Tool Selection for Machining
For milling and drilling operations, tool selection does the following:
• Picks a tool diameter appropriate for the current operation and GCD. See Diameter Selection for Surface Milling and Length to Diameter Ratio Check.
• Picks an appropriate tool series from the lookup table tblSystemToolDeclarations. See Tool Series Selection.
• Establishes values for various tool properties, such as speed and feed. See Tool Properties.
For turning operations, tool selection does the following:
• Picks an appropriate tool series from the lookup table tblSystemToolDeclarations. See Tool Series Selection.
• Establishes values for various tool properties, such as speed and feed. See Tool Properties.
Note that, unlike milling and drilling, turning tool selection does not select a tool diameter. With turning, the diameter relevant to speed and feed (see Feeds and Speeds in the Machining Cost Model) is the workpiece diameter rather than tool diameter (where the workpiece diameter is the diameter of a cross-section at the cut location normal to the turning axis).
This section has the following subsections:
Diameter Selection
Diameter selection is covered in the following sections:
Diameter Selection for Surface Milling
For milling operations on surfaces, tool selection generally picks a tool diameter based in part on the following:
• Overall part size.
• The largest diameter small enough to produce the corners between the GCD and the adjacent convex walls. For many operations, this is specified by one of the following properties:
o GCD property Corner Diameter
o GCD property Bend Diameter
o Wall Corner Diameter property of the Is Accessible From relation for the current GCD and the current operation’s tool orientation--see Setup Axes and Operation Feasibility. (This property takes into account the angle from which tool will approach; it is used for side milling.)
• Process-level setup options that constrain tool diameter:
o Maximum Facing Tool Diameter
o Maximum Side Milling Tool Diameter
o Maximum Contouring Tool Diameter
• Machining node setup options that constrain tool diameter:
o Specify Maximum Radius for Indirect Filetting
o Specify Maximum Radius for Rounding
• Operation-level process setup option Requested Tool Diameter.
• Machine property Max Mill Tool Diameter.
For face milling of a planar face, diameter selection is also affected by process setup options that potentially constrain the total number of distinct tool diameters used for planar face facing:
• Facing Maximum Tool Count
• Estimated Minimum Facing Diameter
• Estimated Maximum Facing Diameter
See Diameter Selection for Planar Face Facing for more information on face milling of planar faces.
For side milling of a partially obstructed surface, tool diameter is sometimes constrained by the Distance to Obstruction property of the relevant Is Accessible From relation—see Examples: Side Milling/Facing.
Diameter Selection for Holemaking and and Hole Finishing
For drilling operations, tool selection generally picks the GCD diameter as the tool diameter, or else it uses the diameter specified by an operation-level setup option, such as Requested Tool Diameter (see Hole Making Options).
For milling operations on holes, tool selection picks half the tool diameter, or else it uses the diameter specified by an operation-level setup option, such as Requested Tool Diameter (see Hole Making Options).
Large hole roughing and milling generally uses a flat end mill tool equal to 1/2 of the hole's diameter, up to the largest allowable end mill for the part. You can customize this fraction of the hole diameter with the cost model variable largeHoleMillingDiameterRatio (0.5 in starting point VPEs). The tool diameter is also constrained to be between 20% and 80% of the hole diameter.
For thread milling operations, tool selection picks 95% of the GCD diameter.
Diameter Selection for Pocket Roughing
Diameter selection picks either one or two diameters for roughing a given pocket. If two diameters are chosen, two occurences of the Rough Milling operation are associated with the pocket. The first occurrence uses the larger diameter to remove most of the pocket’s volume, and the second occurrence uses the smaller diameter (chosen to fit into the corners) to remove the remaining volume.
Users can override aPriori’s choice of diameters with the setup option Requested Percent Milled—see Pocket Rough Milling Options.
Default diameter selection for rough milling first preselects a diameter, snaps to down to a part-specific, industry-standard, preferred diameter.
