Mechanical Features

Several types of manufacturing features are commonly encountered when designing mechanical parts. This section describes a group of objects which make it easier to construct models which contain those features. The manufacturing features currently provided include different types of holes, slots, pockets, bosses, and grooves. There are also linear, rectangular, radial, and point list pattern generators which generate patterns of either a mechanical feature or any other object. The features are constructed in any arbitrary location and orientation by using anchors. In the documentation, we will refer to a local coordinate system of the feature in order to have a reference for dimensions. The hole features, the slot feature, and the pocket features are automatically provided with extensions in the local Z (axial) direction to facilitate using these features with the set_op program. The extensions provide a true intersection as opposed to a tangency condition with the construction plane when the features are constructed with the reference or center points located on the construction plane.

 The entire features package (especially the patterns) relies quite heavily on the use of anchors for position and orientation of the individual features. This allows features to be defined in a convenient local coordinate system, but positioned and oriented arbitrarily in three-space. Features can still be used in the objTransform routine, but good use of anchors should generally make that unnecessary.

 The positional argument to the features (often called the location argument) can be entered as either a point, or an anchor. If entered as a point, the initialization of the feature creates an anchor at that point's location with a default orientation aligned with the coordinate axes.

 Anchors are right-handed coordinate frames defined by an origin and three vectors. The length of the vectors is unimportant. (In fact, the initialization causes them to be of unit length.) The depth of all of the features corresponds to the Z direction of its anchor. The use of the other directions depends on the particular feature.

Table of Contents

Hole Features

The hole features include a plain hole, a counterbored hole, a countersunk hole, a tapped hole, a counterdrilled hole, a back counterbore, and a back countersink. All the hole features are constructed in the XY plane. The hole, counterbored hole, countersunk hole, tapped hole and counterdrilled hole take a positive number for the depth of the hole in the local negative Z direction and use a Thru option to indicate whether or not the hole extends through the material. If this option is true, the hole is extended and left open on the bottom. If the Thru option is flase, the hole is capped with an 120 degree included angle cone. The back counterbore and back countersink are primarily intended to be used for manufacturing operations where the hole would be made from one side and the counterbore or countersink would be done later from the opposite side. These features do not produce a hole. If the hole would be drilled from the back side, the standard counterbored hole should be used and oriented in the desired position. The back counterbore takes a positive number for a depth in the local positive Z direction.

 A 45 degree chamfer may be specified for all the hole features except the countersunk hole and the back countersink. (The automatic extensions that are added to the feature are 0.027 units long. Therefore, specifying a chamfer that has a dimension of exactly 0.027 units may cause problems with using the combiner.) The tapped hole takes an extra Metric option to indicate whether metric (SI) or standard American English units are being used. This is necessary to correctly interpret the numbers used to specify the thread. Threads in the English units system are specified by threads per inch while metric threads are specified by pitch or millimeters per thread. The standard tap drill size is calculated using this information.

 For all the hole features below, the location of the point or anchor will correspond to the top of hole. The depth of the hole will correspond to the Z axis of the anchor. Since holes are symmetric in X and Y, the other anchor directions are unimportant.

 

