Dovetail Finishing Options

The operation Finish Dovetail Milling provides the following GCD-level options (the options apply to a specified slot):

• Cutting Method on First Pass: by default in starting point VPEs, aPriori attempts to select a tool under the assumption that the tool will cut both sides of the roughed slot at once during the first finishing pass. If no such tool can be found, tool selection fails. This assumption generally allows selection of a larger, higher-speed tool (see Diameter Selection for Dovetail Slot Finishing), which significantly reduces cycle time (see Feed, Speed, and Cut Time).

VPE Administrators can change the default by setting the cost model variable preferAggressiveDovetailCuttingMethod to false. In this case, aPriori attempts to select a tool under the assumption that the tool will cut only one side of the roughed slot during the first finishing pass. If no such tool can be found, aPriori attempts to select a tool under the assumption that the tool will cut both sides of the roughed slot at once during the first finishing pass. If no such tool can be found, tool selection fails.

With this setup option, users can override the default for a given GCD. Check one of the following checkboxes:

o Let aPriori Decide: this is the default setting—see above.

o Conservative Method: in this case, aPriori attempts to select a tool under the assumption that the tool will cut only one side of the roughed slot during the first finishing pass. If no such tool can be found, tool selection fails.

o Aggressive Method: in this case, aPriori attempts to select a tool under the assumption that the tool will cut both sides of the roughed slot at once during the first finishing pass. If no such tool can be found, tool selection fails.

Note that the effect of this assumption on cycle time due to a reduction in the total number of passes required is negligible, because the feed rate must be reduced during a first pass that cuts both sides at once. But the effect on cycle time due to the use of a larger, higher-speed tool is significant.

• Drop Hole Override: for closed loop dovetail slots (see Slot Properties) the presence or absence of a drop hole affects tool selection. In general, the presence of a drop hole allows for selection of a larger, higher-speed tool (see Diameter Selection for Dovetail Slot Finishing), which can significantly reduce cycle time (see Feed, Speed, and Cut Time).

If a closed loop slot lacks a drop hole in the CAD model, this option allows the user to add a drop hole of a specified diameter, for the purposes of tool selection.

Select one of the following options:

o Drop Hole from 3D Geometry: this is the default. Tool selection assumes the presence of a drop hole only if one is modelled in the CAD.

o User Override: enter the drop hole diameter. This must be between the rough slot width (GCD property Width) and the width of the slot including undercuts (GCD property Major Diameter).

Note that this option has no effect on whether the operation Dovetail Edge Rounding is applied to the slot. If you specify the presence of a drop hole with this setup option, but no drop hole is modeled in the CAD, rounding is nevertheless applied when the slot has rounds (see Dovetail Slot Operations).

• Requested Number of Radial Passes per Dovetail Side: by default, the number of passes required per side for finishing is determined using a heuristic derived from a large, representative data sample. The heuristic represents the number of passes as a linear combination of tool neck diameter and slot depth (GCD property Dovetail Depth A). The number of passes impacts cycle time (see Chipmaking Time for Finish Dovetail Milling).

Users can override the default by selecting one of the following:

o Computed Number of Radial Passes: this is the default.

o User Override: enter the number of passes to assume for the purposes of calculating cycle time.

Note that overriding the default has no effect on tool selection; tool selection always assumes the number of passes given by the default heuristic (see Diameter Selection for Dovetail Slot Finishing).

• Requested 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 (along with speed and tool diameter) to determine tool axis speed. See Tool Axis Speed.

Select one of the following options:

o 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.

o 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 Number of Teeth on Tool: number of tool teeth. This value together with feed per tooth determines feed (which affects tool axis speed)—see Tool Axis Speed.

Select one of the following options:

o 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.

o 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.

• Requested 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 is used (along with feed and tool diameter) to determine tool axis speed. See Tool Axis Speed.

Select one of the following options:

o Use Recommended Tool Cutting Speed: aPriori determines this value by interpolation from data tables based on tool series, 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.

o 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. The adjusted value is used to help determine tool axis speed.

• Override Tool Dimensions: By default, the tool diameter is chosen as described in Diameter Selection for Dovetail Slot Finishing. With this option, users can override the default. Select one of the following options:

o Override Major Diameter: enter the tool diameter (also known as the tool major diameter).

o Override Neck Diameter: enter the tool neck diameter. The tool neck diameter is the difference between the tool major diameter and twice the slot undercut width (GCD property Undercut Width A).

• Tool Series: the tools in the default tool series are not coated with titanium aluminum nitride (AlTiN). With this setup option, users can override the default, and direct aPriori to use a tool series whose tools are titanium coated, which extends tool life and performance. For titanium-coated tools:

o Feed per tooth is 7.5% greater than tools that are not coated.

o Tool cost is 7.0% greater.

o Tool life is 10% greater.