Diameter preselection for pockets proceeds as follows:
1 Find the largest diameter that fits inside the pocket and into the pocket’s corners; that is, choose the minimum of the following geometric properties:
o Corner Diameter
o SER Width
o SER Length
If the Corner Diameter is 0, do not choose a diameter in this step.
2 Pick a diameter that is a fraction of the pocket’s Inside Diameter; in particular, choose the diameter that is the fraction of Inside Diameter specified by the cost model variable maxRoughingInsideDiaPercentile (0.85 in starting point VPEs), but no less than 50% of the Inside Diameter.
3 If a diameter was chosen in step 1, and it is less than the diameter chosen in step 2, the results of 1 and 2 are used as the preselected diameters. In this case, there will be two instances of the Roughing operation for the current GCD; the first will use the step 1’s diameter as the preselected diameter, and the second will use step 2’s diameter as the preselected diameter.
If the diameter chosen in step 1 is greater than or equal to the diameter chosen in step 2, the result of step 2 is used as the only preselected diameter. In this case, there will be one instance of the Roughing operation for the current GCD, and that instance will use step 2’s diameter as the preselected diameter.
If no diameter was chosen in step 1, that is, if the Corner Diameter is 0, the cost model assumes that the corners of the actual part are not accurately reflected by the CAD model. In this case, the cost model further assumes that the diameter chosen in step 2 is small enough to fit into the actual corners, so the result of step 2 is used as the only preselected diameter.
The diameters of ball end mills are bounded above by the maximum values for the tool type specified in the lookup table tblOperationSizeRanges.
Diameter Selection for Dovetail Slot Finishing
Dovetail finishing uses a tool whose geometry is assumed to match the angle and depth of the slot-wall undercuts. In two or more passes, the tool removes the material that occupies the undercut portions of the slot.
This section describes default diameter selection. Users can override the default with the setup option Override Tool Dimensions (see Dovetail Finishing Options).
For a given dovetail slot, the cost model attempts to identify the largest diameter tool that meets the following requirements:
• The tool must be small enough to fit in a space from which it can initiate the first finishing pass:
o For a closed loop dovetail slot with no drop hole, the tool must fit within the roughed slot. That is, tool diameter must be no greater than the roughed slot width (GCD property Width).
Tool Diameter <= GCD Width
o For a closed loop dovetail slot with a drop hole, the tool must fit within the drop hole. That is, tool diameter must be no greater than the drop hole width (slot property Throat Diameter).
Tool Diameter <= GCD Throat Diameter
o For an open-ended dovetail slot, this criterion places no restriction on diameter.
• The tool must be small enough to cut at an appropriate radial depth in the first pass, given the width of the roughed slot:
o For conservative finishing (see Aggressive versus Conservative in this section, below), the tool diameter must not exceed the rough slot width (GCD property Width) by more than the appropriate first-pass, per-side, radial cut depth.
Tool Diameter <= GCD Width + First-pass, Per-side, Radial Cut Depth
o For aggressive finishing (see Aggressive versus Conservative in this section, below), the tool diameter must not exceed the rough slot width (GCD property Width) by more than twice the appropriate first-pass, per-side, radial cut depth.
Tool Diamater <= GCD Width + 2 * First-pass, Per-side, Radial Cut Depth
The appropriate first-pass, radial cut depth depends on slot depth, slot undercut width, and tool neck diameter, and is determined as described later in this section (see Radial Cut Depth, below).
