Operation Routing and Feasibility for Machining
This section contains the following subsections:
Surface Milling and Turning Operations
Each machining process generally supports a variety of individual machining operations. The operations available for the milling processes (3-Axis Mill, 4-Axis Mill, and 5-Axis Mill) can be classified into several basic groups:
• Roughing (including the bulk removal/bulk milling operation)
• Finishing
• Keyway machining
• Rounding
• Filleting
• Indirect filleting
Similarly, the turning processes (2-Axis Lathe, 3-Axis Lathe, and Mill Turn) support a wide variety of turning operations, classified into several groups including
• Rough Turning
• Finish Turning
• Bach Rough Turning
• Back Finish Turning
• Grooving
• Parting
For each routing and process evaluated during costing, aPriori automatically determines which operation sequences to assign in order to manufacture each GCD on the part or assembly. Sequences are constrained by the general routing strategy that is in effect (see General Routing Strategy in Machining Node Process Setup Options).
Operation feasibility requirements for surface milling operations (on a mill machine or on a lathe with live tooling) include (but are not limited to) the following:
• Appropriate setup axis and part-relative tool orientation can be found. See Setup Axes and Operation Feasibility.
• GCD has no sharp corners (corners that would require a 0 tool diameter). Consider whether you should activate a setup axis to allow facing, or (if sharp corners are not the intended geometry) modify the CAD model.
• GCD’s extracted dimensions are not unreasonably small.
• For finishing operations, geometric tolerance is achievable. See the "Specifying Tolerance and Roughness" section of the aPriori User Guide.
• For Rounding, the GCD has a constant radius of curvature.
• For Side Milling, the selected tool has a length-to-diameter ratio that is smaller than the maximum side milling threshold. See Maximum Side Milling Length to Diameter Ratio in Machining Node Process Setup Options.
• For Indirect Filleting, surface is a fillet that can be created by the corner radius of a bull nose end mill, as a byproduct of facing, side-milling, or flank-milling the walls adjacent to that fillet. The geometric relation Is Fillet Of obtains between a fillet and an adjacent wall.
In addition, the surface’s fillet radius or bend diameter is sufficiently small. That is, either the fillet radius or half the bend diameter must be less than the value of the setup option Specify Maximum Radius for Indirect Filleting (see Machining Node Process Setup Options).
The default setting is the percentage of the part’s size specified for indirect filleting in the lookup table tblOperationSizeRanges (12% in starting point VPEs), or else the value of the cost model variable absoluteMaxFilletRadius (300mm in starting point VPEs), if that’s smaller.
Indirect filleting is a no-cost feature, with 0 cycle time, since it is assigned to features that are created as a side-effect of side milling, facing, or ball mill contouring.
• For Direct Filleting: surface is a fillet that must be made as a distinct operation separate from the finishing of adjacent walls. (For example, a fillet between two walls that meet at an acute angle cannot be made by indirect filleting, since the side of a standard cylindrical bull-nose end mill would interfere with one of the walls.)
Direct Filleting is assumed to use a ball nose end mill with a radius matching that of the fillet.
Direct Filleting cycle times account for the time required to drive the ball nose end mill along the fillet trajectory. Direct Filleting is much faster than Contouring, which assumes that the surface is finished with a smaller-radius ball nose end mill and must traverse multiple back-and-forth toolpaths in order to “scrub” the surface.
See also Multiple Approach Surface Finishing.
Operation feasibility requirements for surface turning operations include the following:
• An appropriate turning axis is available.
• For internal GCDs, boring bar length to diameter ratio is within range.
• For finish turning and back finish turning, geometric tolerance is achievable.
• For grooving, there is face and radial tool accessibility.