hole( Loc, HoleDia, HoleDepth, Chamfer, Thru )
Returns
<hole> Constructs a hole parametric type.
Loc
<anchor | euclidPoint> Anchor for the feature. If a point is given, an anchor positioned at that point and aligned with the coordinate axes will be constructed.
HoleDia, HoleDepth
<number> Diameter and overall depth (from the specified center point) of the drilled hole.
Chamfer
<number> Width or depth of a 45 degree chamfer.
Thru
<boolean> Indicates whether or not the hole extends thru the material.
counterBore( Loc, BoreDia, BoreDepth, HoleDia, HoleDepth, Chamfer, Thru )
Returns
<counterBore> Constructs a counterBore parametric type.
Loc
<anchor | euclidPoint> Anchor for the feature. If a point is given, an anchor positioned at that point and aligned with the coordinate axes will be constructed.
BoreDia, BoreDepth
<number> Diamenter and depth of the counterbore.
HoleDia, HoleDepth
<number> Diameter and overall depth (from the specified center point) of the drilled hole.
Chamfer
<number> Width or depth of a 45 degree chamfer.
Thru
<boolean> Indicates whether or not the hole extends thru the material.
counterSink( Loc, CSinkDia, Angle, HoleDia, HoleDepth, Thru )
Returns
<counterSink> Constructs a counterSink parametric type.
Loc
<anchor | euclidPoint> Anchor for the feature. If a point is given, an anchor positioned at that point and aligned with the coordinate axes will be constructed.
CSinkDia
<number> Diameter of the countersink.
Angle
<number> Included angle of the countersink.
HoleDia, HoleDepth
<number> Diameter and overall depth (from the specified center point) of the drilled hole.
Thru
<boolean> Indicates whether or not the hole extends thru the material.
counterDrill( Loc, CDrillDia, CDrillDepth, Angle, HoleDia, HoleDepth, Chamfer, Thru )
Returns
<counterDrill> Constructs a counterDrill parametric type.
Loc
<anchor | euclidPoint> Anchor for the feature. If a point is given, an anchor positioned at that point and aligned with the coordinate axes will be constructed.
CDrillDia, CDrillDepth
<number> Diameter and depth of the counterdrilled section.
Angle
<number> Included angle of the counterdrill.
HoleDia, HoleDepth
<number> Diameter and overall depth (from the specified center point) of the drilled hole.
Chamfer
<number> Width or depth of a 45 degree chamfer.
Thru
<boolean> Indicates whether or not the hole extends thru the material.
tappedHole( Loc, ThreadDia, Thread, ThreadDepth, HoleDepth, Chamfer, Thru, Metric )
Returns
<tappedHole> Constructs a tapped hole parametric type.
Loc
<anchor | euclidPoint> Anchor for the feature. If a point is given, an anchor positioned at that point and aligned with the coordinate axes will be constructed.
ThreadDia
<number> Nominal thread diameter.
Thread
<number> Threads per inch for English units or metric pitch (millimeters per thread) for metric units.
ThreadDepth
<number> Depth of the threaded section of the hole.
HoleDepth
<number> Overall depth (from the specified center point) of the drilled hole.
Chamfer
<number> Width or depth of a 45 degree chamfer.
Thru
<boolean> Indicates whether or not the hole extends thru the material.
Metric
<boolean> Indicates whether the thread is being given in threads per inch or metric pitch (millimetrs per thread).
cdTappedHole( Loc, ThrDia, Thr, ThrDepth, HoleDep, CDDia, CDDepth, Cham, Thru, Metric )
Returns
<cdTappedHole> Constructs a counter-drilled tapped hole parametric type.
Loc
<anchor | euclidPoint> Anchor for the feature. If a point is given, an anchor positioned at that point and aligned with the coordinate axes will be constructed.
ThrDia
<number> Nominal thread diameter.
Thr
<number> Threads per inch for English units or metric pitch (millimeters per thread) for metric units.
ThrDepth
<number> Depth of the treaded section of the hole.
HoleDep
<number> Overall depth (from the specified center point) of the drilled hole.
CDDia
<number> Diameter of the counter-drill.
CDDepth
<number> Depth of the counter-drill.
Cham
<number> Width or depth of a 45 degree chamfer.
Thru
<boolean> Indicates whether or not the hole extends thru the material.
Metric
<boolean> Indicates whether the thread is being given in threads per inch or metric pitch (millimetrs per thread).
backCounterBore( Loc, BoreDia, BoreDepth, Chamfer )
Returns
<backCounterBore> Constructs a back counterbore parametric type.
Loc
<anchor | euclidPoint> Anchor for the feature. If a point is given, an anchor positioned at that point and aligned with the coordinate axes will be constructed.
BoreDia, BoreDepth
<number> Diameter and depth of counterbore.
Chamfer
<number> Width or depth of a 45 degree chamfer.
backCounterSink( Loc, CSinkDia, Angle )
Returns
<backCounterSink> Constructs a back countersink parametric type.
Loc
<anchor | euclidPoint> Anchor for the feature. If a point is given, an anchor positioned at that point and aligned with the coordinate axes will be constructed.
CSinkDia
<number> Diameter of the countersink.
Angle
<number> Included angle of the countersink.
stepBore( Loc, DiamArray, DepthArray, Chamfer, FilletRad, Thru )
Returns
<stepBore> Constructs a stepBore parametric type.
Loc
<anchor | euclidPoint> Anchor for the feature. If a point is given, an anchor positioned at that point and aligned with the coordinate axes will be constructed.
DiamArray, DepthArray
<arrayOf number> Arrays of diamenters and depths for the stepBore. The diameters should be strictly decreasing in size while the depths strictly increase. There must be the same number of elements in each array.
Chamfer
<number | arrayOf number> Width or depth of a 45 degree chamfer, used on the interior corners. The numbers in the array are used consecutively, and the last number repeated as necessary. If only one number is given, it is used for all the chamfers.
FilletRad
<number | arrayOf number> Radius of fillet to be used on the exterior corners. The numbers in the array are used consecutively, and the last number repeated as necessary. If only one number is given, it is used for all the rounds.
Thru
<boolean> Indicates whether or not the hole extends thru the material.

