SOLIDWORKS Part Modeling PDF

Unit – III PART M ODELLING 3.1 Introduction The 3D part is the basic building block of the parametric modelling software. Features are the individual shapes that, when combined, make up the part. è Parent and Child Relations : Feat...

Unit – III PART M ODELLING 3.1 Introduction The 3D part is the basic building block of the parametric modelling software. Features are the individual shapes that, when combined, make up the part. è Parent and Child Relations : Features are normally built upon other existing features. For example, you create a base extrude feature and then create additional features such as a boss or cut extrude. The original base extrude is the parent feature; the boss or cut extrude is a child feature. The existence of a child feature depends on the parent. 3.2 Reference Geometry Reference geometry defines the shape or form of a surface or a solid. Reference geometry includes items such as planes, axes, coordinate systems, and points. You can use reference geometry in the creation of several kinds of features. For example : è Planes are used in lofts and sweeps. è An axis is used in a circular pattern. 3.2.1 Reference Planes You can create planes in part or assembly documents. You can use planes to sketch, to create a section view of a model, for a neutral plane in a draft feature, and so on. To create a reference plane : 1) Click Plane (Reference Geometry toolbar) or Insert > Reference Geometry > Plane. 2) In the PropertyManager, select an entity for First Reference. 3) The software creates the most likely plane based on the entity you select. You can select options under First Reference, such as Parallel, Perpendicular, and so forth to modify the plane. 4) To clear references, right-click the item in First Reference and click Delete. 5) Select a Second Reference and Third Reference as necessary to define the plane. 6) The Message box reports the status of the plane. The plane status must be Fully defined to create the plane. 7) Click. Plane PropertyManager You select geometry and apply constraints to the geometry to define reference planes. 33  Options Description First Reference Select the first reference to define the plane. Based on your selection, other constraint types appear. Coincident Creates a plane that passes through the selected reference. Parallel Creates a plane parallel to the selected plane. Perpendicular Creates a plane perpendicular to the selected reference. Project Projects a singular entity such as a point, vertex, origin, or coordinate system onto a non-planar surface. Parallel to Creates a plane at the selected vertex that is parallel to the current view screen orientation. Tangent Creates a plane tangent to cylindrical, conical, non-cylindrical, and non-planar faces. At angle Creates a plane through an edge, axis, or sketch line at an angle to a cylindrical face or plane. You can specify the Number of planes to create. Offset distance Creates a plane parallel to a plane or face, offset by a specified distance. You can specify the Number of planes to create. Flip Normal Flips the normal vector of the plane. Mid Plane Creates a mid plane between planar faces, reference planes, and 3D sketch planes. Select Mid Plane for both references. Second Reference and Third Reference These sections contain the same options as First Reference, depending on your selections and model geometry. Set these references as needed to create the desired plane. Examples : Parallel Perpendicular Tangent At angle Multiple offset Mid plane 34 3.2.2 Reference point You can create several types of reference points to use as construction objects. You can also create multiple reference points that are a specified distance apart on curves. To create a single reference point : 1) Click Point on the Reference Geometry toolbar, or click Insert > Reference Geometry > Point. 2) In the PropertyManager, select the type of reference point to create. 3) In the graphics area, select the entities to use to create the reference point. 4) You can create reference points at the intersections of the following entities: è An axis and a plane è An axis and a surface, both planar and non-planar è Two axes 5) Click. 3.2.3 Reference Axes You can use an axis in creating sketch geometry or in a circular pattern. To create a reference axis : 1) Click Axis on the Reference Geometry toolbar, or click Insert > Reference Geometry > Axis. 2) Select the axis type in the Axis PropertyManager, then select the required entities for that type. 3) Verify that the items listed in Reference Entities correspond to your selections. 4) Click. 5) Click View > Hide/Show > Axes to see the new axis. Reference Axis PropertyManager The Axis PropertyManager appears when you create a new axis or edit an existing axis. Selections Option Description Reference Entities Displays the selected entities. One Line/Edge/Axis. Select a sketch line, an edge, or axis. Two Planes Select two planar faces. Two Points/Vertices Select two vertices, points, or midpoints. Cylindrical/Conical Face Select a cylindrical or conical face. Point and Face/Plane Select a surface or plane and a vertex point, or midpoint. 35 3.2.4 Coordinate Systems You can define a coordinate system for a part or assembly. Coordinate systems are useful : è With the Measure and Mass Properties tools è When exporting SOLIDWORKS documents to other graphics standards. è When applying assembly mates To create a coordinate system : 1) Click Coordinate System (Reference Geometry toolbar) or Insert > Reference Geometry > Coordinate System. 2) Use the Coordinate System PropertyManager to create the coordinate system. 3) To change your selections, right-click in the graphics area and select Clear Selections. 4) To reverse the direction of an axis, click its Reverse Axis Direction button in the PropertyManager. 