• Tool diameter and tool neck diameter must be within range and appropriately proportioned with respect to one another and with respect to the slot depth (the larger of GCD properties Dovetail Depth A and Dovetail Depth B). The tool neck diameter is the difference between the tool diameter (also known as the tool major diameter) and twice the slot undercut width (GCD property Undercut Width A):
In particular, all the following quantities must be within range (starting point VPE ranges are shown in parentheses):
o Tool neck diameter (bounded below by 0.35mm)
o Tool major diameter (bounded above by 25.4mm)
o Ratio of tool neck diameter to tool major diameter (bounded above by 1)
o Ratio of dovetail depth to tool major diameter (bounded above by 1.05)
o Ratio of dovetail depth to tool neck diameter (bounded above by 3.75)
The lookup table tblOperationSizeRanges specifies the acceptable range for each of these quantities.
A value of -1 indicates that the range is unbounded on one end.
See Slot Properties for more information on the GCD properties mentioned in this section.
Tool selection fails if aPriori can find no tool that meets the selection criteria. In starting point VPEs, tool selection also fails if the slot walls form an angle of less than 30 degrees with the slot floor. This lower bound on the wall angle (GCD property Wall Angle A) is specified in the lookup table tblOperationSizeRnages.
If tool selection fails for Finish Dovetail Milling, the operation General Finish Dovetail Milling is used instead.
Aggressive versus Conservative
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.
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.
Users can override the default with the setup option Cutting Method on First Pass (see Dovetail Finishing Options). In this case, aPriori attempts to select a tool only under the assumption specified by the setup option. If no such tool can be found, tool selection fails.
Radial Cut Depth
First-pass, per-side, radial cut depth is determined as follows:
1 Determine the number of passes required, based on slot depth and tool neck diameter: this uses 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 (the larger of the GCD properties Dovetail Depth A and Dovetail Depth B).
2 Look up by number of passes the percent of total undercut width to be removed in the first pass: this uses the lookup table tblDovetailFinishingPassCharacteristics:
3 The first-pass cut depth is this percentage of the slot’s undercut width (GCD property Undercut Width A).
Diameter Selection for Slot Milling
For a given slot, the cost model selects the largest standard tool diameter that doesn’t exceed the slot width.
Tool selection fails if this diameter is out of range for the tool series, or if it exceeds either of the following upper bounds on tool diameter:
• Upper Bound specified in the lookup table tblOperationSizeRanges for Slot Milling and the current tool type (Flat End Mill or Ball End Mill).
• Percentage of the part’s size specified in the lookup table tblOperationSizeRanges for Slot Milling and the current tool type (Flat End Mill or Ball End Mill)--12% in starting point VPEs. The part size, here, is the sum of the two smaller dimensions among length, width, and height.
In addition, the tool’s length-to-diameter ratio must be less than the cost model variable easyL2DRatio (3 in starting point VPEs) or the setup option Specify Easy Side Milling Length to Diameter Ratio (see Machining Node Process Setup Options).
Tool Width Selection for Groove Milling
The cost model selects a tool width that is the smaller of the following:
• Slot width
• The maximum tool width appropriate for the slot, based on a number of factors, including the current tool series, groove depth, material cut code, and tool type (see Max Groove Width in the lookup table tblGrooveMilling), as well as the geometric property Min Floor Diameter (diameter of the tightest upward curve in the slot floor and ends).
Once the tool width is established, the diameter is looked up by tool series, tool width, groove depth, material cut code, and tool type in the lookup table tblGrooveMilling.
Tool selection fails if the tool diameter is out of range, or if the diameter is too large to make the tightest upward curve in the floor (as specified by the geometric property minFloorDiameter).
Diameter Selection for Slot Rough Milling
For a given slot, the cost model attempts to identify the largest diameter that does not exceed any of the following upper bounds on tool diameter:
• Slot Width
• Upper Bound specified in the lookup table tblOperationSizeRanges for Rough Milling and the current tool type (Flat End Mill or Ball End Mill, in the Comment field)
• Upper Bound specified in the lookup table tblOperationSizeRanges for Rough Milling and the tool type Face Mill (in the Comment field)
• Machine property Max Mill Tool Diameter
• Percentage of the part’s size specified in the lookup table tblOperationSizeRanges for Slot Milling and the current tool type (Flat End Mill or Ball End Mill)--12% in starting point VPEs. The part size, here, is the sum of the two smaller dimensions among length, width, and height.