Slot Features

The slot feature is constructed in the XY plane with the slot length extending in the positive X direction and both ends rounded with the radius equal to one-half the slot width. The center point is located at the center of the left radius. The slot may either extend through the material or not, as indicated by the Thru flag. If the Thru flag is true, automatic extensions are provided for both the top and the bottom edge of the slot. If the Thru flag is false, a flat bottom is created for the slot.

 Because we are using right handed anchors, but we use the convention of normals pointing into a solid, anchors must be used carefully to get a "normal slot" (the one you will probably expect). The anchor Z axis corresponds to the slot depth, the anchor X axis corresponds to the slot length and the anchor Y axis is the width. To get the usual slot, use the NegZOriginAnchor.

 

slot( Loc, SlotLength, SlotWidth, SlotDepth, Chamfer, DraftAngle, BottomRadius, Thru )
Returns
<slot> Constructs a slot parametric type.
Loc
<anchor | euclidPoint> Anchor for the feature. If a point is given, an anchor positioned at that point and aligned with the coordinate axes will be constructed.
SlotLength
<number> Overall length of the slot.
Width
<number> Width of the slot.
Depth
<number> Depth of the slot.
Chamfer
<number> Width or depth of a 45 degree chamfer.
DraftAngle
<number> Draft angle for side walls.
BottomRadius
<number> Radius between the sides and the bottom.
Thru
<boolean> Indicates whether or not the slot extends thru the material.

Pocket Features

There are two pocket features, a simple rectangular pocket, and an arbitrary profile pocket. Pockets have flat sides and a flat bottom but may have a radius between the sides and the bottom. The rectangular pocket is defined by specifying the lower left corner, the length, the width, the depth, the corner radius, and the bottom radius. The four-sided pocket is defined by specifying all the corners starting with the lower left corner and going around in a CCW direction. The profile pocket is defined by a profile curve defining the outline of the top of the pocket. The top edge of the pockets are provided with automatic extensions in the Z direction to facilitate using these features with the combiner. 
rectangularPocket( ULCorner, PLen, PWid,PDepth, CrnrRad, Chamfer, DraftAngle, BottomRadius )
Returns
<rectangularPocket> Constructs a rectangularPocket parametric type.
ULCorner
<anchor | euclidPoint> Location and orientation for pocket, the upper left corner. The anchor Z direction corresponds to the pocket depth, the anchor X axis corresponds to the pocket length, and the anchor Y axis corresponds to the pocket width. If a point is given, an anchor positioned at that point and aligned with the coordinate axes will be constructed.
PLen, PWid, PDepth
<number> Overall dimensions of the pocket.
CrnrRad
<number> Radius between the sides.
Chamfer
<number> Width or depth of a 45 degree chamfer.
DraftAngle
<number> Draft angle for side walls.
BottomRadius
<number> Radius between the sides and the bottom.
profilePocket( ProfileCrv, PocketDepth, Chamfer, DraftAngle, BottomRadius, Location )
Returns
<profilePocket> Constructs a profilePocket parametric type.
ProfileCrv
<curve | arrayOf curve> The outline of the top edge of the pocket. If multiple curves are given, the first is the outer edge and the rest are islands.
PocketDepth
<number> Depth of the pocket.
Chamfer
<number> Width or depth of a 45 degree chamfer.
DraftAngle
<number> Draft angle for side walls.
BottomRadius
<number> Radius between the sides and the bottom.
Location
<anchor | euclidPoint> (Optional) The new origin and orientation of the pocket feature. The pocket origin will be aligned with the location anchor.