5) Click. Coordinate System PropertyManager The Coordinate System PropertyManager appears when you add a new coordinate system to a part or assembly or edit an existing coordinate system. Selections : Options Description Origin Select a vertex, point, midpoint, or the default point of origin on a part or assembly for the coordinate system origin. X axis, Y axis, and Select one of the following for the Axis Direction Reference : Z axis è Vertex, point, or midpoint : Aligns the axis toward the selected point. è Linear edge or sketch line : Aligns the axis parallel to the selected edge or line. è Non-linear edge or sketch entity : Aligns the axis toward the selected location on the selected entity. è Planar face : Aligns the axis in the normal direction of the selected face. Reverse Axis Reverses the direction of an axis. Direction 3.3 Features Toolbar The Features toolbar provides tools for creating model features. The set of features icons is very extensive so not all of them are included on the default Features toolbar. You can customize this toolbar by adding and removing icons to suit your working style and frequent tasks. 36 Tool Description Tool Description Extruded Boss/Base Wrap Revolved Boss/Base Live Section Plane Swept Boss/Base Model Break View Lofted Boss/Base Instant3D Boundary Boss/Base Suppress Thicken Unsuppress Extruded Cut Unsuppress with Dependents Revolved Cut Linear Pattern Swept Cut Circular Pattern Lofted Cut Mirror Feature Boundary Cut Curve Driven Pattern Thickened Cut Sketch Driven Pattern Cut with Surface Table Driven Pattern Fillet Fill Pattern Chamfer Variable Pattern Rib Split Scale Intersect Shell Combine Draft Join Move Face Delete/Keep Body Simple Hole Heal Edges Hole Wizard Imported Geometry Advanced Hole Insert Part Thread Move/Copy Bodies Hole Series Recognize Features Dome FeatureWorks Options Freeform Grid System Deform Convert to Mesh Body Indent 3D Texture Flex Segmented Imported Mesh Body 37 3.4 Extrude Extrude tool is used to extend a sketched profile in one or two directions as either a thin feature or a solid feature. An extrude operation can either add material to a part (in a base or boss) or remove material from a part (in a cut). You can create the following types of extruded features : Extruded Boss/base Feature Extruded Cut Feature Extruded Thin Feature Extruded Surface Feature To create an extrude feature : 1) Create a sketch. You can use a closed profile sketch or an open profile. For cuts, open profile sketches are only valid for Blind or Through All end conditions 2) Click one of the extrude tools : è Extruded Boss/Base on the Features toolbar, or click Insert > Boss/Base > Extrude è Extruded Cut on the Features toolbar, or click Insert > Cut > Extrude è Extruded Surface on the Surfaces toolbar, or click Insert > Surface > Extrude 3) Set the PropertyManager options. 4) Click. Extrude PropertyManager Set the PropertyManager options based on the type of extrude feature. 38 From : Sets the starting condition for the extrude feature. Option Description Sketch Plane Starts the extrude from the plane on which the sketch is located. Surface/Face/Plane Starts the extrude from one of these entities. Vertex Starts the extrude from the vertex you select for Vertex. Offset Starts the extrude on an plane that is offset from the current sketch plane. Set the offset distance in Enter Offset Value. Direction 1 Option Description Direction 1 Determines how the feature extends. Set the end condition type. If necessary, click Reverse Direction to extend the feature in the opposite direction from that shown in the preview. è Blind : Set the Depth. è Through All : Extends the feature from the sketch plane through all existing geometry. è Through All – Both : Extends the feature from the sketch plane through all existing geometry for Direction 1 and Direction 2. è Up to Vertex : Select a vertex in the graphics area for Vertex. è Up to Surface : Select a face or plane to extend to in the graphics area for Face/Plane. è Offset From Surface : Select a face or plane in the graphics area for Face/Plane , and enter the Offset Distance. è Up To Body : Select the body to extrude to in the graphics area for Solid/Surface Body. è Mid Plane : Set the Depth. Direction of Select a direction vector in the graphics area to extrude the sketch in a Extrusion direction other than normal to sketch profile. Draft On/Off Adds draft to the extruded feature. Set the Draft Angle. Select Draft outward if necessary. Direction 2 : Set these options to extrude in both directions from the sketch plane. The options are the same as Direction 1. Thin Feature : è Use the Thin Feature options to control the extrude thickness (not the Depth ). è A Thin Feature base can be used as a basis for a sheet metal part. è Thin Feature is required when using an open contour sketch. Thin Feature is optional when using a closed contour sketch. 39  Option Description Type Sets the type of thin feature extrude. è One-Direction : Sets the extrude Thickness in one direction (outward) from the sketch. è Mid-Plane : Sets the extrude Thickness equally in both directions from the sketch. è Two-Direction : Allows you to set different extrude thicknesses for Direction 1 Thickness and Direction 2 Thickness. Cap Covers the end of the thin feature extrude, creating a hollow part. You must also specify ends the Cap Thickness. This options is available only for the first extruded body in a model. Selected Contours Selected Allows you to use a partial sketch to create extrude features from open or Contours closed contours. Select sketch contours and model edges in the graphics area. 3.5 Revolves Revolves add or remove material by revolving one or more profiles around a centerline. You can create revolved boss/bases, revolved cuts, or revolved surfaces. The revolve feature can be a solid, a thin feature, or a surface. Sketch Revolved Feature To create a revolve feature: 1) Create a sketch that contains one or more profiles and a centerline, line, or edge to use as the axis around which the feature revolves. 2) Click one of the following revolve tools: è Revolved Boss/Base (Features toolbar) or Insert > Boss/Base > Revolve. è Revolved Cut (Features toolbar) or Insert > Cut > Revolve. è Revolved Surface (Surfaces toolbar) or Insert > Surface > Revolve. 3) In the PropertyManager, set the options. 4) Click. 