Hole-making and Hole-finishing Operations
The machining cost model supports the following hole-making operations:
• Step Drilling (must be manually selected)
• Counterboring
• Center Drilling
• Drilling
• Pecking
• Groove Turning
• Groove Milling
• Gun Drilling
• Preturn Drilling
• Postdrill Rough Turning
• Rough Boring
• Semi-finish Boring (see Boring Enlargement)
• Jig Boring (See Jig Boring and Jig Grinding)
• Large Hole Milling (Rough Milling followed by Side Milling)
• Large Hole Turning (Preturn Drilling followed by Postdrill Rough Turning)
The machining cost model supports the following hole-finishing operations:
• Reaming
• Finish Turning
• Finish Boring
• Jig Grinding operations (General Grinding, ID Finish Plunge Grinding, ID Finish Traverse Grinding)
See also Threading Operations and Edge Operations.
All hole-making operations are subject to the following constraints:
• GCD is not flanged.
• GCD is not obscured (undercut)—except for Groove Milling and Turning operations.
• Appropriate setup axis exists--except for Back Counterboring. See Setup Axes and Operation Feasibility.
Below are additional feasibility constraints, listed by operation. Note that, for each process, acceptable ranges (such as diameter ranges and length-to-diameter ratio ranges) are specified in the lookup table tblOperationSizeRanges.
Deep Bore Machine operations:
• Drilling and Trepanning
o GCD axis is coincident with part’s turning axis.
o GCD diameter is within range.
o GCD length-to-diameter ratio is within range.
Gun Drill operation:
• Drilling
o GCD length-to-diameter ratio is within range.
o Required tolerance is achievable by the operation.
Drill Press, Mill, and Lathe operations:
• Boring
o GCD diameter is within range.
o Required tolerance is achievable by the operation.
• Center Drilling:
o GCD length-to-diameter ratio is within range.
o GCD diameter is within range, if the part is delicate (see the cost model variable delicatePartRatio).
Note that optionality rules remove center drilling from an operation sequence if the GCD’s axis coincides with the stock’s axis, for tube stock.
Similarly, center drilling is removed from an operation sequence if the GCD is part of a multistep hole but is not the smallest hole of the multistep hole.
• Countersinking
o GCD has a chamfered edge.
o GCD diameter is within range.
Note that, when a hole is countersunk at both ends, a current limitation in geometry extraction prevents the cost model from assigning distinct setup axes to each countersinking operation. While the cost model accounts for the cost of both countersinking operations, it only accounts for the cost of the setup for one of the operations.
• Drilling
o GCD length-to-diameter ratio is within range.
o GCD is part of a multistep hole only if it is the smallest hole of the multistep hole.
• Counterboring
o GCD is part of a multistep hole and is not the smallest hole of the multistep hole.
o GCD diameter is within range.
• Back Counterboring; see Back Counterboring.
• Pecking
o GCD length-to-diameter ratio is within range.
o GCD diameter is within range, if the part is delicate (see the cost model variable delicatePartRatio).
• Reaming
o GCD diameter is within range.
o Required tolerance is achievable by the operation.
Other Mill and Lathe operations:
• Finish Turning
o GCD length-to-diameter ratio is within range.
o Required tolerance is achievable by the operation.
• Finish Boring
o GCD diameter is within rage.
o Required tolerance is achievable by the operation.
• Postdrill Rough Turning
o GCD’s axis is coincident with part’s turning axis.
o GCD diameter is within range.
o GCD length-to-diameter ratio is within range.
• Preturn Drilling
o Part is not made from tube stock
o GCD is part of a multistep hole only if it is the smallest hole.
• Rough turning
o GCD length-to-diameter ratio is within range.
• Gun Drilling
o Machine supports gun drilling (as specified by the machine property Can Gun Drill).
o GCD length is less than the value of the cost model variable maxGunDrillingLegth.
o GCD length-to-diameter ratio is within range.
o Required tolerance is achievable by the operation.
• Side Milling
o GCD length-to-diameter ratio is within range.
o Required tolerance is achievable by the operation.