Tool selection fails if this diameter is out of range for the tool series.
In addition, the tool’s length-to-diameter ratio must be less than the cost model variable easyL2DRatio (3 in starting point VPEs) or the setup option Specify Easy Side Milling Length to Diameter Ratio (see Machining Node Process Setup Options). Tool length is the slot length, for a tool whose axis is oriented parallel to the slot floor.
Diameter Selection for Stock Trim Roughing
By default, roughing performed on a part’s Stock Trim GCD is assumed to use the same tool as roughing on the part’s Bulk Removal GCD. You can override the default behavior, and assign distinct tool diameters, and even a separate Stock Prep Mill process if desired.
Diameter Selection for Planar Face Facing
By default in starting point VPEs, the total number of distinct tool diameters used for face milling the current part’s planar faces is limited to 4, 5, or 6, depending on part geometry (see Part-specific Preferred Diameters, below). VPE administrators can customize the default maximum limit with the cost model variable maxFacingToolsDefault. Users can customize or remove the limit with the setup option Facing Maximum Tool Count (defined on the Machining node).
The setup option has two modes:
• Unlimited number of facing tools: in this case, potentially, each faced surface uses a distinct tool diameter.
• Limited number of facing tools: this is the default mode. Users can enter a limit explicitly.
If the number of tools is unlimited, tool selection for planar face facing follows these steps:
1 Preselect a diameter based on the surface’s geometry. Preselection chooses a theoretically ideal tool size, taking into account the corner diameters of any surrounding walls. For details, see Preselected Diameters, below.
2 Snap down the preselected diameter to the nearest industry-standard tool size; that is, select the largest industry-standard tool size that is less than or equal to the pre-selected size. Industry standard tool sizes are listed in the lookup table tblPreferredSizes in the Machining process group.
If the number of tools is limited to N distinct tool diameters, then the cost model forms a list of N preferred diameters based on the geometry of all the part's planar faces that are accessible to facing (see Part-specific Preferred Diameters, below). The list includes at least 4 standard tool diameters. Only preferred diameters are used for facing, but they are not necessarily all used. In this case, tool selection follows these steps:
1 Preselect a diameter based on the surface’s geometry. Preselection chooses a theoretically ideal tool size, taking into account the corner diameters of any surrounding walls. For details, see Preselected Diameters, below.
2 Snap down the preselected diameter to the nearest preferred size. The preferred sizes consist of N industry-standard tool diameters spread out between the minimum and maximum, snapped-down, preselected diameters for the part as a whole. The preferred diameters are not evenly spread out from the minimum to the maximum, but rather are more tightly clustered near the minimum and are more spread out towards the maximum.
For details, see Part-specific Preferred Diameters, below.
Users can override the maximum and minimum preferred diameters with the setup options Estimated Minimum Facing Diameter and Estimated Maximum Facing Diameter (defined on the Machining node).
Preselected Diameters: Diameter preselection for a given planar face depends on whether the surface is raised, sunken (almost entirely surrounded by concave walls), or partially sunken (partially surrounded by concave walls):
• Raised: A planar face is considered raised if its Percent Concave Perimeter property is 0. In this case, preselection picks the largest tool that is small enough to satisfy all the following selection criteria:
o Smaller than the current machine’s maximum diameter
o Smaller than the selected tool series’ maximum diameter
o Smaller than the maximum diameter appropriate for the part (calculated based on the largest two dimensions of the part’s bounding box)
o Smaller than the maximum diameter for face mill facing listed in the lookup table tblOperationSizeRanges
• Sunken: A planar face is considered sunken if its Percent Concave Perimeter property is 98% or more. In this case, preselection picks the largest tool that is small enough to satisfy all the following selection criteria:
o Small enough to fit in all the surface’s corners (as indicated by the property Corner Diameter)
o Diameter less than or equal to 80% of the largest diameter that can access at least 80% of the surface
o Smaller than the current machine’s maximum diameter
o Smaller than the selected tool series’ maximum diameter
o Smaller than the maximum diameter appropriate for the part (calculated based on the largest two dimensions of the part’s bounding box)
o Smaller than the maximum diameter for face mill facing listed in the lookup table tblOperationSizeRanges
• Partially sunken: A planar face is considered partially sunken if its Percent Concave Perimeter property is greater than 0 and less than 98%.
