Solid Modelling Practical Manual PDF

SOLID MODELLING PRACTICAL MANUAL  Contents Page No. Unit – I : Introduction ………………………………………… 1 Unit – II : Sketching …………………………………………… 15 Unit – III : Part Modelling …………………………………….....

SOLID MODELLING PRACTICAL MANUAL  Contents Page No. Unit – I : Introduction ………………………………………… 1 Unit – II : Sketching …………………………………………… 15 Unit – III : Part Modelling …………………………………….. 33 Unit – IV : Assembly ……………………………………………. 57 Unit – V : Drawing Views …………………………………….. 66 Keyboard Shortcuts ………………………………. 80 EXERCISES PART – A : 3D COMPONENT MODELLING 1. Model – 1 …………………………………………… 85 2. Model – 2 …………………………………………… 91 3. Model – 3 …………………………………………… 95 4. Model – 4 …………………………………………… 99 5. Model – 5 …………………………………………… 103 6. Model – 6 …………………………………………… 107 PART – B : PART MODELLING, ASSEMBLY AND DRAWING VIEWS 1. Revolving Centre ………………………………….. 113 2. Tailstock ……………………………………………. 127 3. Machine Voce ……………………………………… 139 4. Crane Hook ………………………………………… 151 5. Petrol Engine Connecting Rod …………………. 161 6. Pipe Vice ……………………………………………. 169 Question Paper & Allocation of Marks ………. 178  SOLID MODELLING PRACTICAL OBJECTIVES: è Prepare 2D Drawing using sketcher or part modelling of any parametric CAD software. è Generate 3D Solid models from 2D sketch or part modelling of any parametric CAD software. è Prepare assembly of part models using assembly of any parametric CAD software. è Generate orthographic views of 3D solid models/assemblies using drafting of any parametric software. è Plot a drawing for given part model/assembly. DETAILED SYLLABUS Parametric CAD software – sketch – elements – entities: line – circle – arc – ellipse – polygon – text – dimensions – sketch tools – fillet – chamfer – offset – trim – extend – mirror – rotate – block. Part modelling – reference planes – reference point – reference axes – co-ordinate system – extrude – revolve – swept – helix and spiral – lofts – dome – shell – draft – rib – wrap – intersect – holes – patterns. Assembly – approaches – mate – coincident – sub assembly –rebuild – isolate. Drawing views – Save – Plot – model view – exploded view – projected view – section view – import – export – Appearance – rendering. EXERCISES PART A : Draw the given 3D drawing using 3D modelling commands. Model – 1 Model – 2  Model – 3 Model – 4 Model – 5 Model – 6 PART B : Draw the part models and assemble the components using 3D modelling. 1) Revolving Centre 2) Tail stock 3) Machine Vice 4) Crane hook 5) Petrol Engine Connecting Rod 6) Pipe Vice  BOARD EXAMINATION Note : è All the exercises should be completed. All the exercises should be given for examination. The students are permitted to select by lot or the question paper from DOTE should be followed. Record notebook should be submitted during examination. è Two exercises will be given for examination by selecting one exercise in each PART. The printout of exercises of the student work should be submitted with answer paper and the same have to be evaluated as per the allocation. DETAILED ALLOCATION OF MARKS Sl. No. Performance Indicator Marks Part – A : 3D Component Modelling 1. Sketching..................................................... 15 2. 3D Modelling............................................... 15 Part – B : Assembly Drawing Modelling 3. Sketching / Part modelling........................... 20 4. Assembly..................................................... 30 5. Solid Model / Views..................................... 10 6. Viva voce................................................... 10 Total 100  Unit – I IN TR O D U CTIO N 1.1 Parametric Modelling Parametric is a term used to describe a dimension’s ability to change the shape of model geometry as soon as the dimension value is modified. It eliminates the need for a design engineer to constantly redraw a design every time one of the design’s dimensions change. Feature-based is a term used to describe the various components of a model. For example, a part can consists of various types of features such as holes, grooves, fillets, and chamfers. A ‘feature’ is the basic unit of a parametric solid model. Parametric modelling uses the computer to design objects with real world behaviour. Parametric models use feature-based, solid and surface modelling design tools to manipulate the system attributes. One of the most important features of parametric modelling is that attributes that are interlinked automatically change their features. For example, to modify a 3D solid, the designer had to change the length, the breadth and the height. However, with parametric modelling, the designer need only alter one parameter; the other two parameters get adjusted automatically. There are two popular parametric representation models : 1) Constructive Solid Geometry (CSG) : CSG defines a model in terms of combining basic (primitive) and generated (using extrusion and sweeping operation) solid shapes. It uses Boolean operations to construct a model. CSG is a combination of 3D solid primitives (for example a cylinder, cone, prism, rectangle or sphere) that are then manipulated using simple Boolean operations. 2) Boundary Representation (BR) : In BR, a solid model is formed by defining the surfaces that form its spatial boundaries (points, edges, etc.) The object is then made by joining these spatial points. Many Finite Element Method (FEM) programs use this method, as it allows the interior meshing of the volume to be more easily controlled. Advantages of parametric modelling The following are the benefits of 3D parametric modelling over traditional 2D drawings: è Capability to produce flexible designs è 3D solid models offer a vast range of ways to view the model è Better product visualization, as you can begin with simple objects with minimal details è Better integration with downstream applications and reduced engineering cycle time è Existing design data can be reused to create new designs è Quick design improvement, increasing efficiency 1 1.2 Parametric modelling softwares There are many software choices available in the market today for parametric modelling. A few of the leading industry softwares are : 1) SOLIDWORKS SOLIDWORKS is a parametric modelling software owned by Dassault Systemes. It is more popular with engineers as it can easily create electrical, mechanical and automotive components. Key functions and use : è It comes with numerous tools for planning, fabrication, simulations and validation. è In addition to parametric modelling, it also combines CADD (Computer-aided design and drafting), CAM (Computer-aided manufacturing) and CAE (Computer-aided engineering) systems. è The model can be used to estimate cost and manufacturability checks. è With SOLIDWORKS, any advanced designs, from product to mechanical to parametric architecture, can be efficiently planned and created. 