• Hole Bottom Finishing (see Hole Bottom Geometry and Hole Bottom Finishing)
Hole Bottom Geometry and Hole Bottom Finishing
By default in starting point VPEs, the cost model does not take CAD-modeled hole bottom geometry literally; it assumes that hole bottoms are conical in shape, regardless of how they are modelled in CAD. That is, by default in starting point VPEs, the cost model assumes that the actual hole bottom is produced by the tip of a standard drilling tool, and that no milling operations are required to achieve the desired shape.
VPE administrators can customize this default with the cost model variable flatHoleBottoms. The cost model variable has two possible values:
• Flexible: This is the default. Hole bottoms are not interpreted literally. Milling operations are not assigned to the hole-bottom surfaces; the hole is assumed to be made by a drilling sequence alone (unless the diameter of the hole is beyond the drillable diameter threshold and the hole is routed to a rough/finish milling operation sequence).
• Literal: Hole bottoms are interpreted literally. Milling operations are assigned to the hole-bottom surfaces, if necessary.
Users can override the default behavior on a part-by-part basis with the setup option Hole Bottom Geometry Interpretation, defined on the Machining routing node.
The setup option has two possible settings (with the same meanings as the associated cost model variable values):
• Flexible: This is the default. Hole bottoms are not interpreted literally. Milling operations are not assigned to the hole-bottom surfaces. The hole is assumed to be made by a drilling sequence alone.
• Literal: Hole bottoms are interpreted literally. Milling operations are assigned to the hole-bottom surfaces, if necessary.
To override the default for a particular hole, manually assign a specific hole-making operation sequence to the hole, or assign surface-finishing operations to the hole’s child surfaces.
The example below shows the costing results of both the flexible and literal interpretations of two different holes.
The first hole is modeled in CAD with a flat bottom. With the Flexible setting, the flat bottom is assumed to be a modeling simplification, and is not interpreted literally; the hole is assumed to be created by the drilling sequence Center Drilling > Pecking alone. No finishing operations are assigned, resulting in a shorter cycle time, compared to the results of the Literal setting.
With the Literal setting, the first hole is assigned finishing operations subsequent to the drilling sequence:
• Planar Face facing
• Curved Surface filleting
resulting in a longer cycle time, compared to the results of the Flexible setting.
The second hole is modeled in CAD with a nearly spherical bottom. With the Flexible setting, the modeled hole bottom geometry is not interpreted literally; the hole is assumed to be created by the drilling sequence Center Drilling > Drilling alone. No finishing operations are assigned, resulting in a shorter cycle time, compared to the results of the Literal setting.
With the Literal setting, the second hole is roughed and finished with milling operations. Finishing operations include:
• Planar Face facing
• Curved Wall side milling
• Curved Surface indirect (no cost) filleting (a secondary effect of Curved Wall side milling)
resulting in a longer cycle time, compared to the results of the Flexible setting.
Perimeter Milling Operation
The 3 Axis Mill, 4 Axis Mill, and 5 Axis Mill processes provide the Perimeter Milling operation. Perimeter milling is a technique used to mill external or internal contours of through-all features, resulting in a “dropped-off” volume of material either outside or inside the milled perimeter. Without the use of perimeter milling, all removed starting billet volume is converted to chips.
With Stock Machining, aPriori decides to include Perimeter Milling in a perimeter GCD’s operation sequence if all the following hold:
• Setup option Roughing Technique is set to Perimeter Milling with Dropoff. The default setting is specified by the Stock Machining cost model variable defaultRoughingTechnique (All Bulk Milling in starting point VPEs--see Stock Machining Node Process Setup Option).
• Perimeter is external (see PSCs and Perimeters).
• Perimeter is sufficiently closely aligned with a principal, rotational, or user-activated setup axis. Maximum allowable misalignment is specified by the Machining cost model variable perimeterMillingAngularTolerance (5 degrees in starting point VPEs).
