Access: |
Ribbon:
CAM tab
![]() ![]() ![]() |
An Adaptive Clearing strategy creates a toolpath from chained contours rather than surfaces or solids. It is possible to define a taper angle for the walls.
The type of coolant used with the tool.
The rotational speed of the spindle.
The spindle speed expressed as the speed of the tool on the surface.
The rotational speed of the spindle when performing ramp movements.
Feed used in cutting moves.
The cutting feedrate expressed as the feed per tooth.
Feed used when leading in to a cutting move.
Feed used when leading out from a cutting move.
Feed used when doing helical ramps into stock.
Feed used when plunging into stock.
The plunge feedrate expressed as the feed per revolution.
Enable to specify the perimeter of the stock that needs to be faced.
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:
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, 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 HSM 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.
Specifies the amount of engagement the adaptive strategies should maintain.
High Speed clearing toolpath
Legacy clearing toolpath
With Minimum cutting radius set
With Minimum cutting radius set - Sharp corners in the toolpath are avoided minimizing chatter in finished parts.
Without Minimum cutting radius set
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.
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
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
The Direction option lets you control if Inventor HSM should try to maintain either Climb or Conventional milling.
Climb
Select Climb to machine all the passes in a single direction. When this method is used, Inventor HSM attempts to use climb milling relative to the selected boundaries.
Climb
Conventional
This reverses the direction of the toolpath compared to the Climb setting to generate a conventional milling toolpath.
Conventional
Specifies that multiple depths should be taken.
With Multiple Depth cuts
Without Multiple Depth cuts
Specifies the maximum stepdown between Z-levels for roughing.
Maximum stepdown - shown without finishing stepdowns
Specifies that the passes should be ordered top down.
Disabled
Enabled
Positive
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.
None
No Stock to Leave - Remove all excess material up to the selected geometry.
Negative
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.
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 HSM 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, Inventor HSM 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.
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.
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 "dogleg" 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.
Specifies the maximum distance allowed for stay-down moves.
1" Maximum stay-down
2" Maximum stay-down distance
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%.
Specifies the lift distance during repositioning moves.
Lift height 0
Lift height .1 in
Specifies the feedrate used for movements where the tool is not in engagement on the material, but is also not retracted.
Specifies the radius for horizontal lead-in moves.
Horizontal lead-in radius
Specifies the radius for horizontal lead-out moves.
Horizontal lead-out 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 of the vertical lead-out.
Vertical lead-out radius
Specifies how the cutter moves down for each depth cut.
Plunge Outside Stock
Predrill
To use the Predrill option, Predrill location(s) must be defined.
Plunge
Zig-Zag
Notice the smooth transitions on the Zig-Zag ramp type.
Profile
Smooth Profile
Helix
Specifies the maximum ramping angle.
The desired taper angle of the helical ramps. Use this setting to keep the tool shaft slightly away from the stock and improve chip escape during ramping.
Height of ramp over the current stock level.
Specifies the helical ramp diameter.
Specifies the minimum ramp diameter.
Select points where holes have been drilled to provide clearance for the cutter to enter the material.
Select geometry near the location where you want the tool to enter.