40 Revolve PropertyManager The Revolve PropertyManager appears when you create a new revolve feature, or when you edit an existing revolve feature. Axis of Revolution Axis of Revolution Select an axis around which the feature revolves. This can be a centerline, line, or an edge, depending on the type of revolve feature you create. Direction1 : Defines the revolve feature in one direction from the sketch plane. Revolve Sets the end condition of the revolve feature relative to the sketch plane. To reverse the Type revolve direction, click Reverse Direction. Select one of these options: è Blind : Creates the revolve in one direction from the sketch. Set the angle covered by the revolve in Direction 1 Angle. è Up to Vertex : Creates the revolve from the sketch plane to the vertex you specify in Vertex. è Up to Surface : Creates the revolve from the sketch plane to the surface you specify in Face/Plane. è Offset from Surface : Creates the revolve from the sketch plane to a specified offset from the surface you specify in Face/Plane. Set the offset in Offset Distance. To offset in the opposite direction, select Reverse offset. è Mid-Plane : Creates the revolve in the clockwise and counterclockwise directions from the sketch plane, which is located at the middle of the revolve Direction 1 Angle. Merge Merges resultant body into an existing body if possible. If not selected, the feature creates result a distinct solid body. Direction2 : After completing Direction1, select Direction2 to define the revolve feature in the other direction from the sketch plane. The options are the same as in Direction1. Thin Feature Type Defines the direction of thickness. Select one of these options: è One-Direction : Adds the thin-walled volume in one direction from the sketch. To reverse the direction in which the thin-walled volume is added, click Reverse Direction. è Mid-Plane : Adds the thin-walled volume using the sketch as the middle, and applying thin-walled volume equally on both sides of the sketch. è Two-Direction : Adds the thin-walled volume on both sides of the sketch. Direction 1 Thickness adds thin-walled volume outward from the sketch. Direction 2 Thickness adds thin-walled volume inward from the sketch. Direction 1 Sets the thin-walled volume thickness for One-Direction and Mid-Plane thin Thickness feature revolves. Selected Contours : Use this option when you create a revolve using multiple contours. 41 3.6 Sweeps Sweep creates a base, boss, cut, or surface by moving a profile (section) along a path. A sweep can be simple or complex. Profile & Path Swept Solid To create a sweep : 1) Sketch a closed, non-intersecting profile on a plane or a face. 2) Create the path for the profile to follow. Use a sketch, existing model edges, or curves. 3) Click one of the following: è Swept Boss/Base on the Features toolbar or Insert > Boss/Base > Sweep è Swept Cut on the Features toolbar or Insert > Cut > Sweep è Swept Surface on the Surfaces toolbar or Insert > Surface > Sweep 4) In the PropertyManager : è Select a sketch in the graphics area for Profile. è Select a sketch in the graphics area for Path. è Set the other PropertyManager options. 5) Click. Swept Boss/Base PropertyManager Set the PropertyManager options based on the sweep boss/base feature. Sketch Profile : Creates a sweep by moving a 2D profile along a 2D or 3D sketch path. Profile Sets the profile (section) used to create the sweep. You can select faces, edges, and curves directly from models as sweep profiles. The profile must be closed for a base or boss sweep feature. Path Sets the path along which the profile sweeps. Select the path in the graphics area or FeatureManager design tree. The path can be open or closed, and can be a set of sketched curves contained in one sketch, a curve, or a set of model edges. The start point of the path must lie on the plane of the profile. 42 The following controls are available when the path extends through a profile. Direction 1 Creates a sweep for one side of the path. Bidirectional Creates a sweep that extends in both directions of the path from a sketch profile. Direction 2 Creates a sweep for the other direction of the path. Circular Profile : Creates a solid rod or hollow tube along a sketch line, edge, or curve directly on a model. Profile Sets the profile (section) used to create the sweep. Select the profile in the graphics area or FeatureManager design tree. The profile must be closed for a base or boss sweep feature. Diameter Specifies the diameter of the profile. 3.7 Helix and Spiral You can create a helix or spiral curve in a part. The curve can be used as a path or guide curve for a swept feature, or a guide curve for a lofted feature. Creating a Helix or Spiral You can create a helix or spiral curve in a part. In a part, do one of the following : 1) Open a sketch and sketch a circle. 2) Select a sketch that contains a circle. The diameter of the circle controls the starting diameter of the helix or spiral. 3) Click Helix and Spiral (Curves toolbar) or Insert > Curve > Helix/Spiral. 4) Set values in the Helix/Spiral PropertyManager. 5) Click. Spiral Swept with Circular Profile option Helix Constant pitch Taper angle Swept cut 43 Helix/Spiral PropertyManager Defined By : Specifies the type of curve (helix or spiral) and which parameters to use to define the curve. Select one of the following : Pitch and Revolution Creates a helix defined by Pitch and Revolutions. Height and Revolution Creates a helix defined by Height and Revolutions. Height and Pitch Creates a helix defined by Height and Pitch. Spiral Creates a spiral defined by Pitch and Revolutions. Parameters : Sets parameters of the curve. Your selection under Defined By determines which parameters are available. Constant pitch (Helix only.) Creates a helix with a constant pitch. Variable pitch (Helix only.) Creates a helix with a pitch that varies based on the region parameters you specify in the table below. Region (Variable pitch helix only). Sets the number of revolutions (Rev), height (H), parameters diameter (Dia), and pitch (P) for regions along the helix. Parameters that are inactive or for information only are shown in gray. Height (Helix only.) Sets the height. Pitch For helixes: Sets the distance between turns. For spirals: Sets the radial distance between revolutions of the curve. Revolutions Sets the number of turns. Reverse direction For helixes: Extends the helix backwards from the point of origin. For spirals: Creates an inward spiral. Start angle Sets where to start the first turn on the sketched circle. Clockwise Sets the direction of the turns to clockwise. Counterclockwise Sets the direction of the turns to counterclockwise. Taper Helix : Creates a tapered helix. (Available only for constant pitch helixes.) Select Taper Helix. Taper Angle Sets the angle of the taper. Taper outward Tapers the helix outward. 