You can turn perimeter milling on or off for individual Perimeter GCDs by editing the GCD’s operation sequence.
See also Stock Machining Routing and Plate Stock.
Threading Operations
All threading operations are subject to the following feasibility constraints:
• GCD is threaded.
• GCD diameter is within range (as specified in the lookup table tblOperationSizeRanges).
• Current operation sequence does not contain a prior threading operation.
• Material is compatible with threading (based on cut code) on the current machine.
Edge Operations
Edge treatment operations are subject to the following feasibility constraints:
• Chamfer milling and Countersinking:
o Edge is chamfered.
o Diameter is within range (as specified in the lookup table tblOperationSizeRanges).
• Countersinking:
o Edge is chamfered.
o Diameter is within range (as specified in the lookup table tblOperationSizeRanges).
• Round milling:
o Edge is rounded.
• Edge turning:
o Appropriate turning axis exists.
o Edge is not sharp.
Keyway Broaching
Keyway broaching operations include the following:
• Single Pass Keyway Broaching. This used by default. It is pull-type keyway broaching, suitable for high-volumes.
• Multipass Keyway Broaching. This must be selected manually. It is shim-type keyway broaching, suitable for low volumes.
The feasibility rules for these operations require that the keyway GCD have the following characteristics:
• Bottom is flat.
• Open at both ends (through).
• No shoulders obstructing line of sight.
• Internal.
• Desired tolerance is achievable by the operation.
Internal Keyway appropriate for Broaching
Note that only keyways with rectangular cross-sections are recognized by geometry extraction.
Boring Enlargement
Hole that are aound 1 to 2 inches in diameter and that have tight positional or diametrical tolerance may be assigned an operation sequence that includes boring enlargement (rough boring followed by semi-finish boring).
Optional boring enlargement is available as part of the Standard Drilling operation and Drilling and Boring sequences. A hole that meets all the following conditions is assigned a Standard Drilling operation sequence:
• Hole is not undercut.
• Diameter is within range for Standard Drilling, as specified by the lookup table tblOperationSizeRanges. In starting point VPEs, this is less than 20% of the part’s length, width, or height, whichever dimension is between the other two.
• At least one of the following holds:
o Length-to-diameter ratio is within range for Standard Drilling (as specified by the lookup table tblOperationSizeRanges)—less than 3 in starting point VPEs). Deep drilling and gun drill are not supported.
o Part is not delicate (that is, the ratio of the part’s two smallest box dimensions is less than the cost model variable delicatePartRatio—8 in starting point VPEs).
o Hole requires boring enlargement (see below).
Boring enlargement is required for a hole, and included in the Standard Drilling sequence, if the hole meets all the following conditions:
• Diameter falls between the following two values (inclusive):
o Cost model variable roughBoringLowerDiameter (25.4mm in starting point VPEs)
o Cost model variable roughBoringUpperDiameter (50.8mm in starting point VPEs)
• At least one of the following holds:
o Positional tolerance is less than the value of the cost model variable roughBoringToleranceThreshold (0.254mm in starting point VPEs).
o Diametrical tolerance is less than the value of the cost model variable roughBoringToleranceThreshold (0.254mm in starting point VPEs).
• Bottom is not flat (that is, the hole bottom is not a PlanarFace).
• Tools of the required sizes can be found (as specified by the lookup table tblSystemToolDeclarations)
Boring enlargement consists of both the following operations:
• Rough Boring
• Semi-Finish Boring
Note that boring enlargement (Rough Boring followed by Semi-Finish Boring) is followed by Finish Boring, if a finishing step is necessary to achieve the required tolerance. The operations in this sequence are assumed to use the following types of tools:
• Rough Boring: 3-tooth mill bore
• Semi-Finish Boring: 2-tooth mill bore
• Finish Boring: 1-tooth mill bore
Note: Do not specify Number of Occurrences for Rough Boring or Semi-Finish Boring. Use the setup options listed below, instead.