2) CATIA CATIA (Computer Aided Three-Dimensional Interactive Application) is also owned by Dassault Systèmes. It is widely used for product design, as parametric modelling software and also PLM (Product Lifecycle Management) software. Its is effectively used in the automotive and aeronautics industries. Key functions and use : è CATIA combines shape sculpting modelling (control-points manipulation) with parametric associativity. This enables designers to explore more design ideas and make relevant changes efficiently. è CATIA can also create and animate virtual human models for better simulation and validation of the product according to user requirements and experience. This is an advantage, especially in the automotive industry where human avatars are needed for ergonomics and safety checks. è This software allows users to venture into virtual reality. è The Collaborate Designer feature also enables creating and visualising linear infrastructures, electrical, piping and mechanical components. 3) Siemens NX (Unigraphics) NX is an advanced high-end CAD/CAM/CAE software owned by Siemens Digital Industries Software. Siemens NX software is a flexible and powerful integrated solution that helps you deliver better products faster and more efficiently. NX delivers the next generation of design, simulation, and manufacturing solutions that enable companies to realize the value of the digital twin. 2 Key functions and use : è Supports every aspect of product development, from concept design through engineering and manufacturing. è NX gives an integrated toolset that coordinates disciplines, preserves data integrity and design intent, and streamlines the entire process. è It is used for design (parametric and direct solid/surface modelling), engineering analysis (static, dynamic, electro-magnetic, thermal, and fluid dynamics), manufacturing finished design by using included machining modules. 4) Creo Parametric (Pro-Engineer) This is a 3D CAD parametric modelling software owned by PTC Inc. (Parametric Technology Corporation). It provides digital solutions to engineering, manufacturing and industrial services. Key functions and use : è The 3D design in Creo is aided by parametric and freestyle surfacing features as well as CAM and Generative design. These features allow curves and surface manipulation by transforming, scaling, stretching, tapering the geometry etc. è The 3D parts and their assembly are created with precise geometry, regardless of the complexity, for efficiency, time and cost-effectiveness. These models can then be accessed for both static and dynamic interference detection. è As Creo Parametric is heavily focused on mechanical and product design, its design capabilities also aid in such design projects. Sheet metal design, piping and cabling designs are all feasible with Creo with its modelling and analysis capabilities. 5) Fusion 360 Fusion 360 is an Autodesk cloud-based 3D modelling software that integrates CAD, CAM and PCB (Printed circuit board) features for product design and manufacturing. Key functions and use : è As a 3D modelling software, it comprehensively includes both parametric and non-parametric, or direct, mesh and surface modelling tools. Therefore the user can choose what to work on based on the need and the skill of the user. è As it is also cloud-based, Fusion 360 allows a design team to centralise all activities and communicate effectively in real-time. è The software also includes electronics and PCB design tools for powerful product modelling. 6) Autodesk Inventor Inventor is used as a parametric modelling and CAD software mainly for mechanical designs. It has an intuitive user interface and is capable of direct, free-form and rules-based design, in addition to parametric modelling. 3 Key functions and use : è Inventor tests the combination of the design by accessing the fit and function and identifying interference patterns before rendering, documentation and planning for manufacturing processes can begin. è Components can be easily placed and assembled with a list of commands available. è It also supports inserting third party design components and models directly into the assembly. 1.3 Starting SOLIDWORKS application The SOLIDWORKS software can be started by è Clicking in Windows Start Menu è Double clicking icon on the Desktop The SOLIDWORKS Welcome dialog box is displayed by default. To open the Welcome dialog box, you can click Welcome SOLIDWORKS from the Standard toolbar. è Home Tab : You can open new and existing documents, view recent documents and folders, and access SOLIDWORKS resources. è Recent Tab : You can view a list of recent documents and folders. è Learn Tab : It gives access for instructional resources to help you learn more about the SOLIDWORKS software. è Alerts Tab : It provides important SOLIDWORKS news. 4 Select an option from Home Tab to open a new or existing document: Option Description Part Opens a new document to create a Part Assembly Opens a new document to create an Assembly Drawing Opens a new document to create engineering drawing. Opens the New SOLIDWORKS Document dialog box, where you can open a Advanced new document based on an alternate template. Open Specifies an existing document to open. After selecting an option, the SOLIDWORKS Graphics window is displayed. 1.4 Solidworks User Interface The figure shows the main elements in SOLIDWORKS user interface. It includes the following : 1) Menu Bar The menu bar contains the SOLIDWORKS menus, a set of Quick Access tools, the SOLIDWORKS Search, and the Help options. 