3.8 Lofts Loft creates a feature by making transitions between profiles. A loft can be a base, boss, cut, or surface. You create a loft using two or more profiles. Only the first, last, or first and last profiles can be points. All sketch entities, including guide curves and profiles, can be contained in a single 3D sketch. For a solid loft, the first and last profiles must be model faces or faces created by split lines, planar profiles, or surfaces. 44 To create lofts : 1) Do one of the following: è Click Lofted Boss/Base (Features toolbar) or Insert > Boss/Base > Loft. è Click Lofted Cut (Features toolbar) or Cut > Loft > Insert. è Click Lofted Surface (Surfaces toolbar) or Insert > Surface > Loft. 2) Set the options in the PropertyManager. 3) Click. Sketch profile Loft 3.9 Dome You can create one or more dome features simultaneously on the same model. To create a dome : 1) Click Dome on the Features toolbar, or click Insert > Features > Dome. Circular Dome Elliptical Dome Continuous Dome Dome PropertyManager Options Faces to Dome Select one or more planar or non-planar faces. Distance Set a value for the distance by which the dome expands. Reverse Direction Click to create a concave dome (default is convex). 45  Constraint Point or Control the dome feature by selecting a sketch that contains points to Sketch constrain the shape of the sketch. Direction Click Direction , and select a direction vector from the graphics area to extrude the dome in a direction other than normal to the face. Elliptical dome Specify an elliptical dome for cylindrical or conical models. Continuous dome Specify a continuous dome for polygonal models. Show preview Check for a preview. 3.10 Shells The shell tool hollows out a part, leaves open the faces you select, and creates thin-walled features on the remaining faces. If you do not select any face on the model, you can shell a solid part, creating a closed, hollow model. You can also shell a model using multiple thicknesses. Before shell After shell To create a shell feature of uniform thickness : 1) Click Shell (Features toolbar) or Insert > Features > Shell. 2) In the PropertyManager, under Parameters : è Set Thickness to set the thickness of the faces you keep. è Select one or more faces in the graphics area for Faces to remove. è When you shell a multibody part, the Solid Body box appears. After you select a face to remove, or a body, the box disappears. è Select Shell outward to increase the outside dimensions of the part. è Select Show preview to display a preview of the shell feature. 3) Click. 3.11 Drafts Draft tapers faces using a specified angle to selected faces in the model. One application is to make a molded part easier to remove from the mold. You can insert a draft in an existing part or draft while extruding a feature. You can apply draft to solid or surface models. You can also apply a draft angle as a part of an extruded base, boss, or cut. 46  Before draft After draft (5O) To draft a model face : 1) Click Draft (Features toolbar) or Insert > Features > Draft. 2) Set the options in the PropertyManager. 3) Click Detailed Preview to preview the draft. 4) Click. 3.12 Ribs Rib is a special type of extruded feature created from open or closed sketched contours. It adds material of a specified thickness in a specified direction between the contour and an existing part. You can create a rib using single or multiple sketches. You can also create rib features with draft, or select a reference contour to draft. Before rib After rib To create a rib : 1) Sketch the contour to use as the rib feature on a plane that intersects the part, or is parallel or at an angle to an existing plane. 2) Click Rib (Features toolbar) or Insert > Features > Rib. 3) Set the PropertyManager options. 4) Click. 47 3.13 Wrap You can choose between two methods to create a wrap feature. è The Analytical method wraps a sketch onto a planar or non-planar face. è The Spline Surface method wraps a sketch on any face type. To create a wrap feature using the Analytical method : 1) Select the sketch you want to wrap from the FeatureManager design tree. 2) The sketch to wrap can contain multiple, closed contours only. You cannot create a wrap feature from a sketch that contains any open contours. 3) Click Wrap on the Features toolbar, or click Insert > Features > Wrap. 4) In the PropertyManager, under Wrap Type, Select an option: Option Description Creates a raised feature on the face. Emboss Creates an indented feature on the face. Deboss Creates an imprint of the sketch contours on the face. Scribe 5) Under Wrap Method, select Analytical. 6) Select a non-planar face in the graphics area for Face for Wrap Sketch , under Wrap Parameters. 7) Set a value for Thickness. 8) Select Reverse direction, if necessary. 9) If you select Emboss or Deboss , you can select a line, linear edge, or plane to set a Pull Direction. For a line or linear edge, the pull direction is the direction of the selected entity. For a plane, the pull direction is normal to the plane. 10) To wrap the sketch normal to the sketch plane, leave Pull Direction blank. 11) Click. 3.14 Intersect You can intersect solids, surfaces, and planes to modify existing geometry, or to create new geometry with the Intersect tool. For example, you can add open surface geometry to a solid, remove material from a model, or you can create geometry from an enclosed cavity. You can also merge solids that you define with the Intersect tool, or cap some surfaces to define closed volumes. 48 To create geometry from solids, surfaces, or planes in a part : 1) Click Intersect (Features toolbar) or Insert > Features > Intersect. 2) Select solids, surfaces, or planes. 3) Click Intersect. 4) Select the regions to exclude and click. 