You can control the number of passes performed by each operation with the following setup options:
• Num Semi Finish Boring Passes: In starting point VPEs, the default number of semi-finishing passes is 2. You can customize the default number of passes with the cost model variable defaultNumSemiFinishBoringPasses. You can override the default on a GCD-by-GCD basis with this setup option; specify a value greater than or equal to 1.
• Number of Rough Boring Passes: By default, aPriori determines the number of rough boring passes based on the following factors:
o Hole radius: This is the depth of material (measured from the center outwards) that must be removed in order to create the hole.
o Radius of the initial drilling pass: this is the depth of material removed by the Drilling operation, that is, half the diameter of the Drilling tool. In starting point VPEs, the drill diameter for this initial operation of the sequence is 70% of the hole diameter (or the maximum available drill size, whichever is smaller). VPE administrators can customize this percentage with the cost model variable enlargementDrillAsFractOfHole.
o Number of semi-finishing passes (see above)
o Depth of a single semi-finishing pass: This is either 7.2mm or half the depth not removed by initial drilling and finishing, whichever is less.
o Whether a finishing pass is required and, if so, its depth (that is, the depth of material removed by the hole finishing operation). If a finishing pass is required, this is assumed to be 0.3% of the hole radius, provided this value falls between 0.0508mm (0.002 inches) and 0.127 (0.005 inches).
o Depth of a single, typical rough boring pass. This is assumed to be 7.5mm.
aPriori uses this information to determine the depth of material that must be removed by rough boring in order that the total depth of material removed by all operations adds up to the hole radius. The required number of passes is the depth that must be removed by rough boring divided by the depth of a single typical rough boring pass, rounded up to the nearest whole number of passes.
You can override the default on a GCD-by-GCD basis with this setup option; specify a value greater than or equal to 1.
Note that boring of cast holes is not currently supported.
Boring data such as feed and speed data are stored in the lookup table tblBoringV2; the lookup table tblBoring is retained for compatibility only.
Back Counterboring
For 3-Axis Mill, 4-Axis Mill, 5-Axis Mill, Mill Turn, and 3-Axis Lathe routings, inaccessible counterbores are assigned to the Back Counterboring operation performed by the Drill Press process. Back counterboring is assigned to a simple hole that meets the following conditions:
• Is a child of a multistep hole
• Is not the smallest-diameter child of that multistep hole
• Is not accessible from any setup axis
In this case, the cost model assumes that the hole is created using a manually-assembled, multi-piece counterboring tool. (Note that such a tool is not a tool with an expandable cutting edge that can be collapsed, fed through the smaller diameter, and then expanded.)
The hole shown in yellow, below, is assigned to back counterboring:
Backboring cycle time includes time to do all the following
• Feed the main tool piece through the smaller-diameter hole, and attach the back counterboring tool piece to the main tool piece.
• Center the drill press.
• Cut the hole (see Cut Time for Machining Operations).
• Detach the back counterboring tool, and remove the main piece.
Time to assemble and disassemble the tool is specified by the cost model variable counterBoringToolChangeTime (1 minute in starting point VPEs). Time to center the tool is specified by the cost model variable drillPressToolCenterTime (10 seconds in starting point VPEs).
Jig Boring and Jig Grinding
Jig Boring and Jig Grinding processes are included only if the user manually assigns a GCD to the Jig Boring operation sequence (which includes Jig Grinding for GCDs with tight tolerances).
This operation sequence is available for parts manufactured with the following primary process groups:
• Stock Machining
• 2-Model Machining
• Casting (Die and Sand)
• Forging
The Jig Boring operation is feasible for a GCD only if all the following hold:
• Part is not delicate or diameter is sufficiently small (as specified in tblSystemToolDeclarations).
• GCD’s length-to-diameter ratio within range.
• GCD is not undercut.
