Slot Milling Options
Slot Milling provides the following GCD-level options (the options apply to a specified slot):
Tool Diameter
Diameter of the selected tool. By default this is the slot width. (It is the largest value in the lookup table tblStandardToolSizes that is less than or equal to the value of the Width property for the slot.) You can override the default with this option. Tool diameter can affect axial cut depth (see Axial Cut Depth), which can affect cycle time (see Chipmaking Time for Slot Milling).
Requested Number of Axial Passes
By default the number of axial passes is determined as follows:
• If the tool axis is parallel to the slot floor (see Standard Slot Operations), the number of passes is the sum of the geometric properties End1 Length, Length, and End2 Length divided by the axial cut depth (see Axial Cut Depth), rounded up to the nearest integer.
• Otherwise, the number of passes is the larger of the geometric properties Depth A and Depth B divided by the axial cut depth (see Axial Cut Depth), rounded up to the nearest integer.
Users can override the default with this option.
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 Slot 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.
See also Feeds and Speeds in the Machining Cost Model.
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 Slot 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 Slot 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.
See also Feeds and Speeds in the Machining Cost Model.
Axial Cut Depth
Cut depth either in millimeters or as a percentage of the tool diameter. This is the length along the tool axis of the area of contact between the part and the tool during chipmaking. Axial cut depth helps determine the number of passes required to create the slot. See Chipmaking Time for Slot Milling.
By default, axial cut depth is half the tool diameter.
Users can override the default, with this setup option, by doing one of the following:
• Specify the axial cut depth in millimeters.
• Specify the axial cut depth as a percentage of the tool diameter.