.

Machine cavities

Enable to machine on the inside of the selected closed contours.

Disable to machine on the outside of the selected closed contours.

Open contours may only be specified when this option is enabled.



Machine cavities enabled



Machine cavities disabled

Use slot clearing

Enable this setting to start pocket clearing with a slot along its middle, before continuing with a spiral motion towards the pocket wall.

This feature can be used to reduce linking motion at corners for some pockets.



Use slot clearing enabled



Use slot clearing disabled

Slot clearing width:

The width of the initial clearing slot along the middle of the pocket before continuing with a spiral motion towards the pocket wall.



Slot clearing width

Direction:

The Direction option lets you control if Inventor CAM should try to maintain either Climb or Conventional milling.

Remember: 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, Inventor CAM 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.



Climb



Conventional

Maximum roughing stepdown:

Specifies the maximum stepdown between Z-levels for roughing.



Maximum Stepdown - shown without Finishing Stepdowns

Note: Sequential Z-level stepdowns are taken at the Maximum stepdown value. The Final Roughing stepdown takes the remaining stock, once the remaining stock is less than the Maximum stepdown value.

Fine stepdown:

Specifies the fine stepdown for intermediate steps. These steps are upwards in the direction of the tool axis.

Flat area detection

If enabled, the strategy attempts to detect the heights of flat areas and peaks, and machine at these levels.

If disabled, the strategy machines at exactly the specified stepdowns.

Caution: Enabling this feature may increase calculation time considerably.

Minimum stepdown:

Used when detecting flat areas. This is the smallest allowable stepdown to make.

Minimum axial engagement:

Enable to ensure that at least one flute is constantly engaged as it turns during the intermediate steps to avoid chatter and reduce tool wear.

Attention: Skipping intermediate steps will leave extra stock for the semi-roughing operation that follows.

Order by Depth

Specifies that the passes should be ordered top down.



Disabled



Enabled

Order by area

Toolpaths are ordered by area rather than by depth.

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, Inventor CAM 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, Inventor CAM 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 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 settings



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.

Maximum Stay-Down Distance

Specifies the maximum distance allowed for stay-down moves.



1" Maximum stay-down distance



2" Maximum stay-down distance

Stay-down level:

Use this setting to control when to stay down rather than doing retracts when moving around obstacles. Generally, you will want the Adaptive strategy to stay-down more if your CNC machine does slow retracts compared to high feed moves. In such cases, increase the level value in the Stay-down level: drop-down menu. Values increase by increments of 10% with the Least setting at 0% and the Most setting at 100%.

Remember: Keep in mind that calculation time can increase significantly as you increase the stay-down level.

Lift height:

Specifies the lift distance during repositioning moves.



Lift height 0



Lift height .1 in

No-engagement feedrate:

Specifies the feedrate used for movements where the tool is not in engagement on the material, but is also not retracted.

Horizontal lead-in and lead-out radius:

Specifies the radius for horizontal lead-in and lead-out moves.



Horizontal lead-in radius



Horizontal lead-out radius

Vertical lead-in and lead-out radius:

The vertical arc smoothing radius it goes from the entry move onto the toolpath and off of the toolpath.



Vertical lead-in radius



Vertical lead-out radius

Ramp type:

Specifies how the cutter moves down for each depth cut.



Predrill

Note: To use the Predrill option, Predrill location(s) must be defined.


Plunge



Helix

Ramping Angle (deg)

Specifies the maximum ramping angle of the helix during the cut.

Ramp Taper Angle

Creates a conical helix entry into the part. Excellent for chip clearance.

Ramp Clearance Height

The Height above the stock where the helix start its ramping move.

Helical Ramp Diameter

The maximum diameter to use for a helical entry into the cavity.

An optimal value causes the tool to overlap it's center, while still creating the maximum helical bore for the entry into the cavity. The goal is for good chip evacuation. If the value is bigger than the diameter of the tool it can leave a boss standing in the center of the helix.

Value of 1.8 x the Dia.

Value of 0.8 x the Dia.

Minimum Ramp Diameter

The smallest Helix Ramp Diameter that is acceptable.

This value should always be smaller than the Helix Ramp Diameter, so the system can calculate a range that fits the available pocket or channel. Smaller diameters can reduce the chip evacuation, create jerking machine motion and can cause tool breakage.

Predrill positions

Select points where holes have been drilled to provide clearance for the cutter to enter the material.

Entry positions

Select geometry near the location where you want the tool to enter.

Topics in this section
Parent topic: 3D Milling Functionality