Facing Features

The straightStep feature is used for facing operations which involve a single step in height. A profileFace feature is also available for step-features which have an arbitrary outline. 
straightStep( Location, Length, Width, Depth, Radius )
Returns
<straightStep> Constructs a straightStep feature.
Location
<anchor | euclidPoint> Location and orientation for the feature.
Length, Width, Depth
<number> Length, width and depth of the feature.
Radius
<number> Radius for the corners of the step feature.
profileFace( CrvArray, OptLocation )
Returns
<profileFace> Constructs a profileFace feature.
CrvArray
<arrayOf curve> Curves describing the outline of the area to be faced.
OptLocation
<anchor | euclidPoint> Optional location and orientation for the feature.

Groove Features

There are four groove features that are defined including an internal groove, an external groove, a face groove, and a profile groove. 
internalGroove( CtrPt, InDia, Width, Depth, WallAngle, Radius, Chamfer )
Returns
<internalGroove> Constructs a (circular) internalGroove parametric type, which is intended to be used to add a groove to the inside (hollow) of a surface of revolution.
CtrPt
<anchor | euclidPoint> Center location for the groove (the center of the circular path of the groove).
InDia
<number> Diameter of the groove at its smallest point.
Width
<number> Width of the groove at the base.
Depth
<number> Depth of the groove.
WallAngle
<number> Angle of the walls from perpendicular to base.
Radius
<number> Radius between the bottom and the sides of the groove.
Chamfer
<number> Width or depth of a 45 degree chamfer.
externalGroove( CtrPt, OutDia, Width, Depth, Angle, BottomRad, Chamfer )
Returns
<externalGroove> Constructs a (circular) externalGroove parametric type, which is intended to be used to add a groove to the outside of a surface of revolution.
CtrPt
<anchor | euclidPoint> Center location for the groove (the center of the circular path of the groove).
OutDia
<number> Diameter of the groove at its largest point.
Width
<number> Width of the groove at the base.
Depth
<number> Depth of the groove.
Angle
<number> Angle of the walls from perpendicular to base.
BottomRad
<number> Radius between the bottom and the sides of the groove.
Chamfer
<number> Width or depth of a 45 degree chamfer.
faceGroove( Location, OutDia, Width, Depth, WallAngle, Radius, Chamfer )
Returns
<faceGroove> Constructs a (circular) faceGroove parametric type, which is intended to be used to add a circular groove to a flat face.
Location
<anchor | euclidPoint> Center location for the groove (the center of the circular path of the groove).
OutDia
<number> Diameter of the groove at its largest point.
Width
<number> Width of the groove at the base.
Depth
<number> Depth of the groove.
WallAngle
<number> Angle of the walls from perpendicular to base.
Radius
<number> Radius between the bottom and the sides of the groove.
Chamfer
<number> Width or depth of a 45 degree chamfer.
profileGroove( Profile, Width, Depth, Chamfer, WallAngle, BottomRadius, Thru, Loc )
Returns
<profileGroove> Constructs a profileGroove parametric type, which is like a face groove, but which may follow any arbitrary path.
Profile
<curve> Profile curve.
Width
<number> Width of the groove at the base.
Depth
<number> Depth of the groove.
Chamfer
<number> Width or depth of a 45 degree chamfer.
WallAngle
<number> Angle of the walls from perpendicular to base.
BottomRadius
<number> Radius between the bottom and the sides of the groove.
Thru
<boolean> Indicates whether or not the hole extends thru the material.
Loc
<anchor | euclidPoint> Location and orientation of the feature.