3.15 Holes è You can create various types of hole features in a model. You place a hole and set a depth on a planar face. You can specify its location by dimensioning it afterward. è In general, it is best to create holes near the end of the design process. This helps you avoid inadvertently adding material inside an existing hole. Also, if you are creating a simple hole, which does not require additional parameters, use Simple Hole. è The Hole Wizard introduces additional parameters that are not required with simple holes. Simple Hole provides better performance than Hole Wizard for simple holes. Hole Wizard creates holes with complex profiles, such as Counterbore or Countersunk. è You can also define holes from the near and far side faces with the Advanced Hole tool. Hole element flyouts help guide the process. To create and position a simple hole : 1) Select a planar face on which to create the hole. 2) Click Simple Hole (Sheet Metal toolbar) or Insert > Features > Simple Hole. 3) In the PropertyManager, set the options. 4) Click to create the simple hole. 5) Right-click the hole feature in the model or the FeatureManager design tree, and select Edit Sketch. 6) Add dimensions to position the hole. You can also modify the hole diameter in the sketch. 7) Exit the sketch or click Rebuild. è To change the diameter, depth, or type of the hole, right-click the hole feature in the model or the FeatureManager design tree, and select Edit Feature. Make the required changes in the PropertyManager, and click. 49 3.16 Hole Wizard You can use the Hole Wizard to create customized holes of various types. To create hole wizard holes : 1) Create a part and select a surface 2) Click Hole Wizard (Features toolbar) or Insert > Features > Hole > Wizard 3) Set the PropertyManager options 4) Click. You can create the following types of Hole Wizard holes : è Counterbore è Countersink è Hole è Straight Tap è Tapered Tap è Legacy When you create a hole using the Hole Wizard, the type and size of the hole appears in the FeatureManager design tree. 3.17 Threads You can create helical threads on cylindrical edges or faces using profile sketches and store custom thread profiles as library features. The two methods of creating a thread feature are cut thread and extrude thread. The direction of the thread can be right-handed or left-handed. You can design a multiple start thread and align the thread trim to a start face or end face. Creating a Thread You can select any shape or size on a thread profile. The diameter of a hole or shaft does not determine the thread profile. Internal Thread External Thread 50 To create a thread: 1) Open a model with a cylindrical part and click Insert > Features > Thread. 2) In the graphics area, select a circular edge. 3) In the PropertyManager, set options and values. 4) Click. Specification Type Select one of the following: è Metric Tap : Creates internal threads. è Metric Die : Creates external threads. Size Select a thread size. Displays configurations in the library part file from the Type list. Override Click to manually override the diameter of the cylindrical face or helix. Enter Diameter a value or start with = (equal sign) to create an equation. Override Click to manually override the pitch of the helix. Enter a value or start with = Pitch (equal sign) to create an equation. Thread Select one of the following: Method è Cut Thread : Creates a swept cut using the profile è Extrude Thread : Creates a swept boss using the profile. Creating hexagonal nut and bolt To create hexagonal nut of M12 x 1 mm pitch : 1) Select Front Plane and click Extruded Boss/Base. 2) Draw Hexagon of side 12 mm and extrude to a Depth 12 mm. (Fig.1) Fig.1 Fig.2 Fig.3 Fig.4 3) Select the front face and click Sketch. Draw circle touching the edges of the hexagon. Use tangent relation between the circle and edges of hexagon. (Fig.2) 4) Click Extruded Cut and Select the circle. Set the following options in the PropertyManager. è Depth : Draft :. 51  5) Similarly Extruded Cut on the other face. (Fig.3) 6) Select the front face and click Sketch. Draw a circle of j12 mm. Extruded Cut the circle to Depth 12 mm. 7) Create internal threads. Click Insert > Features > Thread. 8) Select the j12 mm circle and set the following options : è Depth : 15mm Size : è Diameter : 12mm Pitch : 1mm (Fig.4) To create hexagonal bolt of M12 x 1 mm pitch and 40 mm long : 1) Select Front Plane and click Extruded Boss/Base. 2) Draw Hexagon of side 12 mm and extrude to a Depth 12 mm. (Fig.1) Fig.1 Fig.2 Fig.3 3) Select the front face and click Sketch. Draw circle touching the edges of the hexagon. Use tangent relation between the circle and edges of hexagon. 4) Click Extruded Cut and Select the circle. Set the following options in the Property Manger. è Depth : Draft :. (Fig.1) 5) Select the other face and click Sketch. Draw a circle of j12 mm. Extrude the circle to a Depth 40 mm. 6) Create Chamfer of 1 mm at the end. (Fig.2) 7) Create external threads. Click Insert > Features > Thread. Select the j12 mm circle and set the following options : è Depth : 40mm Size : è Diameter : 12mm Pitch : 1mm (Fig.3) You can also insert bolts and nuts from SOLIDWORKS Design Library during assembly. 52 To insert a Toolbox component into an assembly : 1) Open the assembly. 2) In the Design Library task pane, under Toolbox , expand the standard, category, and type of the component to insert. 3) Images and descriptions of available components appear in the task pane. 4) Drag a component into the assembly. If you drop a component near an appropriate feature, a SmartMate positions the part in the assembly. For example, if you drag a bolt and drop it onto a hole, the SmartMate mates the bolt to the hole. 5) Set the options In the PropertyManager. 6) Click. Creating square thread To draw square thread of 20 mm x 5 mm pitch to a length of 75 mm : 1) Click Extruded Boss/Base and select Front Plane. 2) Draw circle of j20 mm and extrude to a Depth 75 mm. 3) Select the left end of the cylinder and click Sketch. Draw a circle of j20 mm. 4) Select the circle and click Helix and Spiral (Curves toolbar) or Insert > Curve > Helix/Spiral. 5) Set the following values in the Helix/Spiral PropertyManager. è Defined by : Height : Pitch : 6) Click. 