Multi-Axis Contour



Access:

Ribbon: CAM tab Multi-Axis Milling panel Multi-Axis Contour
Important: This functionality is only available in Inventor HSM Ultimate.

The Multi-Axis Contour strategy for machining is done with the tip of the tool along a given contact curve. By default, the tool is normal to the surface but lead/lag and sideways tilt can be applied, when desired, to control the contact point on the tool. The strategy allows center, left, and right compensation.

Tool tab settings



Coolant:

The type of coolant used with the tool.

Spindle speed:

The rotational speed of the spindle.

Surface speed:

The spindle speed expressed as the speed of the tool on the surface.

Ramp spindle speed:

The rotational speed of the spindle when performing ramp movements.

Cutting feedrate:

Feed used in cutting moves.

Feed per tooth:

The cutting feedrate expressed as the feed per tooth.

Lead-in feedrate:

Feed used when leading in to a cutting move.

Lead-out feedrate:

Feed used when leading out from a cutting move.

Ramp feedrate:

Feed used when doing helical ramps into stock.

Plunge feedrate:

Feed used when plunging into stock.

Feed per revolution:

The plunge feedrate expressed as the feed per revolution.

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



Curve selections

Selection button to choose the faces to be machined.

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.

Passes tab settings



Tolerance:

The machining tolerance is the sum of the tolerances used for toolpath generation and geometry triangulation. Any additional filtering tolerances must be added to this tolerance to get the total tolerance.



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.

Cutting mode:

The cutting mode specifies how to machine along a given contact curve.

Sideways compensation:

Specifies the compensation direction.

Repeat finishing pass

Enable to perform the final finishing pass twice to remove stock left due to tool deflection.

Tangential fragment extension distance:

Specifies the tangential extension of the passes.

Axial offset:

Specifies an axial offset value for the toolpath for the chosen contour.

Pass overlap:

Specifies the distance to extend machining for a closed pass.

Maximum fan distance:

Specifies the maximum distance over which to fan the tool axis.

Forward tilt:

Specifies the number of degrees the tool should be tilted forward.

Sideways tilt:

Specifies the number of degrees the tool should be tilted sideways.

Minimum tilt:

Specifies the minimum allowed tilt from the selected operation tool axis.

Maximum tilt:

Specifies the maximum allowed tilt from the selected operation tool axis.

Maximum segment length:

Specifies the maximum length of a single segment for the generated toolpath.

Maximum tool axis sweep:

Specifies the maximum angle change in a single tool axis sweep for the generated toolpath.

Stock to Leave



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.

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.

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.

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

Lead-in radius:

Specifies the radius for lead-in moves.



Lead-in radius

Lead-out radius:

Specifies the radius for lead-out moves.



Lead-out radius

Transition type:

Specifies the type of connection done between passes.

Entry positions

Selection button to choose entry positions.