Boss Features

The boss parametric type constructs a boss or a protrusion that is often used to strengthen a casting or forging around a hole.

The profileBoss feature is used to remove everything from a piece of stock except for a particular profile. This feature requires specification of both the outline of the stock curve and the profile of the boss (so that the geometric construction can extend the surfaces to meet the edges of the stock). The profileBoss can be subtracted from a piece of stock using boolean operations, just like the other features. 

profileBoss( StockCrv, BossCrv, Height, Chamfer, DraftAngle, Radius, Location )
Returns
<profileBoss> Constructs a profileBoss parametric type.
StockCrv
<curve> Outline of the stock from which the boss will be cut.
BossCrv
<curve | arrayOf curve> Outline profile of the boss. It may contain multiple curves and islands.
Height
<number> Height of the boss.
Chamfer
<number> Width or depth of a 45 degree chamfer.
DraftAngle
<number> Angle for side walls of the boss.
Radius
<number> Blend radius between the sides of the boss and the surface where the boss will be located.
Location
<anchor | euclidPoint> New location and orientation for the boss feature. See profilePocket for more information about this parameter.

Other Profile Features

Three other features, profileSide, profileChamfer and profileRound are also based on a profile curve specification. 
profileChamfer( ProfileCrv, Side, Width, Height, Location )
Returns
<profileChamfer> Constructs a profileChamfer parametric type.
ProfileCrv
<curve> Profile along which the chamfer is to be made.
Side
<string> Which side of the curve to cut. Possible values are: "inside", "outside", "left", and "right."
Width
<number> Width of the chamfer.
Height
<number> Height of the chamfer.
Location
<anchor> New location and orientation for the chamfer feature. See profilePocket for more information about this parameter.
profileRound( ProfileCrv, Side, Radius, Location )
Returns
<profileRound> Constructs a profileRound parametric type.
ProfileCrv
<curve> Profile along which the round is to be made.
Side
<string> Which side of the curve to cut. Possible values are: "inside", "outside", "left", and "right."
Radius
<number> Radius of the round.
Location
<anchor> New location and orientation for the round feature. See profilePocket for more information about this parameter.
profileSide( ProfileCrv, Side, Depth, Chamfer, WallAngle, BottomRadius, Location )
Returns
<profileSide> Constructs a profileSide parametric type, which is basically an extrusion which is expected to be side-milled.
ProfileCrv
<curve> Profile for the extrusion.
Side
<string> One of "inside", "outside", "left" or "right." Indicates which side of the profile to do the milling on.
Depth
<number> The depth of the extrusion.
Chamfer
<number> Width or depth of a 45 degree chamfer.
WallAngle
<number> Angle of the walls from perpendicular to base.
BottomRadius
<number> Radius between the bottom and the sides of the groove.
Location
<anchor> New location and orientation for the feature. See profilePocket for more information about this parameter.

