Groove Milling Options
Groove Milling provides the following GCD-level options (the options apply to a specified slot):
Requested Tool Width
By default, tool width is slot width (the value of the geometric property
Width), if a large enough tool can be found. Otherwise, default tool width is the
Max Tool Width, looked up by groove depth and width in
tblGrooveMilling, and adjusted by a factor looked up by tool series in
tblToolSeriesMultiplier. Users can override the default with this option. Tool width affects cycle time—see
Chipmaking Time for Groove Milling.
Requested Number of Axial Passes
By default, this is the slot width (the value of the geometric property
Width) divided by the tool width (see
Requested Tool Width), rounded up to the nearest integer. Users can override the default with this setup option. The number of axial passes affects cycle time—see
Chipmaking Time for Groove Milling.
Tool Diameter
By default, tool diameter is looked up by groove depth and width in
tblGrooveMilling, and adjusted by a factor looked up by tool series in
tblToolSeriesMultiplier. Default tool diameter is also bounded above by the diameter of the tightest upward curve (pitch) in the slot floor (specified by the geometric property
Min Floor Diameter). Users can override the default with this option. Tool diameter affects tool axis speed which affects cycle time—see
Tool Axis Speed and
Chipmaking Time for Groove Milling.
Requested Number of Radial Passes
By default, this is the slot depth (the larger of the geometric properties
Depth A and
Depth B) divided by the
Radial Cut Depth, rounded up to the nearest integer. Users can override the default with this setup option. The number of radial passes affects cycle time—see
Chipmaking Time for Groove Milling.
Feed per Tooth
Distance the tool travels along the surface of the part per tooth of the tool during one rotation. The number of tool teeth times this value is the distance the tool travels along the surface of the part per rotation of the tool. This value is used to help determine the tool axis speed. See
Tool Axis Speed and
Chipmaking Time for Groove Milling for more information.
Select one of the following options:
• Use Computed Feed per Tooth: aPriori determines this value by interpolation from data tables based on tool series, tool diameter, and material cut code—see
Tool Selection. aPriori multiplies this value by the number of teeth to derive tool feed. This value is adjusted to compensate for various factors, including tool reach and required tolerance. Tool feed is also adjusted by multiplying by the cost model variable
millFeedAdjustment. The adjusted value is used to help determine tool axis speed.
• User Override: aPriori multiplies the value you enter by the number of teeth to derive tool feed. This value is adjusted to compensate for various factors, including tool reach and required tolerance. Tool feed is also adjusted by multiplying by the cost model variable millFeedAdjustment. The adjusted value is used to help determine tool axis speed.
Requested Num Teeth
Number of tool teeth. This value together with
Feed per Tooth determines feed (which affects tool axis speed)—see
Tool Axis Speed and
Chipmaking Time for Groove Milling.
Select one of the following options:
• Number of teeth: aPriori determines this value by interpolation from data tables based on tool series, tool diameter, and material cut code—see
Tool Selection. aPriori multiplies this value by the feed per tooth to derive tool feed. This value is adjusted to compensate for various factors, including tool reach and required tolerance. Tool feed is also adjusted by multiplying by the cost model variable
millFeedAdjustment. The adjusted value is used to help determine tool axis speed.
• User Override: enter a value greater than or equal to 2.
If you supply a user override for both Number of Teeth and Requested Feed per Tooth, aPriori multiplies the two values together to derive tool feed.
If you supply a user override for Number of Teeth, and you do not specify a user override for Requested Feed per Tooth, aPriori sets the unadjusted value for feed as follows:
Feed = Interpolated Feed * (Specified Number of Teeth / Interpolated Number of Teeth)
(Interpolated feed and interpolated number of teeth are derived from data tables during tool selection—see
Tool Selection.)
In either case, the value is adjusted to compensate for various factors, including tool reach and required tolerance. Tool feed is also adjusted by multiplying by the cost model variable millFeedAdjustment. The adjusted value is used to help determine tool axis speed.
Tool Cutting Speed
How fast the tool turns in unit distance per unit time; that is, the speed at which a point on the outer edge of the tool moves along the circular path around the center of the tool. This value helps determine tool axis speed. See
Tool Axis Speed and
Chipmaking Time for Groove Milling for more information.
Select one of the following options:
• Use Recommended Tool Cutting Speed: aPriori determines this value by interpolation from data tables based on tool series, tool type, tool diameter, and material cut code--see
Tool Selection. This value is adjusted to compensate for various factors, including machine spindle speed limitations and stock hardness. The value is also adjusted by multiplying by the cost model variable
millSpeedAdjustment. The adjusted value is used to help determine tool axis speed.
• Override Tool Cutting Speed: enter a speed in meters per minute. This value is adjusted to compensate for various factors, including machine spindle speed limitations and stock hardness. The value is also adjusted by multiplying by the cost model variable
millSpeedAdjustment, and a factor associated with the setup option
Rough Milling Aggression Adjustment Dial (see
User Inputs for Machining). The adjusted value is used to help determine tool axis speed.
Radial Cut Depth
Cut depth either in millimeters or as a percentage of the tool width. This is the length, along the depth of the slot, of the region of contact between the part and the tool during chipmaking. Radial cut depth helps determine the number of passes required to create the slot. See
Chipmaking Time for Groove Milling.
By default, radial cut depth is 25% of tool diameter for standard groove milling tools, and 45% of diameter for reduced shank groove mills. (Reduced shank groove mills have 20% lower feed and tool life than standard tools, and 20% higher cost—see the lookup table tblToolSeriesMultipliers.)
Users can override the default with this setup option, by doing one of the following:
• Specify the radial cut depth in millimeters.
• Specify the radial cut depth as a percentage of the tool width.