2) Toolbars Toolbars are available for most SOLIDWORKS tools. Named toolbars assist you in performing specific design tasks. To display SOLIDWORKS toolbars: Click Tools > Customize. On the Toolbars tab, select the toolbars to display. 3) Context Toolbars When you select items in the graphics area or Feature Manager design tree, context toolbars appear and provide access to frequently performed actions for that context. 4) Flyout Tool Buttons Similar commands are grouped into flyout buttons on toolbars and the Command Manager. For example, variations of the rectangle are grouped together in a button with a flyout control. 5 6 SOLIDWORKS User Interface 5) Command Manager The Command Manager is a context-sensitive toolbar that dynamically updates based on the toolbar you want to access. By default, it has toolbars embedded in it based on the document type. When you click a tab below the Command Manager, it updates to show that toolbar. For example, if you click the Sketches tab, the Sketch toolbar appears. 6) Manager Pane The left panel of the SOLIDWORKS window manages part and assembly designs, drawing sheets, properties, configurations, and third-party applications. The Command Manager provides access to the SOLIDWORKS tools. 7) Feature Manager Design Tree è Names of features display from top to bottom in the order created in the Feature Manager design tree, unless you reorder them. Features can be considered as components of parts. è The Feature Manager design tree in assemblies displays components (parts or subassemblies and their features), a Mates folder, and assembly features. è The Feature Manager design tree in drawings contains an icon for each sheet. Under each sheet are icons for the sheet format and each view. Under each view are the parts and assemblies that belong to the view. 8) Feature Manager Design Tree Filter It helps to search for specific features of parts and components of assemblies. 9) Property Manager Most sketch, feature, and drawing tools in SOLIDWORKS open a Property Manager in the left panel. The Property Manager displays the properties of the entity or feature so you specify the properties without a dialog box covering the graphics area. 7 10) Configuration Manager The Configuration Manager is a means to create, select, and view multiple configurations of parts and assemblies. 11) DimXpert Manager The DimXpert Manager lists the tolerance features defined by DimXpert for parts. It also displays DimXpert tools that you use to insert dimensions and tolerances into parts. You can import these dimensions and tolerances into drawings. 12) Search You can use SOLIDWORKS Search to find information in documentation and forums. You can also find files and models, and find and run a SOLIDWORKS command with just a few keystrokes. 13) Graphics Area The graphics area displays and lets you manipulate parts, assemblies, and drawings. 14) Reference Triad A triad appears in part and assembly documents to help orient you when viewing models. You can also use it to change the view orientation. You can hide the triad but you cannot use it as an inference point. 15) Triad The triad facilitates manipulating various objects such as 3D sketch entities, parts, certain features, and components in assemblies. 16) Origin The model origin represents the (0,0,0) coordinate of the model. When a sketch is active, a sketch origin represents the (0,0,0) coordinate of the sketch. 8 17) Heads-up View Toolbar It is a transparent toolbar in each viewport provides all the common tools required for manipulating the view. It includes the following : Icon Description Icon Description View Orientation Hide/Show Items Previous View View Planes Redraw View Live Section Planes Zoom to Fit View Axes Zoom to Sheet View Temporary Axes Zoom to Area View Origins Zoom In/Out View Coordinate Systems Zoom to Selection View Datum Reference Frame View Orientation View Curves Rotate View View Sketches Roll View View Grid Turn Camera View 3D Sketch Plane 3D Drawing View View Sketch Dimensions Pan View All Annotations Display Style View Dimension Names Wireframe View Points Hidden Lines Visible View Routing Points Hidden Lines Removed View Parting Lines Shaded with Edges View Lights Shaded View Cameras Draft Quality HLR/HLV View Decals Perspective View Sketch Relations Shadows in Shaded Mode Change Display States Section View View Simulation Symbols 9  Icon Description Icon Description Camera View View Weld Beads Curvature Add Walk-through Zebra Stripes Ambient Occlusion Body Compare Take Snapshot Surface Curvature Combs Filter Modified Components Draft Analysis View Center of Mass Undercut Analysis View Top Level Annotations Parting Line Analysis View Component Annotations RealView Graphics Hide/Show Primary Planes Apply Scene Cartoon Edit Appearance Simulation Display Copy Appearance View Bounding Box Paste Appearance View Component Envelopes Edit Sketch or Curve Color View Top Level Envelopes The View Orientation flyout tool bar can be accessed by pressing SPACEBAR. It consists of the following : Icon Description Icon Description Front Normal To Back Single View Left Two View - Horizontal Right Two View - Vertical Top Four View Bottom Link Views Isometric View Selector Trimetric New View Dimetric 10 18) Task Pane The Task Pane provides access to SOLIDWORKS resources, libraries of reusable design elements, views to drag onto drawing sheets, and other useful items and information. Right-click when the pointer changes to to accept the preview, or click to return to the preview without accepting the values. 19) Confirmation Corner Confirmation Corner is used to accept features. You can Click the OK or Cancel icons that appear in the Confirmation Corner of the SOLIDWORKS graphics area. Click the Exit Sketch icon in the Confirmation Corner to finish the sketch or click the Cancel Sketch icon to discard changes to the sketch. 