Pattern Features

There are four pattern features, linearPattern, rectPattern, radialPattern, and ptListPattern that can be used to create patterns of other features or any other objects. If the object being instanced has a shell for the geometry, then the return type for the geometry of all the patterns is a shell containing multiple instances of the object. Otherwise, the return type is a group. For most users of the Alpha_1 features package, the wise use of anchors will become most critical when creating pattern features. Using anchors, it is possible to specify both the location and orientation of the pattern itself as well as the location and orientation of the individual instances which make up the pattern. The actual geometry which is constructed for a pattern feature depends on the anchor used to create object being instanced. 
linearPattern( Location, Obj, NumberOfObjs, Space, UseObjectPosition )
Returns
<linearPattern> Constructs a linearPattern parametric type.
Location
<euclidPoint | Anchor> Starting location of the pattern. The point or position of the anchor specifies the new origin for the first instance in the pattern. If an anchor is given, then its orientation specifies the orientation of the pattern. The Z axis of the anchor specifies the normal to the plane in which the pattern is defined. The X axis of the anchor specifies the direction that subsequent objects in the pattern will be offset. If the Location argument is a point, then the pattern will be defined in the XY plane and the objects will be displaced in the X direction of the world coordinate system.
Obj
<object> The object to use in the pattern.
NumberOfObjs
<integer> Number of objects in the pattern.
Space
<number> Spacing between the objects.
UseObjectPosition(true)
<boolean> Default is "true" meaning that the object's position is the starting point for the pattern. A "false" value indicates that the object is to be placed at the origin before it is offset by the pattern specification.
rectPattern( Location, Obj, NRows, NCols, RowSpace, ColSpace, UseObjectPosition )
Returns
<rectPattern> Constructs a rectangular pattern parametric type.
Location
<euclidPoint | Anchor> Starting location of the pattern. The point or position of the anchor specifies the new origin for the first instance (upper left) in the pattern. If an anchor is given, then its orientation specifies the orientation of the pattern (the Z axis is the normal to the plane of the pattern, the X axis is the row direction and the Y axis is the column direction).
Obj
<object> The object to use in the pattern.
NRows, NCols
<integer> Number of objects in rows and columns of the pattern.
RowSpace, ColSpace
<number> Spacing between the row and column objects.
UseObjectPosition(true)
<boolean> Default is "true" meaning that the object's position is the starting point for the pattern. A "false" value indicates that the object is to be placed at the origin before it is offset by the pattern specification.
radialPattern( Location, Obj, NumberOfObjs, AngularSpacing, PitchDia, UseObjectPosition )
Returns
<radialPattern> Constructs a radialPattern parametric type.
Location
<euclidPoint | Anchor> Location of the pattern. The point or position of the anchor specifies the location of the center of the pattern. If an anchor is given, then its orientation specifies the orientation of the pattern.
Obj
<object> The object to use in the pattern.
NumberOfObjs
<integer> Number of objects in the pattern.
AngularSpacing
<number> Angle between successive items in the pattern.
PitchDia
<number> Diameter of the radial pattern.
UseObjectPosition(true)
<boolean> Default is "true" meaning that the object's position is the starting point for the pattern. A "false" value indicates that the object is to be placed at the origin before it is offset by the pattern specification.
ptListPattern( PtArray, Obj, UseObjectPosition )
Returns
<ptArrayPattern> Constructs a point list pattern parametric type.
PtArray
<arrayOf euclidPoint | arrayOf Anchor> Positions or orientations for instances of the object.
Obj
<object> The object to use in the pattern.
UseObjectPosition(true)
<boolean> Default is "true" meaning that the object's position is the starting point for the pattern. A "false" value indicates that the object is to be placed at the origin before it is offset by the pattern specification.

Other Features

srfRev( Profile, Kind, Axis )
Returns
<srfRev> Construct a srfRev object.
Profile
<curve> The profile curve.
Kind
<string> Possible values are "inside", "outside" and "face".
Axis
<anchor | point> Axis of revolution.
latheTool( Name, Direction, Type, Front, Back, TipRad, ToolRad, Length, Width, Depth, Material, Coating, Chip, Hand, Grade )
Returns
<latheTool>
Name
<string>
Direction
<string> "both", "right" or "left"
Type
<string> "turning", "boring", "cutoff", "inner_r_groove", "outer_r_groove", "inner_o_groove" or "outer_o_groove"
Front, Back
<number> Front & back angles.
TipRad, ToolRad
<number> Tip & tool radii.
Length, Width, Depth
<number>
Material
<string> "hss", "carbide" or "unknown"
Coating
<string> "uncoated", "cvd" or "tri_phase"
Chip
<string> "normal", "p" or "uf"
Hand
<string> "left" or "right"
Grade
<string>
sprocket( Pitch, NTeeth, Width, Location )
Returns
<sprocket>