A GCD that has been assigned to jig boring will be assigned to jig grinding if the upstream operations can’t achieve the required positional tolerance, diametrical tolerance, or roughness.
Jig grinding is feasible only on materials with compatible cut codes (41,42, 51,or 52).
Note the following about costs associated with jig boring and jig grinding:
• They occur on separate Jig Boring machines and Jig Grinding machines, and so they incur batch setup costs, as well as part setup costs.
• Part setup times based on positional tolerance. The time is based on linear interpolation:
o For Jig Boring, it falls somewhere between the values of the cost model variables jigBoreMinPartSetupTime (2 hours in starting point VPEs) and jigBoreMaxPartSetupTime (6 hours in starting point VPEs), depending on where part’s tightest required tolerance falls between the cost model variables jigBoreMinPosTol (0.005mm in starting point VPEs) and jigBoreMaxPosTol (0.0254mm in starting point VPEs).
o For Jig Grinding, it falls somewhere between the values of the cost model variables jigGrindMinPartSetupTime (2 hours in starting point VPEs) and jigGrindMaxPartSetupTime (6 hours in starting point VPEs), depending on where part’s tightest required tolerance falls between the cost model variables jigGrindMinPosTol (0.005mm in starting point VPEs) and jigGrindMaxPosTol (0.0254mm in starting point VPEs).
• Tool indexing costs are much higher for non-CNC machines (see Machine Selection for Jig Bore and Jig Grind).
Dovetail Slot Operations
Dovetail slots are Slot GCDs whose Slot Type property is set to DOVETAIL (see Slot GCD). These slots have flat floors and symmetric, undercut walls. They are open on both ends. Any two cross-sections (in planes normal to the walls) are the same size and shape. Dovetail slots are created with the help of a special finishing tool whose geometry matches the wall undercuts.
The operation sequence for dovetail slots always includes a roughing operation followed by a finishing operation, and is sometimes followed by a rounding operation:
• Roughing operation: dovetail slot roughing uses a flat end mill to remove all the material necessary to create the slot except for the slot’s undercuts. So the roughed out portion of the slot has parallel walls.
The roughing operation is one of the following:
o Slot Milling: this is used if an appropriate tool can be found. See Diameter Selection for Slot Milling.
o Rough Milling: this is used if no appropriate slot milling tools can be found and an appropriate rough milling tool can be found. See Diameter Selection for Slot Rough Milling.
See Standard Slot Operations for more information on Slot Milling and Rough Milling.
• Finish Dovetail Milling: dovetail finishing uses a tool whose geometry matches the angle of the slot walls. In two or more passes per side, the tool removes the material that occupies the undercut portions of the slot.
• Dovetail Edge Rounding: this operation is included in the operation sequence if and only if both the following hold:
o Slot has rounded edges.
o Slot is a closed loop with no modeled drop hole.
For open-ended dovetails and loops with drop holes, the cost model assumes that rounding is performed by Finish Dovetail Milling, whose tool geometry is assumed to accommodate the rounds.
Note that if you specify the presence of a drop hole with the setup option Drop Hole Override (see Dovetail Finishing Options), but no drop hole is modeled in the CAD, rounding is nevertheless applied when the slot has rounds.
Slots for which no appropriate Slot Milling or Rough Milling setup or tool can be found (see Standard Slot Operations) are assigned General Rough Milling. Similarly, slots for which no appropriate Finish Dovetail Milling setup or tool can be found (see Diameter Selection for Dovetail Slot Finishing), are assigned General Finish Dovetail Milling. These are fallback versions of Rough Milling and Dovetail Finish Milling that use a much smaller tool diameter.
For all operations, the tool axis is normal to the slot floor.
Some of the terms used above can be defined in terms of GCD properties and relations as follows:
• Slot is a dovetail slot: the geometric property Slot Type has value DOVETAIL.
• Slot has rounded edges: the geometric property Top Round Radius A or Top Round Radius B is greater than 0.