53  7) Select Right Plane and click Sketch. Draw a Center Rectangle of size 2.5 mm x 5 mm. 8) Select center-point of the rectangle and start point of the helix by pressing Shift. Apply Pierce relation from the PropertyManager. 9) Click Swept Cut on the Features toolbar or Insert > Cut > Sweep 10) Set the following values in the Helix/Spiral PropertyManager. è Sketch : Select the rectangle è Profile : Select the Helix Biderectional 11) Click. 3.18 Pattern Pattern repeats the selected features in an array based on a seed feature. You can create a linear pattern, a circular pattern, a curve driven pattern, a fill pattern, or use sketch points or table coordinates to create the pattern. Linear Patterns You can use linear patterns to create multiple instances of one or more features that you can space uniformly along one or two linear paths. Seed feature Linear pattern Linear pattern (one direction) (two directions) To create a linear pattern: 1) Create one or more features to replicate. 2) Click Linear Pattern (Features toolbar) or Insert > Pattern/Mirror > Linear Pattern. 3) Set the PropertyManager options. 4) Click. Circular Patterns Use circular patterns to create multiple instances of one or more features that you can space uniformly around an axis. To create a circular pattern: 1) Create one or more features to replicate. 2) Click Circular Pattern (Features toolbar) or Insert > Pattern/Mirror > Circular Pattern. 3) Set the PropertyManager options. 4) Click. 54  Cut extrude feature applied Cut extrude feature using the Cut extrude feature using the to all multibody parts circular pattern applied to circular pattern applied to all single body bodies 3.19 Move/Copy Bodies In multibody parts, you can move, rotate, and copy solid and surface bodies, or place them using mates. To move, copy, rotate, or mate a solid or surface body: 1) Click Move/Copy Bodies (Features toolbar) or Insert > Features > Move/Copy. 2) The Move/Copy Body PropertyManager appears. It displays one of two pages: Translate/Rotate Specify parameters to move, copy, or rotate bodies. Constraints Apply mates between bodies. (Note: Refer 4.3 for types of mates) 3) Click Translate/Rotate or Constraints at the bottom of the PropertyManager (if necessary) to switch to the page you want. 4) Set options in the PropertyManager. 3.20 Combine Bodies In a multibody part, you can combine multiple solid bodies to create a single-bodied part or another multibody part. You can add or subtract bodies, or keep material that is common to the selected bodies. In a multibody part, you can combine multiple bodies to create a single body. You can only combine bodies contained within one multibody part file. You cannot combine two separate parts. However, you can create a multibody part by using Insert Part to place one part into the other part file. Then you can use Combine on the multibody part. To combine bodies: 1) Click Combine (Features toolbar) or Insert > Features > Combine. 2) In the PropertyManager, under Operation Type, select of the following: è Add: to combine multiple bodies to create a single body è Subtract: to subtract one or more bodies from another body. è Common: to create a body defined by the intersection of multiple bodies. 3) For Bodies to Combine, select the bodies to combine. 55  4) You can select bodies in the graphics area or the Solid Bodies folder in the FeatureManager design tree. 5) Click Show Preview to preview the feature. 6) Click. Add Combines solids of all selected bodies to create a single body. Subtract Removes overlapping material from a selected main body. Common Removes all material except that which overlaps. 3.21 Editing an Existing Feature To edit an existing feature: è Right-click a feature in the Feature Manager design tree, or right-click a feature in the graphics area, and select Edit Feature. 56  Unit – IV ASSEMBLY 4.1 Introduction You can build complex assemblies consisting of many components, which can be parts or other assemblies, called subassemblies. For most operations, the behavior of components is the same for both types. Adding a component to an assembly creates a link between the assembly and the component. When SOLIDWORKS opens the assembly, it finds the component file to show it in the assembly. Changes in the component are automatically reflected in the assembly. 4.2 Approaches in assemblies The following approaches are used to create assemblies; 1) Bottom-up design 2) Top-down design 1) Bottom-up Design è Bottom-up design is the traditional method. You first design and model parts, then insert them into an assembly and use mates to position the parts. To change the parts, you must edit them individually. These changes are then seen in the assembly. è Bottom-up design is the preferred technique for previously constructed, off-the-shelf parts, or standard components like hardware, pulleys, motors, etc. These parts do not change their shape and size based on your design unless you choose a different component. 2) Top-down Design è In Top-down design, shapes, sizes, and locations of parts can be designed in the assembly itself. For example, you can model a motor bracket so it is always the correct size to hold a motor, even if you move the motor. SOLIDWORKS automatically resizes the motor bracket. This capability is particularly helpful for parts like brackets, fixtures, and housings, whose purpose is largely to hold other parts in their correct positions. è The advantage of top-down design is that much less rework is needed when design changes occur. The parts know how to update themselves based on the way you created them. 4.3 Creating assemblies To create a new assembly : 1) Click New (Standard toolbar) or File > New and select Assembly. 2) An assembly opens with the Begin Assembly PropertyManager active. 3) Select the parts or assembly from the list, or click Browse to open existing documents. 4) Use suitable Mates to properly align and assemble the parts. 57 To create an assembly from a part : 1) Click Make Assembly from Part/Assembly (Standard toolbar) or File > Make Assembly from Part. 2) An assembly opens with the Insert Component PropertyManager active. 3) Click in the graphics area to add the parts to the assembly. 