In this case, if there are non-negligible corners (the face’s Corner Diameter is greater than or equal to 0.254mm), preselection does one if the following:
o If 90% or more of the planar face is the floor of a slot (see Slot GCD), and the width of the slot's fillets (if any) is less than 25% of the slot width, the preselected diameter is equal to the slot width. (90%, here, is used in Starting point VPEs; the value can be customized with the cost model variable areaOfSurfaceInSlot. Similarly, 25%, here, is used in starting point VPEs; the value can be customized with the cost model variable filletCoverageForFacingOfSlotFloor.)
o Otherwise, preselection picks the largest tool that is small enough to fit in the corners. If there are no non-negligible corners, tool selection picks a diameter that is the weighted average of (1) the diameter that would be chosen if the surface were raised, and (2) the diameter that would be chosen if the surface were sunken (see above). The first term is weighted by the fraction of the surface’s perimeter that is not surrounded by a wall, and the second term is weighted by the fraction of the surface’s perimeter that is surrounded by walls (as specified by Percent Concave Perimeter).
Note: Diameter selection ignores corners that are, in the CAD model, smaller than any realistic mill diameter (that is, smaller than 0.254mm, the smallest preferred number in the US unit system). In such a case, it is assumed that the corners of the actual part are not accurately reflected by the CAD model. The cost model assumes that the tool selected based on the other selection criteria (see above) is small enough to fit into the actual corners.
Part-specific Preferred Diameters: Tool selection follows these steps in order to find the preferred diameters:
1 Find the total number, n, of distinct, preselected diameters (see Preselected Diameters, above), taking into account all the part’s planar faces that are accessible from a direction normal to the face.
2 Determine the total number, N, of part-specific preferred diameters. By default, this is determined from n (found in step 1) as follows:
N = max(min(6, roundup(0.4n + 2.5)), 4)
In other words, by default,
• N is roundup(0.4n + 2.5), if roundup(0.4n + 2.5) is between 4 and 6.
• N is 4, if roundup(0.4n + 2.5) is less than 4.
• N is 6, if roundup(0.4n + 2.5) is greater than 6.
Users can override the default, and specify N explicitly—see Facing Maximum Tool Count in Machining Node Process Setup Options
3 Find the maximum and minimum preferred diameters. By default, these are the minimum and maximum diameters found in step 1, snapped down to the nearest industry-standard tool size. Industry-standard tool sizes are listed in the lookup table tblPreferredSizes. Users can override the maximum and minimum with the setup options Estimated Minimum Facing Diameter and Estimated Maximum Facing Diameter (defined on the Machining node).
4 Form a Renard sequence of N preferred diameters as follows (where N is defined in step 2, above): form a geometric progression starting with the minimum diameter and ending with the maximum diameter (found in step 3), where the ratio of each pair of successive terms is the N-1 root of the ratio of the maximum diameter to the minimum diameter, that is, where the common ratio of the geometric progression is
(Maximum Diameter/Minimum Diameter)^(1/(N-1))
5 Snap down each member of the Renard sequence to the nearest industry-standard tool size (except the maximum and minimum, which are already snapped down). These snapped-down values are the part-specific preferred tool sizes.
Using a Renard sequence in this way generally minimizes the discrepancies (as a percentage of diameter) between the preselected diameters and the preferred diameters.