• Slot is a closed loop: the geometric properties End1 Type and End2 Type have value LOOP.
• Slot has no modeled drop hole: a loop without a drop hole has a value of -1 for the property Throat Diameter (the diameter of the drop hole).
See also Slot Properties.
Standard Slot Operations
This section covers the operations used to make standard slots. Some of these operations are also used to help create dovetail slots (see Dovetail Slot Operations).
Standard slots are Slot GCDs that are not dovetail slots. For these slots, the Slot Type property is not DOVETAIL, but rather indicates the slot’s floor type: STRAIGHT_FLOOR (for a flat floor), SEMICIRCULAR_FLOOR, or THROUGH (for no floor). Standard slots have parallel walls that are normal to the floor, and they can have open, cylindrical or bathtub ends. They can also form a closed loop. See Slot GCD.
Standard slot roughing is performed by one of the following operations:
• Slot Milling: this operation uses a flat end mill or a ball end mill (see Tool Type Selection for Standard Slot Milling) whose diameter is the width of the slot (see Diameter Selection for Slot Milling). It creates the slot in one or more axial passes, with full radial engagement along the width of the slot, and an axial depth of cut of half the tool diameter (by default).
There are two preferred tool axis orientations for this operation:
o Normal to the slot floor: during each pass, the tool moves along the length of the slot, with an axial depth of cut that runs along the depth of the slot.
o Parallel to the slot floor and walls: during each pass, the tool moves along the depth of the slot, with an axial depth of cut that runs along the length of the slot.
In some cases, the operation is performed with a ball end mill oblique to the floor.
• Groove Milling: this operation uses a wheel cutter (a groove mill or a keyseat mill), and orients the tool axis normal the slot walls. The tool width is less than or equal to the slot width (see Tool Width Selection for Groove Milling).
Groove Milling creates the slot in one or more axial passes and one or more radial passes. During each pass, the tool moves along the length of the slot, with full axial engagement (along the width of the tool and width of the slot), and a radial depth of cut, along the depth of the slot, that is 50% of the tool width.
Unlike Slot Milling on a 3-Axis Mill, this operation is feasible for flat-floor slots with upward pitch or bathtub ends. It can also make some slots that are obstructed from the tool approaches used by Slot Milling.
• Rough Milling: as with Slot Milling, this operation uses a flat end mill or a ball end mill (see Tool Type Selection for Standard Slot Milling). Unlike Slot Milling, Rough Milling can use a tool whose diameter that is less than the width of the slot (see Diameter Selection for Slot Rough Milling), so it is appropriate for slots that are too wide for Slot Milling. It creates the slot in multiple radial and axial passes. As with Slot Milling, there are two preferred tool axis orientations: normal to the slot floor, and parallel to the slot floor and walls. In some cases the operation is performed with the a ball end mill oblique to the floor.
• General Rough Milling: a version of Rough Milling that uses a 20% lower feed, this provides a fallback when no other milling operation is feasible with an appropriate tool and setup.
• Wire EDM: must be manually assigned.
Finishing of standard slots is performed on the individual surfaces of the slot. Note that the surfaces that make up the slot floor, walls, ends, fillets, rounds, and chamfers are not child GCDs of the Slot GCD, but they are associated with the slot through GCD relations: Is Floor Of, Is Wall Of, and Is End Of, Is Fillet Of, Is Round Of, and Is Chamfer Of.
If more than one of the above operations is feasible for a slot, Slot Milling is generally preferred, followed by Groove Milling and Rough Milling. General Rough Milling is used only if the other three cannot be assigned. Wire EDM must be manually assigned.
Operation assignment depends both on the feasibility rules listed below, as well as on considerations related to tool availability, part setup, and GCD accessibility.