20) Status Bar The status bar at the bottom of the SOLIDWORKS window provides information related to the function that you are performing. To display or hide the status bar : Click View > User Interface > Status Bar. Information provided in the status bar : è A brief description as you move the pointer over a tool or click a menu item. è A rebuild icon , if you change a sketch or part that requires the rebuild of the part. è Sketch status and pointer coordinates, when you are working in a sketch. è Common measurements for selected entities, such as the length of an edge. è A message to indicate that you are editing a part while in an assembly. è An icon for accessing the Reload dialog box when you use collaboration options. è Unit System , which shows the unit system for the active document in the status bar and lets you change or customize the unit system. è An icon to display or hide the Tags box, used to add keywords to features and parts to aid in searching. 1.5 SOLIDWORKS Options To open the SOLIDWORKS Options dialog box: è Click Options (Standard toolbar) or Tools > Options. 11 The following tabs are available: System The system options are stored in the registry and are not part of the documents. Options Therefore, these changes affect all documents, current and future. Document The document properties apply only to the current document, and the Document Properties Properties tab is available only when a document is open. New documents get their document settings (such as Units, Image Quality, and so on) from the document properties of the template used to create the document. Use the Document Properties tab when you set up document templates. The options listed on each tab are displayed in tree format on the left side of the dialog box. As you click an item in the tree, the options for the item appear on the right side of the dialog box. The title bar displays the title of the tab and the title of the options page. 1.5.1 System options The system options include the following : è System Options - General è File Locations Options è MBD (Model Based Definitions )Options è FeatureManager Options è Drawings Options è Spin Box Increments Options è System Colors Options è View Options è Sketch Options è Backup/Recover Options è Display Options è Touch Options è Selection Options è Hole Wizard/Toolbox Options è Performance Options è File Explorer Options è Settings with OpenGL è Search Options è Assemblies Options è Collaboration Options è External References Options è Messages/Errors/Warnings è Default Templates Options è Synchronize Settings 1.5.2 Document Properties The document properties that are available on the left side of the Document Properties tab depend on the type of document that is open. Some document properties are relevant to all document types (parts, assemblies, and drawings). It includes the properties for the following: Option Description Drafting Standard Set the overall detailing drafting standard, and rename, copy, delete, export, or load saved custom drafting standards Annotations pages Fonts, attachments, leading and trailing zeros, and so on 12  Option Description Dimensions pages Text alignment, fonts, leaders, arrow styles and so on Centerlines / Fonts, slot options, and so on Center Marks DimXpert Dimensioning schemes and options for chamfers, slots, and fillets for use with the DimXpert tool Tables pages Various controls for tables View Labels pages Label content and format for detail, section, and auxiliary view labels Virtual Sharps Virtual sharp display styles Detailing Display filter, text scale, and so on Grid/Snap Grid display, spacing, and so on Units Specify how units are displayed Line Font Style and weight of lines for various kinds of edges in drawing documents Line Style Create, save, load, or delete line styles Line Thickness Set line weights that work best with your printer or plotter Image Quality HLR/HLV resolution Document Properties - Units Unit system : Sets the document-level units and precision to a standard system or lets you modify units. Standard systems are : è M K S (meter, kilogram, second) è CGS (centimeter, gram, second) è MMGS (millimeter, gram, second) è IPS (inch, pound, second) Click Custom to modify units in the table. è You can change the unit system without opening Document Properties - Units. In the status bar, click Unit System, then click a unit system. Basic Units: Displays document-level dimension units. Units Decimals Determined by your Unit Based on selection, displays from two to eight decimal places. system selection. None displays no decimal places. 13 1.6 Selection of entities You can use the Select tool (Quick Access toolbar) to Exit a command and return to select mode, which is useful when in sketches and with the viewing tools. The Select flyout menu consists of the following: Option Description Select Selects entities that you click in the graphics area or the FeatureManager design tree. Magnified Displays the magnifying glass so that you can inspect a model and make Selection selections without changing the overall view. Box Selection Selects all entities around which you drag a selection box using the pointer. When you select from left to right, all items within the box are selected. When you select from right to left, items that are crossed by the box boundaries are also selected. Lasso Selection Selects all entities around which you draw a free hand loop. You can lasso select items without closing the lasso loop. For clockwise lasso selection, the lasso selects only items contained in the lasso loop. For counter clockwise lasso selection, the lasso selects sketch entities in the lasso loop and items that cross the lasso. Select over Lets you select by dragging a box or lasso over a model without starting the Geometry drag from an empty space in the graphics area. Select All Selects all shown components and highlights them in the FeatureManager design tree. 14  Unit – II SKETCHING 2.1 Introduction When you open a new part document, first you create a sketch. The sketch is the basis for a 3D model. You can create a sketch on any of the default planes (Front Plane, Top Plane, and Right Plane), a created plane or face of a part. General procedure : 1) Click Sketch on the Sketch toolbar, or click Insert > Sketch. 2) Click a sketch entity tool (line, rectangle, and so on) on the Sketch toolbar. 3) Select one of the three planes (Front, Top, and Right) displayed or face of a part. Default Sketch Planes 4) Create a sketch with the sketch entity tool. 5) Dimension the sketch entities. 6) Click Exit Sketch on the Sketch toolbar. Also Click Exit Sketch or Cancel in the Confirmation Corner. 