PSCs and Perimeters
Operation assignment and diameter selection for side milling rely on information about two special GCD types:
• Perimeter GCD
• Parallel Surface Chain (PSC)
It is often possible (and desirable) for all the surfaces that lie on a perimeter or PSC to be side milled using a single setup and a single tool. (See also Diameter Selection for Side Milling.)
A perimeter GCD is the closed boundary around the projection of a part onto a plane normal to the part’s length, width, or depth direction (that is, the length, width, or depth direction of the part’s bounding box, where height <= width <= length).
Each part has three external perimeters:
• Height-direction perimeter: contained in a plane normal to the height direction.
• Width-direction perimeter: contained in a plane normal to the width direction.
• Length-direction perimeter: contained in a plane normal to the length direction.
A part might also have internal perimeters due to internal, through-all cut-outs.
Shown in pink is this part’s height-direction perimeter, which lies in a plane normal to the height direction. The walls that lie on this perimeter are shown in yellow.
The following image shows an internal perimeter in pink, with surfaces that lie on the perimeter in yellow:
An internal perimeter is shown in pink. The walls that lie on this perimeter are shown in yellow.
The LIES ON relation between surfaces and perimeters is shown in the Geometric Cost Drivers pane. A planar face lies on a perimeter if both the following hold:
• Planar face contains line segments that are normal to the plane containing the perimeter.
• For each such line segment there is a line that contains both the line segment and some point on the perimeter.
A curved wall lies on a perimeter if both the following hold:
• Rules of the curved wall are normal to the plane containing the perimeter.
• For each such rule there is a line that contains both the rule and some point on the perimeter.
A curved wall is described by a rule translated along a smooth curve.
A parallel surface chain (PSC) is a non-perimeter GCD that consists of a closed loop of planar faces and curved walls that are all parallel to each other in the following sense:
o The rules of a PSC’s curved walls all run in the same direction.
o Each planar face of a PSC contains lines that are co-directional with rules of the PSC’s curved walls.
PSCs can be internal or external (indicated by the value of the Location property in the Geometric Cost Drivers pane).
An internal or external PSC consists of a closed loop of surfaces that can all be side milled from the same setup.
Some PSCs have the value UNKNOWN for Location, as with the PSC shown in red:
The PSC shown in red has the value UNKNOWN for the Location property, rather than INTERNAL or EXTERNAL.
Diameter Selection for Side Milling
Diameter selection for side milling makes use of some special considerations, including whether the surface to be side milled lies on a PSC or height-direction perimeter (see PSCs and Perimeters). It is often possible (and desirable) for all the surfaces of a perimeter or PSC to be side milled using a single setup and a single tool. In these cases, aPriori chooses a tool diameter as described below.
For surfaces on a perimeter:
• If there is at least one concave curved wall on the perimeter, the tool diameter is the bend diameter of the curved wall with the smallest bend diameter. (See the property Bend Diameter in the Geometric Cost Drivers pane.)
• If there is no concave curved wall, the tool diameter is the height of the part’s bounding box.
For surfaces on the height-direction perimeter, the tool diameter is the bend diameter of the concave wall with the smallest bend diameter. If there is no concave wall, the part’s height is used as the tool diameter.
For surfaces on an external PSC:
• If there is at least one concave curved wall on the perimeter, the tool diameter is the smaller of the following:
o Bend diameter of the curved wall with the smallest bend diameter. (See the property Bend Diameter in the Geometric Cost Drivers pane.)
o Wall height of the surface with the greatest wall height (See the property Wall Height in the Geometric Cost Drivers pane.)
• If there is no concave curved wall, and there is at least one convex curved wall with a value for Diameter (see the Geometric Cost Drivers pane), the tool diameter is the smaller of the following:
o Diameter of the curved wall with the smallest diameter
o Wall height of the surface with the greatest wall height
• If there is no concave curved wall, and there is no convex curved wall with a value for Diameter, the tool diameter is the wall height of the surface with the greatest wall height.