4) Use suitable Mates to properly align and assemble the parts. To insert parts : 1) Click Insert Components (Assembly toolbar) or Insert > Component > Existing Part/Assembly. 2) Previously saved documents that are currently open appear under Part/Assembly to Insert. 3) Click Browse. In the dialog box, select a component and then click Open. 4) In the graphics area, a preview of the component is attached to the pointer. If necessary, rotate the component using Rotate Context Toolbar 5) In the graphics area, click to place the component. 6) Similar insert all the components of an assembly. Each component is inserted where you clicked to place it. 4.4 Mates Mates create geometric relationships between assembly components. As you add mates, you define the allowable directions of linear or rotational motion of the components. You can move a component within its degrees of freedom, visualizing the assembly's behavior. Some examples include : è A coincident mate forces two planar faces to become coplanar. The faces can move along one another, but cannot be pulled apart. è A concentric mate forces two cylindrical faces to become concentric. The faces can move along the common axis, but cannot be moved away from this axis. 4.4.1 Adding Mates To add a mate : 1) Click Mate (Assembly toolbar), or click Insert > Mate. 2) In the PropertyManager, under Mate Selections, select the entities that you want to mate together for Entities to Mate. 3) Click on the Mate type and Click. 58 4.4.2 Mate PropertyManager You add or edit mates in the Mate PropertyManager. Mate Selections Entities to Specifies the entities that you want to mate. Use the Alt key to temporarily Mate hide a front face when you need to select an hidden face (behind the front face) for mates. The components must be displayed in Shaded or Shaded with Edges modes. Move the cursor over a face and press Alt. The face is temporarily hidden. Multiple Mates multiple components to a common reference in a single operation. mate mode Standard Mates All the mate types are shown in the PropertyManager, but only the mates that are applicable to the current selections are available. Coincident Positions the selected faces, edges, and planes so that they share the same plane. Positions two vertices so that they touch. Parallel Places the selected items at a constant distance apart from each other. Perpendicular Places the selected items at a 90° angle to each other. Tangent Places the selected items tangent to each other. At least one selection must be a cylindrical, conical, or spherical face. Concentric Places the selections so that they share the same centerline. Lock Maintains the position and orientation between two components. Distance Places the selected items with the specified distance between them. Angle Places the selected items at the specified angle to each other. Mate Changes the mate alignment. alignment è Aligned : Vectors normal to the selected faces point in the same direction. è Anti-Aligned : Vectors normal to the selected faces point in opposite directions. Advanced Mates Profile Center-aligns rectangular and circular profiles to each other and fully defines Center the components. Symmetric Forces two similar entities to be symmetric about a plane or planar face. Width Constrains a tab between two planar faces. 59  Path Mate Constrains a selected point on a component to a path. Linear/Linear Establishes a relationship between the translation of one component and the Coupler translation of another component. Limit Allows components to move within a range of values for distance and angle mates. Mechanical Mates Cam Forces a cylinder, plane, or point to be coincident or tangent to a series of tangent extruded faces. Slot Constrains the movement of a bolt or a slot within a slot hole. Hinge Limits the movement between two components to one rotational degree of freedom. Gear Forces two components to rotate relative to one another about selected axes. Rack Pinion Linear translation of one part (the rack) causes circular rotation in another part (the pinion), and vice versa. Screw Constrains two components to be concentric, and adds a pitch relationship between the rotation of one component and the translation of the other. Universal The rotation of one component (the output shaft) about its axis is driven by the Joint rotation of another component (the input shaft) about its axis. 4.4.3 Example Part – 1 Part – 2 Assembly To assemble Part – 1 and Part – 2 together, the following conditions must be satisfied : 1) Edge – 1 and Edge – 2 must be concentric. 2) Edge – 3 and Edge – 4 must be concentric 3) Face – 1 and Face – 2 must touch (coincide) each other. 60 Therefore, 1) Click Mate (Assembly toolbar), or click Insert > Mate. 2) Select Edge – 1 and Edge – 2. In the PropertyManager, click under Standard Mate and Click. 3) Select Edge – 3 and Edge – 4. In the PropertyManager, click under Standard Mate and Click. 4) Select Face – 1 and Face – 2. In the PropertyManager, click under Standard Mate and Click. 4.5 Subassemblies When an assembly is a component of another assembly, it is referred to as a subassembly. You can nest subassemblies in multiple levels, to reflect the hierarchy of your design. Creating a Subassembly There are several ways to create a subassembly : è You can create an assembly document as a separate operation, then make it a subassembly by inserting it as a component in a higher-level assembly. è You can insert a new, empty subassembly at any level of the assembly hierarchy while you are editing a top-level assembly, then add components to it in a variety of ways. è You can form a subassembly by selecting a group of components that are already in the assembly. This creates a subassembly and adds components to it in a single step. 4.6 Rebuild When you switch back to the assembly window after editing a component in a separate window, a message asks if you want to rebuild now. è Select Yes or No. Optionally, select Don't show again. Yes Rebuilds the assembly to incorporate the changes you made to the component. No Skips the rebuild of the assembly. Don't show again Suppresses the message. You can specify: Always Rebuild : Select Yes and Don't show again. Never Rebuild : Select No and Don't show again. To rebuild the assembly : è Click Rebuild (Standard toolbar) or Edit > Rebuild. 