2.2 Sketch Modes è There are two modes for sketching in 2D: click-drag or click-click. è If you click the first point and drag, you are in click-drag mode. è If you click the first point and release the pointer, you are in click-click mode. è Double-click or press Esc to terminate the chain of entities. 15 2.3 Sketch Toolbar The Sketch toolbar controls all aspects of sketch creation. It includes the following tools : Tool Description Tool Description Tool Description Select 3 Point Arc Extend Entities Grid/Snap Ellipse Split Entities Sketch or Exit Sketch Partial Ellipse Mirror Entities 3D Sketch Parabola Dynamic Mirror Entities 3D Sketch On Plane Conic Move Entities Slicing Spline Rotate Entities Rapid Sketch Style Spline Scale Entities Instant2D Spline on Surface Copy Entities Shaded Sketch Contours Equation Driven Curve Replace Entity Line Point Stretch Entities Corner Rectangle Centerline Linear Sketch Pattern Center Rectangle Midpoint Line Circular Sketch Pattern 3 Point Corner Rectangle Construction Geometry Make Path 3 Point Center Rectangle Text Modify Sketch Parallelogram Plane No Solve Move Straight Slot Sketch Fillet Sketch Picture Center point Straight Slot Sketch Chamfer Sketch Numeric Input 3 Point Arc Slot Offset Entities Sketch Dimension Driven Center point Arc Slot Offset On Surface Add Dimension Polygon Convert Entities Insert Pen Sketch Circle Intersection Curve Detach Segment On Drag Perimeter Circle Face Curves Reverse Endpoint Tangent Center point Arc Segment Dissolve Entities Tangent Arc Trim Entities 16 2.4 Sketch entities 2.4.1 Sketching lines 1) Click Line on the Sketch toolbar, or click Tools > Sketch Entities > Line. The pointer changes to. 2) Click in the graphics area and sketch the line. 3) Complete the line in one of the following ways: è Drag the pointer to the end of the line and release. è Release the pointer, move the pointer to the end of the line, and click again. 4) Sketch the line with approximate length and angle. 5) After sketching the line, the orientation , length and angle can be modified by one of the following methods : è Click on the line. The Line Properties PropertyManager is displayed. Under Parameters, Set a value for Length. Set a value for Angle. è The line parameters can be modified using Smart Dimension on the Sketch tool bar. 6) Click or double-click to accept the line with modified parameters. Options : Option Description For construction To sketch a construction line Infinite length To sketch a line of infinite length Midpoint line To sketch a line that is symmetrical from the midpoint of the line Centre line To sketch centerlines to create symmetrical sketch elements and revolved features 2.4.2 Sketching rectangles You can sketch the following rectangle types : Rectangle type Tool Rectangle properties Corner Rectangle Sketches standard rectangles. Center Rectangle Sketches rectangles at a center point. 3 Point Corner Rectangle Sketches rectangles at a selected angle. 3 Point Center Rectangle Sketches rectangles with a center point at a selected angle. Parallelogram Sketches a standard parallelogram. 17 To sketch corner rectangles : 1) Click Rectangle. 2) Click to place the first corner of the rectangle, drag, and release when the rectangle is approximately correct size and shape. Rectangle with Modified rectangle approximate size after smart dimension 3) Modify the dimensions of the rectangle using Smart Dimension on the Sketch tool bar. 4) Click. 2.4.3 Sketching circle You can sketch the following circle types: Circle type Tool Circle properties Circle Sketches center-based circles. Perimeter Circle Sketches perimeter-based circles. To sketch circles : 1) Click Circle. 2) Click to place the center of the circle. 3) Drag and click to set the approximate radius. 4) Modify the dimensions using PropertyManager or Smart Dimension 5) Click. 2.4.4 Sketching arcs You can sketch the following arc types : Arc types Tool Arc properties Center point Arc Sketches arcs from a center point, a start point, and an end point. Tangent Arc Sketches arcs that are tangent to sketch entities. 3 Point Arc Sketches arcs by specifying three points (start, end, and midpoint). 18 To sketch center point arcs: 1) Click Center point Arc. 2) Click to place the center of the arc. 3) Release and drag to set the radius and the angle. 4) Click to place a start point. 5) Release, drag, and click to set an end point. 6) Modify the dimensions using PropertyManager or Smart Dimension 7) Click. To sketch tangent arcs: 1) Click Tangent Arc. 2) Click on the end point of a line, arc, ellipse, or spline. 3) Drag the arc to the desired shape and release. 4) Click. To sketch 3 point arcs: 1) Click 3 Point Arc. 2) Click to set a start point. 3) Drag the pointer , then click to set an end point. 4) Drag to set the radius. 5) Click to set the arc. 6) Click. 2.4.5 Sketching ellipse è Use the Ellipse tool to create a complete ellipse. è Use the Partial Ellipse tool to create an elliptical arc. To create an ellipse: 1) Click Ellipse on the Sketch toolbar. 2) Click in the graphics area to place the center of the ellipse. 3) Drag and click to set the major axis of the ellipse. 4) Drag and click again to set the minor axis of the ellipse. 5) Modify the dimensions using PropertyManager. 19 2.4.6 Sketching polygons Equilateral polygons with any number of sides between 3 and 40 can be created. To create a polygon: 1) Click Polygon on the Sketch toolbar. 2) Set the properties in the Polygon PropertyManager as necessary. 3) Click in the graphics area to place the center of the polygon, and drag out the polygon. 4) Modify the dimensions using PropertyManager. 5) Click. 2.4.7 Sketching text To sketch text on a part: 1) Click Text on the Sketch toolbar. 2) To create a profile for placing the text, sketch a circle or a continuous profile from lines, arcs, or splines in a sketch, close the sketch, then open another sketch for the text. 3) In the graphics area, select an edge, curve, sketch, or sketch segment. The selected item appears under Curves. 4) In the PropertyManager, under Text, type the text to display. 5) The text appears in the graphics area as you type. 6) Set the properties in the Sketch Text PropertyManager as necessary. 