Thread reference

Thread is used for milling threads into a hole or a boss, with straight or tapered walls. Select any internal or external circular face to create single or multi-lead threads. The heights and depths are automatically derived from the selected face.

circular face selection example thread mill sim example

Manufacture > Milling > 2D > Thread

thread mill example

Tool tab settings

2d thread 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.

Spindle Speed - The rotational speed of the spindle expressed in Rotations Per Minute (RPM)
Surface Speed - The speed which the material moves past the cutting edge of the tool (SFM or m/min)
Ramp Spindle Speed - The rotational speed of the spindle when performing ramp movements
Cutting Feedrate - Feedrate used in regular cutting moves. Expressed as Inches/Min (IPM) or MM/Min
Feed per Tooth - The cutting feedrate expressed as the feed per tooth (FPT)
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

Geometry tab settings



Face Selection	Diameter Range Selection

Geometry

You can select Faces or a Diameter Range. Select any internal or external circular Face. Faces can be straight walled or tapered. Use Diameter Range to automatically include or exclude holes or bosses by specifying a minimum and maximum range.

Selection Mode

Select the geometry to machine by Faces or Diameter Range. Heights and depths are automatically derived from the selection.


Circular Face Selection		Diameter Range

Select any internal or external circular Face.		Selects all holes or bosses that fit within a minimum and maximum range.

Feature Type

Used with Diameter Range. Filters the hole selection.


Holes only	Bosses only	Both

Minimum and Maximum Diameter

Set the diameter range for the holes to include.

Minimum - Holes equal to or greater than the specified value are included
Maximum - Holes equal to or less than the specified value are included

Select Same Diameter

Check to select all holes with the same diameter as the currently select feature.

select same diameter example

A single selection will find all matching holes. Using this option is associative to the model. If additional holes with the same diameter are added later, regenerating the operation automatically includes the added holes in the drilling cycle.

Example: If you activate this option, select a single 6mm hole and a single 12mm hole, every 6mm and 12mm hole on the part will automatically be selected.

Only Same Hole Depth

Check to select all the holes that share the same top to bottom distance as the currently select feature.

Example: You can use this as a way to distinguish between 6mm tapped holes and 6mm drilled holes of different depths.


Short Depth 6mm holes selected - ISO view	Short Depth 6mm holes selected - Front view

Long Depth 6mm holes selected - ISO view	Long Depth 6mm holes selected - Front view

Only Same Z Top Height

Check to select all the holes that share the same Z top height as the currently select feature.

You can use this as a way to limit machining to one Z level. The red arrow below indicates the selected feature.


All Short Depth Holes, at the Mid Level Height	All Short Depth Holes, at the Mid Level Height All Long Depth Holes, at the Lower Level Height.

Containment Boundary

Use this with Select Same Diameter to include similar items inside the containment areas. Select any Edge or Sketch boundary to contain the drilling locations. Use multiple boundaries or nested boundaries, to include or exclude groups of holes. The toolpath will be inside the selected boundary unless the boundaries are nested. You can nest several boundaries inside each other.

In the examples below, the selected boundaries are shown in blue.


	1) Sketch Boundaries 2) Holes inside are included 3) Nested Boundaries 4) Inside areas are excluded	5) Sketch Boundaries (2) 6) Selecting the rim area only 7) Sketch Boundaries (3) 8) Excluding the rim area

Order

Specifies how the holes should be ordered for machining.


	1) Order selected 2) Optimized order 3) Inside to Outside 4) Order by X motion 5) Order by Y motoion

Reverse order

Enable to reverse the order of the sorted toolpath.


Disabled	Enabled

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:

Setup WCS orientation - Uses the workpiece coordinate system (WCS) of the current setup for the tool orientation.
Model orientation - Uses the coordinate system (WCS) of the current part for the tool orientation.
Select Z axis/plane & X axis - Select a face or an edge to define the Z axis and another face or edge to define the X axis. Both the Z and X axes can be flipped 180 degrees.
Select Z axis/plane & Y axis - Select a face or an edge to define the Z axis and another face or edge to define the Y axis. Both the Z and Y axes can be flipped 180 degrees.
Select X & Y axes - Select a face or an edge to define the X axis and another face or edge to define the Y axis. Both the X and Y axes can be flipped 180 degrees.
Select coordinate system - Sets a specific tool orientation for this operation from a defined user coordinate system in the model. This uses both the origin and orientation of the existing coordinate system. Use this if your model does not contain a suitable point & plane for your operation.

The Origin drop-down menu offers the following options for locating the triad origin:

Setup WCS origin - Uses the workpiece coordinate system (WCS) origin of the current setup for the tool origin.
Model origin - Uses the coordinate system (WCS) origin of the current part for the tool origin.
Selected point - Select a vertex or an edge for the triad origin.
Stock box point - Select a point on the stock bounding box for the triad origin.
Model box point - Select a point on the model bounding box for the triad origin.