 
Pitch
<number> Pitch of the chain in inches.
NTeeth
<integer>Number of Teeth for the sprocket
Width
<number>Width or thickness in inches for the sprocket in z
Location
<anchor | euclid point>This parameter is optional. It gives the new location and orientation for the sprocket. The sprocket origin will be aligned with the location anchor
threads( Dia, Pitch, Style, Hand, Type, Loc, Extent, Geom )
Returns
<threads>
Dia
<number> Diameter.
Pitch
<number>
Style
<string> "un" or "unj"
Handedness
<string> "right" or "left"
Type
<string> "internal" or "external"
Loc
<anchor | euclidPoint> Location.
Extent
<number> Extent of thread in z direction.
Geom
<boolean> Simple or Complex Geometry for display.
gearDesign( PressureAngle, RPM, PowerKW, NTeethp, GearRatio, UltimateStp, UltimateStg, modElasticityp, modElasticityg, FactorOfSafety, ServiceFactor, OverloadFactor, MountingFactor )
Returns
<groupOfData> Returns a set of numbers including module and hardness in BHN for the set of pinion and gear.
PressureAngle
<number> Pressure angle of the spur gear in degrees.
RPM
<number>The speed of rotation of the pinion(driving gear)attached to the power source in revolutions per minute.
PowerKW
<number>The power developed by the source (motor or engine etc.) in Kilowatts(KW).
NTeethp
<integer>Number of tooth for the pinion(driving gear). The recommended minimum value is 18 for a 20 degree involute pair of gears.
GearRatio
<number>The gear ratio required for the application.
UltimateStp
<number>The Ultimate tensile strength in MPa(N/mm^2) for the pinion material.
UltimateStg
<number>The Ultimate tensile strength in MPa(N/mm^2) for the gear material.
modElasticityp
<number>The modulus of elasticity in MPa(N/mm^2) for the pinion material.
modElasticityg
<number>The modulus of elasticity in MPa(N/mm^2) for the gear material.
FactorOfSafety
<number>The factor of safety required in the present application. The recommended values are above 1.5.
ServiceFactor
<number>Based on the different applications, the service factors are tabulated below.

 

Type of driven machine

Value of the Service Factor based on the Source of Power

Electric Motor

Turbine/Multi Cylinder Engine

Single Cylinder Engine

Generators – feeding mechanisms – belt conveyors – blowers – compressors and agitators and mixers

 

1.10

 

1.25

 

1.50

Machine tools – hoists and cranes – rotary drives – piston pumps – distribution pumps

 

1.25

 

1.50

 

1.75

Blanking and shearing presses – rolling mills – centrifuges – steel work machinery

 

1.75

 

2.00

 

2.25
OverloadFactor
<number>The recommended values for the overload correction factor based on the type of applications are tabulated below.

 

Source of Power

Overload Correction Factor based on the type of driven machinery

Uniform

Moderate Shock

Heavy Shock

Uniform

 1.10

 1.25

 1.50

Light Shock

 1.25

 1.50

 1.75

Medium Shock

 1.75

 2.00

 2.25
MountingFactor
<number> The values for the mounting correction factor based on the characteristics of support and the "expected" face-width in mm. are tabulated below.
PS : The actual value of the face width in mm. is assumed as 10 times the calculated module.

 

Characteristics of Support

Values of Mounting Correction factor based on expected Face width (mm.)

0 to 60

152

228

406 up

Accurate mountings, small bearing clearances, minimum deflection, precision gears.

 1.3

1.4

 1.5

1.8

Less rigid mountings, less accurate gears, contact across the full face.

 1.6

1.7

1.8

2.2

Accuracy and mounting such that less than full-face contact exists.

Over 2.2
spurGear( PressureAngle, Module, NTeeth, Width, Location )
Returns
<spurGear>

 
PressureAngle
<number> Pressure angle of the spur gear in degrees.
Module
<number> module of the spur gear.
NTeeth
<integer>Number of Teeth for the gear
Width
<number>Width or thickness in mm for the gear in z
Location
<anchor | euclid point>This parameter is optional. It is the new location and orientation for the spur gear.The gear's origin will be aligned with the location anchor
flatDiameter( Thread )
Returns
<number> Returns the diameter of a thread as measured to the flat.
Thread
<thread> The thread to examine.
featureGroup( Location, Features, Ordered )
Returns
<featureGroup>
Location
<euclidPoint | anchor> Point or anchor location.
Features
<arrayOf features> Array of features.
Ordered
<boolean> Ordered array or not.
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