7) Click. 2.5 Dimensions You can specify dimensions between entities such as lengths, angles and radii. When you change dimensions, the size and shape of the part changes. To fully define the sketch, you add relations and apply dimensions using the Smart Dimension tool (Dimensions/Relations toolbar). The software uses the following two types of dimensions : è Driving Dimensions : Driving dimensions change the size of the model when you change their values. Ordinate and baseline dimensions in sketches are driving dimensions. è Driven Dimensions : Some dimensions associated with the model are driven. You can create driven, or reference dimensions, for informational purposes. The value of driven dimensions changes when you modify driving dimensions or relations in the model. You cannot modify the values of driven dimensions directly unless you convert them to driving dimensions. 20 2.5.1 Dimensions/Relations Toolbar and Menus The Dimensions/Relations toolbar provide tools to dimension and to add and delete geometric relations. It includes the following : Tool Description Tool Description Smart Dimension Path Length Dimension Auto Insert Dimension Chamfer Dimension Horizontal Dimension Fully Define Sketch Vertical Dimension Add Relation Baseline Dimension Automatic Relations Ordinate Dimension Display/Delete Relations Horizontal Ordinate Dimension Scan Equal Vertical Ordinate Dimension Isolate Changed Dimensions Angular Running Dimension 2.5.2 Dimensioning a Sketch You dimension 2D or 3D sketch entities with the Smart Dimension tool. You can drag or delete a dimension while the Smart Dimension tool is active. Dimension types are determined by the sketch entities you select. For some types of dimensions (point-to-point, angular, circular), the location where you place the dimension also affects the type of dimension that is added. To add a dimension to a sketch or drawing : 1) Click Smart Dimension on the Dimensions/Relations toolbar, or click Tools > Dimensions > Smart. 2) The default dimension type is Parallel. Optionally, you can choose a different dimension type from the shortcut menu. Right- click the sketch, and select More Dimensions. Choose from Horizontal, Vertical, Ordinate, Horizontal Ordinate, or Vertical Ordinate. 3) Select the items to dimension. As you move the pointer, the dimension snaps to the closest orientation. 4) Click to place the dimension. 5) You can change Smart Dimension values by clicking over the value and using the Modify box. 21 2.5.3 Sketch Geometry Status Sketches include a status, and sketch entities within the sketch include a state. Sketch entity states are displayed in different colors to facilitate identification. Sketch states include the following : è Dangling : Appears as brown in the graphics area. Indicates sketch geometry that cannot be resolved. For example, deleting an entity that was used to define another sketch entity. è Driven : Appears as gray in the graphics area. Indicates a dimension that is unnecessary and cannot be modified. è Item Conflicts : Appears as yellow in the graphics. Indicates a redundant dimension or an unnecessary relation. è Under Defined : Appears as blue in the graphics area. Indicates a sketch entity which requires a dimension or relation to another sketch entity. è Fully Defined : Appears as black in the graphics area. Indicates all required dimensions and relations to sketch entities are present. è Over Defined : Appears as yellow in the graphics area. Indicates sketch entities that are invalid, creating a sketch without resolution in its current state. Requires deleting some relations or dimensions, or returning the sketch entity to its prior state. è Item is Unsolvable : Appears in red in the graphics area. Indicates the geometry cannot determine the position of one or more sketch entities. Sketch solved with 50 dimension Sketch is unsolvable with 80 dimension 2.5.4 Fully Defined Sketches The Fully Define Sketch tool calculates which dimensions and relations are required to fully define under defined sketches or selected sketch entities. You can access Fully Define Sketch at any point and with any combination of dimensions and relations already added. To fully define a sketch : 1) Create a sketch. 2) Click Fully Define Sketch (Dimensions/Relations toolbar) or Tools > Dimensions > Fully Define Sketch. 22  3) Set the options for relations and dimensions in PropertyManager. Click Calculate. 4) Modify each dimension by clicking on it. 5) Click. Before modification After modification Fully defined sketch 2.6 Relations Relations establish geometric relationships between sketch entities. Automatic Relations is a setting that is turned on by default. When you are sketching, it displays relations that are suggested by the sketch as small yellow icons attached to the cursor and adds those relations to the current sketch entity. Depending on the sketch entities and the position of your pointer, more than one sketch relation can display simultaneously. Inferencing refers to the blue dotted lines that display in Sketch mode when the cursor aligns with endpoints, center points, or the origin. Inferencing creates sketch relations only when the symbol shown on the sketch cursor has a yellow background. 2.6.1 Adding relations You can add relations in the following ways : 1) As you sketch, allow the SOLIDWORKS application to automatically add relations. Automatic relations rely on: è Inferencing è Pointer display è Sketch Snaps and Quick Snaps 2) After you sketch, manually add relations using the Add Relation tool, or edit existing relations using the Display/Delete Relations tool. If you right-click with one or more sketch entities selected, the toolbar that displays stays visible to allow you to add multiple relations. For example, you have two lines selected. You can add vertical and parallel relations to the lines and make them equal without making changes in the PropertyManager or displaying the toolbar. 