For surfaces on an internal PSC:
• If there is at least one concave curved wall on the perimeter, the tool diameter is the bend diameter of the curved wall with the smallest bend diameter. (See the property Bend Diameter in the Geometric Cost Drivers pane.)
• If there is no concave curved wall, the tool diameter is the wall height of the surface with the greatest wall height.
For surfaces on a PSC whose value for Location is UNKNOWN, the tool diameter is the smallest of the following:
• Wall height in the direction of setup axis
• Bend diameter of the curved wall on the PSC with the smallest bend diameter
• Diameter of the curved wall on the PSC with the smallest diameter
Length to Diameter Ratio Check
For side milling, tool selection checks the ratio of the required tool reach to the selected diameter. (The required tool reach is determined by the part-relative tool orientation selected by feasibility checks—see Setup Axes and Operation Feasibility. This orientation--represented by a setup axis--bears an Is Accessible From relation to GCD. The value of the Length attribute of this Is Accessible From relation is the required tool reach.)
Tool selection fails, if the required tool reach divided by the diameter is greater than the value of the cost model variable difficultSideMillingLengthToDiameterRatio.
If the required tool reach divided by the diameter is greater than the value of the setup option easySideMillingLengthToDiameterRatio, tool selection is suspended; the cost engine moves on to consideration of other operations and then other GCDs. If the current GCD remains unassigned to an operation after that, tool selection then proceeds with the current diameter, if the node attribute runFourthCostingPass is set. Otherwise, tool selection fails.
Tool Series Selection
The selection of the tool series is based on, among others, the following factors:
• Tool diameter
• Required tool reach
• Machine capabilities
Tool series that are alike with regard to the selection criteria are ranked in order of preference in the Precedence field of the lookup table tblSystemToolDeclarations.
For turning operations, aPriori chooses the highest precedence tool of type Turning Insert, as specified in tblSystemToolDeclarations.
For threading operations, thread pitch affects tool selection (see Threading Options).
Tool Type Selection for Pocket Rough Milling
The tool type for each occurrence of the pocket rough milling operation is either Flat End Mill or Ball End Mill. aPriori automatically selects a tool type as described below. Users can override aPriori’s choice with the setup option Tool Type—see Pocket Rough Milling Options.
If two diameters are selected for the current pocket (and so there are two occurrences of the roughing operation for this pocket), the tool type for the first occurrence is Flat End Mill.
Moreover, if two diameters are selected for the current pocket, the tool type for the second roughing occurrence is Ball End Mill if and only if the pocket has one or more of the following:
• Matching wall and bottom fillet diameters
• Non-planar floor
• Walls that form an acute angle with the floor
Finally, if a single diameter is selected for the current pocket, the tool type is Ball End Mill if and only if the pocket has one or more of the following (the same three properties listed above):
• Matching wall and bottom fillet diameters
• Non-planar floor
• Walls which form an acute angle with the floor
Tool Type Selection for Standard Slot Milling
Slot Milling uses a flat end mill for slots with flat floors and a ball end mill for slots with semi-circular floors.
Groove Milling uses a keyseat mill if there is a feasible one of the appropriate width; otherwise a goove mill is used if there is a feasible one of the appropriate width.
Rough Milling uses a flat end mill if the slot is open-ended and the tool axis is parallel to the floor. Otherwise, it uses a ball end mill if any of the following hold:
• Slot has a semi-circular floor.
• Slot has a bathtub end.
• Slot is open-ended and has pitch.
Otherwise, Rough Milling uses a flat end mill.
Tool Type Selection for Deburring Operations
By default, tool type depends on GCD type (edge or surface) as well as, for edges, on edge type (internal or external).