Slot Milling is feasible only if all the following hold:
• If the slot either has a bathtub end or pitches up (creating a concavity in the floor), the floor is semi-circular. The GCD property Min Floor Diameter reflects an upper bound on the tool diameter that can be used for the smallest bathtub end or upward pitch on the slot. It is 0 if there is no bathtub end or upward pitch:
If Min Floor Diameter > 0 then Slot Type == SEMICIRCULAR_FLOOR
• (3-Axis Mill only): If the slot has pitch, it has a semicircular floor:
If Pitch == True then Slot Type == SEMICIRCULAR_FLOOR
• If the slot has fillets, they are symmetric (that is, the number of distinct fillet diameters is no greater than 1).
Groove Milling is feasible only if all the following hold:
• The slot has a straight trajectory (GCD property Yaw is false).
• Neither end of the slot is cylindrical (neither End1 Type is nor End2 Type is Cylindrical).
• If the slot either has a bathtub end or pitches up (creating a concavity in the floor), then the tool radius required to make that end or upward pitch is greater than the slot depth. The GCD property Min Floor Diameter reflects the maximum diameter of such a tool required for the part:
Min Floor Diameter / 2 > max(Depth A, Depth B)
• Some groove mill tool can fit between the top of the slot wall and any obstruction above the wall. That is, for any Is Accessible From relation that relates the slot floor to a setup axis, if the relation is Parallel Obstructed, the Distance to Obstruction is at least 3 times the slot depth:
Distance to Obstruction >= 3 * min(Depth A, Depth B)
Rough Milling is feasible only if all the following hold:
• If the slot has a flat floor and a bathtub end or upward pitch (Max Floor Diameter > 0), then it has corner fillets. (The upward pitch or bathtub end requires a ball end mill, which can only make edges or corners with fillets.)
For all three operations, feasibility also requires that a suitable setup axis can be found.
For Groove Milling, the cost model assumes that the tool is oriented normal to the slot walls. For Slot Milling and Rough Milling, the cost model generally assumes that one of the following tool orientations is used:
• Normal to the slot floor: this orientation is used only if it allows the tool to access all of the slot floor. This orientation is often preferred for flat floors.
• Parallel to the slot floor and walls: this orientation is used only if it allows the tool to access all of the floor. For Slot Milling, it is used only if the floor is semi-circular. This orientation is often preferred for low-aspect-ratio, semi-circular floor slots.
• Oblique to the slot floor: this orientation is used only if allows the tool to access all the surfaces of the slot.
• Parallel to the walls: for through slots (slots without floors), this orientation is used if it provides access to walls and ends.
Principal setup axes are preferred over non-principal setups that are used by other operations, which are preferred over non-principal setups that are not already in use (the cost model sometimes activates a new setup in order to make an operation possible).
In general, Slot Milling is preferred to Groove Milling is preferred to Rough Milling. Operation preferences and setup axis preferences interact according to internal heuristics in order to determine operation assignment.
Note that an operation is assigned only if a tool of the suitable type and diameter can be found--see Tool Type Selection for Standard Slot Milling, Diameter Selection for Slot Milling, Tool Width Selection for Groove Milling, and Diameter Selection for Slot Rough Milling.
Note also that if a slot’s surfaces lie on a Parallel Surface Chain GCD, it is possible that these surfaces are created by a Perimeter Cut or Wire EDM Cut operation. In such a case, the slot GCD is not assigned the operations described in this section, but rather is assigned As Perimeter Cut or As Wire EDM Cut.
Deburring Operation Feasibility
Edge Deburring (Automated or Manual) is feasible only if all the following hold:
• Edge is sharp, that is, its Edge Type is neither CHAMFER nor ROUND.
• Edge is not about a turning axis.
• Edge is formed by walls at a sufficiently small angle to one another, that is, the edge's Max Wall Angle or Min Wall Angle is no greater than the value of the cost model variable deburrEdgeAngleCutOff (150 degrees in starting point VPEs).
See also Routing for Deburr Processes, for information on operation assignment.