23 2.6.2 Description of Sketch Relations The following table describes the entities that you can select for a relation and the characteristics of the resulting relation. Relation Entities to select Resulting relations Horizontal One or more lines The lines become horizontal. Vertical One or more lines The lines become vertical. Collinear Two or more lines. The items lie on the same infinite line. Coradial Two or more arcs. The items share the same center point and radius. Perpendicular Two lines. The two items are perpendicular to each other. Parallel Two or more lines. The items are parallel to each other. AlongZ A line and a plane. The line is normal to the face of the selected plane. Tangent An arc, ellipse, or spline, The two items remain tangent. and a line or arc. Concentric Two or more arcs, or a The arcs share the same center point. point and an arc. Midpoint Two lines or a point The point remains at the midpoint of the line. and a line. Intersection Two lines and one The point remains at the intersection of the lines. point. Coincident A point and a line, arc, The point lies on the line, arc, or ellipse. or ellipse. Equal Two or more lines or The line lengths or radii remain equal. two or more arcs. Equal Two splines. The radius of curvature and the vector (direction) Curvature matches between the two splines. Symmetric A centerline and two The items remain equidistant from the centerline, on a points, lines, arcs, or line perpendicular to the centerline. ellipses. Fix Any entity. The entity’s size and location are fixed. Pierce A sketch point and an The sketch point is coincident to where the axis, edge, axis, edge, line, or or curve pierces the sketch plane. The pierce relation is spline. used in sweeps with guide curves. On Edge Edges of a solid. The edges of the solid are projected to the sketch plane using the Convert Entities tool. On Surface Sketch entities on a The sketch entities reside on the surface. surface. 24 2.7 Sketch Tools 2.7.1 Sketch Fillets The Sketch Fillet tool trims away the corner at the intersection of two sketch entities to create a tangent arc. This tool is available for both 2D and 3D sketches. The Fillet tool on the Features toolbar fillets entities such as edges in parts. To create a fillet in a sketch : 1) In an open sketch, click Sketch Fillet on the Sketch toolbar, or Tools > Sketch Tools > Fillet. 2) Set the properties in the Sketch Fillet PropertyManager. 3) Select the sketch entities to fillet. You can select two sketch entities or select a corner. 4) Drag the preview to adjust the fillet size if necessary. 5) Click to accept the fillet. 2.7.2 Sketch Chamfers The Sketch Chamfer tool applies a chamfer to adjacent sketch entities in 2D and 3D sketches. This tool is available for both 2D and 3D sketches. The Chamfer tool on the Features toolbar chamfers entities such as edges in parts. To create a sketch chamfer : 1) In an open sketch, click Sketch Chamfer on the Sketch toolbar, or click Tools > Sketch Tools > Chamfer. 2) In the PropertyManager, set the Chamfer Parameters as necessary. 3) In the graphics area, select the two sketch entities to chamfer. To select the sketch entities, you can: è Hold Ctrl and select two sketch entities. è Select a vertex. 4) The chamfer is applied immediately. Angle- Distance- Equal distance distance distance 5) Click to accept the chamfer. Chamfer Parameters Angle-distance Distance 1 : Applied to the first sketch entity selected. Direction 1 Angle : Applied from the first sketch entity towards the second. Distance - distance Equal distance selected : è Distance 1 is applied to both sketch entities. Equal distance cleared : è Distance 1 is applied to the first sketch entity selected. è Distance 2 is applied to the second sketch entity selected. 25 2.7.3 Offset Entities Offset one or more sketch entities, selected model edges, or model faces by a specified distance. For example, you can offset sketch entities such as splines or arcs, sets of model edges, loops, and so on. If the original entity changes, then the offset entity also changes when you rebuild the model. To create a sketch offset : 1) In an open sketch, select one or more sketch entities, a model face, or a model edge. 2) Click Offset Entities (Sketch toolbar) or Tools > Sketch Tools > Offset Entities. 3) Set the properties in the Offset Entities PropertyManager. When you click in the graphics area, the offset entity is complete. Set the properties before you click in the graphics area. Before offset After offset 4) Click or click in the graphics area. 2.7.4 Trim Entities Select the trim type based on the entities you want to trim or extend. You can use any of the following trim options : Option Description Power Trim You can use Power trim to trim multiple, adjacent sketch entities by dragging the pointer across each sketch entity. Corner Extends or trims two sketch entities until they intersect at a virtual corner. Trim Away Inside Trims open sketch entities that lie inside two bounding entities. Trim Away Outside Trims open sketch entities outside of two bounding entities. Trim to Closest Trim or extend the selected sketch entities. You can also use : è Keep trimmed entities as construction geometry è Ignore trimming of construction geometry Trimming with Power Trim You can use Power trim to trim multiple, adjacent sketch entities by dragging the pointer across each sketch entity. To trim with the Power trim option : 1) Click Trim Entities (Sketch toolbar) or Tools > Sketch Tools > Trim. 2) In the PropertyManager, under Options, select Power trim. 3) Click in the graphics area next to the first entity, and drag across the sketch entity to trim. 26  4) The pointer changes to as it crosses and trims the sketch entity. A trail is created along the trim path. 5) Continue to hold down the pointer and drag across each sketch entity you want to trim. 6) Release the pointer when finished Before Trim After Trim trimming the sketch, then click. 2.7.5 Extend Entities You can add to the length of a sketch entity (line, centerline, or arc). Use Extend Entities to extend a sketch entity to meet another sketch entity. To extend a sketch entity : 1) In an open sketch, click Extend Entities on the Sketch toolbar, or click Tools > Sketch Tools > Extend. The pointer changes to. 2) Move the pointer over the sketch entity to extend. 