4.7 Isolate è You can use Isolate to set the visibility to hidden, transparent, or wireframe for components that are not selected, enabling you to focus on the selected components. 61  è You can Isolate parts or subassemblies to edit them in the context of the assembly. You can isolate components that share a mate. è Use the Isolate pop-up toolbar to change the visibility of the hidden components to Wireframe, Transparent, or Hidden. The transparency used when editing a component in the context of an assembly is not used when Isolate is active. To Isolate components : 1) Select the components to isolate in the graphics area or the FeatureManager design tree. 2) Click View > Display > Isolate, or right-click and click Isolate. 3) To isolate components that share a mate, right-click the mate in the FeatureManager design tree and click Isolate. 4) The removed components change their display state to hidden, wireframe, or transparent. 5) Select a component to edit and click Edit Part or Edit Assembly. 6) When you finish working on the isolated components, click Exit Isolate on the Isolate pop-up toolbar. 7) The model returns to its original display state. 4.8 Creating Exploded Views in Assemblies You create exploded views by selecting and dragging parts in the graphics area, creating one or more explode steps. To create an exploded view : 1) Click Exploded View (Assembly toolbar) or Click Insert > Exploded View. 2) Select one or more components. Rotation and translation handles appear in the graphics area. 3) Drag a translation or rotation handle to move selected components. 4) Modify explode options : 62  Option Description Reverses the translation direction. Reverse Direction Specifies the translation distance. Explode Distance Reverses the rotation direction. Reverse Direction Specifies the rotation angle. Rotation Angle 5) Click Done. 6) Similarly select other components and drag the translation or rotation handle as required. Click Done. 7) Click when completed. 4.8.1 Radial Explode You can explode components aligned radially/cylindrically about an axis in one step. You can explode radially by diverging along an axis. To radially explode components about an axis : 1) In an assembly, click Exploded View (Assembly toolbar) or Insert > Exploded View. 2) In the Explode PropertyManager, under Add a Step, click Radial step. 3) In Explode Step Components , select the components to explode. 4) In the graphics area, drag the handle and release. 5) Click. 4.8.2 Exploding and Collapsing an Exploded View An exploded view is stored with the configuration in which it is created. Each configuration can have multiple exploded views. To explode and collapse an exploded view : 1) In the ConfigurationManager tab , expand the configuration. 2) Right-click the Exploded View feature, and click Explode or Collapse. 3) To animate the exploding and collapsing of the view, right-click Exploded View , and click Animate explode or Animate collapse. The Animation Controller pop-up toolbar appears and provides basic controls over the animation. 63 4.9 Appearances An appearance defines the visual properties of a model, including color and texture. Appearances do not affect physical properties, which are defined by materials. In a part, you can add appearances to faces, features, bodies, and the part itself. In an assembly, you can add appearances to components. 4.9.1 Appearance Types You can apply procedural appearances, which wrap around the reference, or textural appearances, which are mapped to the reference. Procedural Textural One color or a blend of colors applied to the An image representing the complex colorings of the entire reference. appearance, mapped to the reference. Use the Examples : Brushed Aluminum and White Mapping tab of the Appearances PropertyManager to High Gloss Plastic. size, orient, and position the appearance on the model. Examples : Fire Brick and Polished Ash. Brushed Aluminum Fire Brick 4.9.2 Changing an Appearance Change an appearance by assigning a predefined appearance or by using the Appearance PropertyManager to edit appearance properties. To assign an appearance : 1) In the Task Pane, click the Appearances, Scenes, and Decals tab. 2) In the Appearances folder, select a category. 3) Do one of the following: è Drag an appearance onto the model. Then from the Appearance Target palette, select the area of the model where you want to assign the appearance. You can pin the Appearance Target palette when adding multiple appearances to improve workflow. è With nothing selected, double-click an appearance to apply it to an entire part or assembly. è With an entity selected (for example, face or feature), double-click an appearance to apply it to the selection. è Drag an appearance onto an item in the FeatureManager. 64 Editing Appearance Properties : To edit appearance properties such as texture mapping and colors, do one of the following: 1) Right-click a model and on the context toolbar, click Appearances. 2) Alt + drag an appearance from the Task Pane. 3) Click Edit Appearance (Heads-up View toolbar) 4) Click Edit > Appearance > Appearance. 5) At the top of the FeatureManager design tree, click to expand the Display Pane. In the Appearances column , right-click and select Appearance. 4.10 Rendering You can generate high quality, realistic renderings, but it can take time depending on your hardware, project complexity, and resolution of renders. To create renderings : 1) Click Output Tools > Render. 2) In the dialog box, on the Render tab: a) In the Smart Control Bar, select a render profile from the drop-down list or create a custom profile. b) Set options. c) Do one of the following: è Click Start Render to begin the rendering process. If you have enabled Show Progress, the Render viewport opens to let you see the rendering è Select Send to Queue in the rendering options and click Send to Queue to add the current rendering to the SOLIDWORKS Visualize Queue so you can render it later. è Click Close to save the current position and composition for later reference. 3) When finished, the rendering is saved in the Images library. 65