Heights tab settings

2d thread dialog heights tab

Clearance Height

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

clearance height diagram

Clearance Height

Retract height: incremental offset from the Retract Height.
Feed height: incremental offset from the Feed Height.
Top height: incremental offset from the Top Height.
Bottom height: incremental offset from the Bottom Height.
Model top: incremental offset from the Model Top.
Model bottom: incremental offset from the Model Bottom.
Stock top: incremental offset from the Stock Top.
Stock bottom: incremental offset from the Stock Bottom.
Hole top: incremental offset from the Hole Top.
Hole bottom: incremental offset from the Hole Bottom.
Selection: incremental offset from a Point (vertex), Edge or Face selected on the model.
Origin (absolute): absolute offset from the Origin that is defined in either the Setup or in Tool Orientation within the specific operation.

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

Clearance height: incremental offset from the Clearance Height.
Feed height: incremental offset from the Feed Height.
Top height: incremental offset from the Top Height.
Bottom height: incremental offset from the Bottom Height.
Model top: incremental offset from the Model Top.
Model bottom: incremental offset from the Model Bottom.
Stock top: incremental offset from the Stock Top.
Stock bottom: incremental offset from the Stock Bottom.
Hole top: incremental offset from the Hole Top.
Hole bottom: incremental offset from the Hole Bottom.
Selection: incremental offset from a Point (vertex), Edge or Face selected on the model.
Origin (absolute): absolute offset from the Origin that is defined in either the Setup or in Tool Orientation within the specific operation.

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

Clearance height: incremental offset from the Clearance Height.
Retract height: incremental offset from the Retract Height.
Feed height: incremental offset from the Feed Height.
Bottom height: incremental offset from the Bottom Height.
Model top: incremental offset from the Model Top.
Model bottom: incremental offset from the Model Bottom.
Stock top: incremental offset from the Stock Top.
Stock bottom: incremental offset from the Stock Bottom.
Hole top: incremental offset from the Hole Top.
Hole bottom: incremental offset from the Hole Bottom.
Selection: incremental offset from a Point (vertex), Edge or Face selected on the model.
Origin (absolute): absolute offset from the Origin that is defined in either the Setup or in Tool Orientation within the specific operation.

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

Clearance height: incremental offset from the Clearance Height.
Retract height: incremental offset from the Retract Height.
Feed height: incremental offset from the Feed Height.
Top height: incremental offset from the Top Height.
Model top: incremental offset from the Model Top.
Model bottom: incremental offset from the Model Bottom.
Stock top: incremental offset from the Stock Top.
Stock bottom: incremental offset from the Stock Bottom.
Hole top: incremental offset from the Hole Top.
Hole bottom: incremental offset from the Hole Bottom.
Selection: incremental offset from a Point (vertex), Edge or Face selected on the model.
Origin (absolute): absolute offset from the Origin that is defined in either the Setup or in Tool Orientation within the specific operation.

Bottom offset

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

Passes tab settings

2d thread dialog passes tab

Threading Hand

thread hand left-right example

Right handed threads --- Left handed threads

Thread Pitch

The distance traversed for 1 complete thread. For Inch threads, it's the 1/Threads Per Inch (TPI). For Metric it's just the pitch as stated.

thread pitch diagram

Pitch Diameter Offset

The difference between the Major "D" and the Minor "d" thread diameters. This is the thread depth and the value is always positive.

pitch diameter offset diagram

Note: Required if the hole is drawn to the Minor size, or if the Boss/Cylinder is drawn to the Major size.

Do Multiple Threads

Enable to create multiple lead threads.

Number of Threads

Specifies the number of thread leads.

Compensation Type

Specifies the compensation type.

In computer - Tool compensation is calculated automatically by Fusion based on the selected tool diameter. The post-processed output contains the compensated path directly, instead of G41/G42 codes.
In control - Tool compensation is not calculated, but rather G41/G42 codes are output to allow the operator to set the compensation amount and wear on the machine tool control.
Wear - Works as if In computer was selected, but also outputs the G41/G42 codes. This lets the machine tool operator adjust for tool wear at the machine tool control by entering the difference in tool size as a negative number.
Inverse wear - Identical to the Wear option, except that the wear adjustment is entered as a positive number.

Note: Control compensation (including Wear and Inverse wear) is only done on finishing passes.

Multiple Passes

Enable to enter a value for multiple depth cuts when Thread Milling.

multiple passes example

Number of Stepovers

Enter the number of roughing steps. 2 Steps shown above.

Stepover

The maximum distance between finishing passes. (See the illustration shown above)

Repeat Passes

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

Direction

The Direction Lets you specify whether Fusion should either Climb or Conventional mill the thread.

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.

Left (climb milling)

Climb Milling

Right (conventional milling)

Conventional Milling

thread multipass example

Left - A right hand thread on an OD (boss), with a climb cut will mill from the top to the bottom.

Right - A right hand thread on an ID (hole), with a climb cut will mill from the bottom to the top.

Use the Climb or Conventional Direction parameter to control Top to Bottom or Bottom to Top cut direction.

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 walls of the part.

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.

Linking tab settings

2d thread dialog linking tab

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).

Preserve rapid movement - All rapid movements are preserved.
Preserve axial and radial rapid movement - Rapid movements moving only horizontally (radial) or vertically (axial) are output as true rapids.
Preserve axial rapid movement - Only rapid movements moving vertically.
Preserve radial rapid movement - Only rapid movements moving horizontally.
Preserve single axis rapid movement - Only rapid movements moving in one axis (X, Y or Z).
Always use high feed - Outputs rapid movements as (high feed moves) G01 moves instead of rapid movements (G0).

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.