By default in starting point VPEs, edge deburring uses the following tools:
• Internal edge deburring: Wire Tube Brush
• External edge deburring: Wire Wheel Brush
Administrators can customize the defaults with the following cost model variables:
• defaultInternalEdgeDeburrToolType
• defaultExternalEdgeDeburrToolType
Users can override the default on a per-part basis with the setup option Default Edge Deburr Tool Type.
By default in starting point VPEs, surface deburring uses the Wire Cup Brush tool type. Administrators can customize the default with the cost model variable defaultSurfaceDeburrToolType. Users can override the default on a per-part basis with the setup option Default Surface Deburr Tool Type.
Note that users can also override the tool type on a per-GCD basis with the setup option (Manual Deburr process only)
Tool type and material cut code determine the default Process Material Feed Rate, which drives cycle time.
Tool Properties
Tool selection uses interpolation from data tables (which list actual property values for a sampling of individual tools) to derive various tool properties. Tool selection generally derives these properties from the following:
• Tool series
• Tool diameter
• Cut code of the current part’s material (see the VPE Administration Guide for information on cut codes)
• Tool type
Following are some of the data tables used for this purpose:
• tblMilling
• tblDrilling
• tblGeneralTurning
Several other tables are specific to a particular process, such as tblChamfering and tblGunDrilling.
For surface milling operations, tool selection derives, among others, the following properties (see Feeds and Speeds in the Machining Cost Model):
• Speed
• Number of tool teeth
• Feed per tooth
• Maximum cut depth (flute height for the solid mill or the insert height for the insert-based mill)
For roughing operations, tool selection derives, among others, the following properties (see Feeds and Speeds in the Machining Cost Model):
• Speed
• Number of tool teeth
• Feed per tooth
• Axial cut depth
• Radial cut depth
For hole making operations, tool selection derives, among others, the following properties (see Feeds and Speeds in the Machining Cost Model):
• Speed
• Feed
For turning operations, tool selection derives, among others, the following properties (see Feeds and Speeds in the Machining Cost Model and Chipmaking Time for Rough Turning Operations):
• Speed
• Feed
• Cut depth
• Node radius
• Entering angle
For Tapping and Thread Turning, tool selection derives, among others, the following properties (see Feeds and Speeds in the Machining Cost Model and Chipmaking Time for Threading Operations):
• Speed
• Thread pitch
For Thread Milling, tool selection derives, among others, the following properties (see Feeds and Speeds in the Machining Cost Model and Chipmaking Time for Threading Operations):
• Speed
• Feed
• Thread pitch
• Threads per pass
For some edge treatment operations, such as chamfering and rounding, tool selection derives, among others, the following property:
• Linear speed (that is, tool axis speed—see Edge Treatment Engagement Time in Cut Time for Machining Operations)
For all these types of operations, tool selection also derives these properties, which help to determine Expendable Tooling Costs and Process Cycle Time:
• Tool life
• Tool life cost
• Tool hardness
Tool Selection for Keyway Broaching
After finding the appropriate tool series, tool selection for keyway broaching uses the lookup table tblPullTypeKeywayBroaching (for Single Pass Keyway Broaching) or tblShimTypeKeywayBroahcing (for Multipass Keyway Broaching).
Tool selection first finds tools that are appropriate for the GCD width and the material cut code. From those, tool selection chooses a tool whose maximum recommended keyway length is not exceeded by the GCD length. (If the GCD length is less than the minimum recommended keyway length, aPriori assumes that a plate is placed underneath the part to make up for the deficit.)
If the keyway width is too small for all available tools, tool selection picks the smallest-width tool; if the GCD is too wide for all available tools, tool selection picks the largest-width tool.
Based on the values in the lookup table, tool selection for keyway broaching sets the following tool properties:
• Cutting speed: linear cutting speed of the broach in the pull direction
• Teeth: number of teeth on the broach
• Pitch: distance between adjacent teeth
• Feed per tooth: depth of material removed (in the keyway depth direction) per tooth, per pass