3) A preview appears in the direction to extend the entity. Before Extend After Extend & Trim 4) If the preview extends in the wrong direction, move the pointer to the other half of the line or arc. 5) Click the sketch entity to accept the preview. 2.7.6 Split Entities You can split a sketch entity to create two sketch entities. Conversely, you can delete a split point to combine two sketch entities into a single sketch entity. Use two split points to split a circle, full ellipse, or a closed spline. To split a sketch entity : 1) In an open sketch, click Split Entities (Sketch toolbar) or Tools > Sketch Tools > Split Entities. 2) The pointer changes to. 3) Click the sketch entity at the location where you want the split to occur. 4) The sketch entity splits into two entities, and a split point is added between the two sketch entities. 2.7.7 Mirror Entities Select Mirror Entities to mirror pre-existing 2D sketch entities on a plane, and then select the entity about which to mirror. If you want to first select the entity about which to mirror, and then sketch the entities to mirror, select Dynamic Mirror Entities. 27 You can mirror sketches about any these entities : è Centerlines è Lines è Linear model edges è Linear edges on drawings Before Mirror After Mirror To mirror existing sketch entities : 1) In an open sketch, click Mirror Entities (Sketch toolbar) or Tools > Sketch Tools > Mirror. 2) In the PropertyManager: è Select sketch entities for Entities to Mirror. è Clear Copy to add a mirror copy of the entities and remove the original sketch entities. è Select Copy to include both the mirrored copy and the original sketch entities. 3) Select an edge or a line to Mirror about. 4) Click. 2.7.8 Convert Entities You can create one or more curves in a sketch by projecting an edge, loop, face, curve, or external sketch contour, set of edges, or set of sketch curves onto the sketch plane. Sketch plane above part Loop of edges projected onto plane using Convert Entities To convert an entity : 1) Click Convert Entities (Sketch toolbar) or Tools > Sketch Tools > Convert Entities. 2) Click a model edge, loop, face, curve, external sketch contour, set of edges, or set of curves. 3) In the PropertyManager, click Select chain to convert all contiguous sketch entities. 4) Click. 28 2.7.9 Moving or Copying Sketch Entities To move or copy entities : 1) In sketch mode, do one of the following : è Click Move Entities (Sketch toolbar) or Tools > Sketch Tools > Move. è Click Copy Entities (Sketch toolbar) or Tools > Sketch Tools > Copy. 2) In the PropertyManager, under Entities to Move or Entities to Copy : Select sketch entities. 3) Under Parameters, do one of the following : è Select From/To, click Start point to set a Base point , and then drag to position the sketch entities. è Select X/Y and set values for Delta X and Delta Y to position the sketch entities. 4) Click. 2.7.10 Rotating Sketch Entities To rotate sketch entities : 1) In sketch mode, click Rotate Entities (Sketch toolbar) or Tools > Sketch Tools > Rotate. 2) In the PropertyManager, under Entities to Rotate : Select sketch entities. 3) Under Parameters, è Click Base Point (Rotate Point Defined) to set a Base point , and then click in the graphics area to set the Center of rotation. è Set a value for Angle. 4) Click. 2.7.11 Scaling Sketch Entities To scale sketch entities: 1) In Edit Sketch mode click Scale Entities (Sketch toolbar) or Tools > Sketch Tools > Scale. 2) In the PropertyManager, under Entities to Scale, select sketch entities. 3) Under Parameters: è Click Base Point (Scale Point Defined) to set a Base point , and then click in the graphics area to set the point to Scale about. è Set a value for Scale Factor. For example, specify 2 for double size, 0.5 for half size, and so on. 4) Click. 2.7.12 Stretching Sketch Entities To stretch sketch entities: 1) In Edit Sketch mode, click Stretch Entities (Sketch toolbar) or Tools > Sketch Tools > Stretch Entities. 2) In the PropertyManager, under Entities to Stretch, select sketch entities. 3) Under Parameters, do one of the following : 29  è Select From/To, click Base point to set a base point , and then drag to stretch the sketch entities. è Select X/Y and set values for Delta X and Delta Y to stretch the sketch entities. 4) Click. 2.7.13 Sketch Patterns Create linear or circular sketch patterns using elements from sketch entities. To create a linear sketch pattern : 1) In an open sketch, click Linear Sketch Pattern (Sketch toolbar) or Tools > Sketch Tools > Linear Pattern. 2) In the PropertyManager, under Entities to Pattern, select the sketch entities to pattern. 3) Set values for Direction 1 (X-axis). è Click Reverse direction. è Set Spacing between sketch entities. è Select Dimension X spacing to display a dimension between entities. è Set Number of sketch entities. è Select Display instance count to show the number of instances in the pattern. è Set Angle at which to pattern the sketch entities. 4) Repeat for Direction 2 (Y-axis). 5) Click. To create circular sketch patterns : 1) In an open sketch, click Circular Sketch Pattern (Sketch toolbar) or Tools > Sketch Tools > Circular Pattern. 2) In the PropertyManager, under Entities to Pattern, select the sketch entities to pattern. 3) Under Parameters: è Click Reverse direction. è In the graphics area, drag the selection point to select a pattern center other than the sketch origin. è Alternatively, in Center X and Center Y , specify values. è Define Spacing to specify the total number of degrees in the pattern. è Select Equal spacing to pattern instances equidistant from each other. è Select Dimension radius to display the circular pattern radius. è Select Dimension angular spacing to display the dimension between pattern instances. è Specify the Number of Instances. è Select Display instance count to show the number of instances in the pattern. 30  è Specify the Radius of the pattern. è Specify the Arc Angle that is measured from the center of the selected entities to the center point or vertex of the pattern. 4) Click. 2.8 Blocks You create blocks from single or multiple sketch entities. The Blocks Toolbar includes the following : Tool Description Make Block Convert sketch entities to blocks. Edit Block Add or remove sketch entities. Change dimensions and relations. Insert Block Create multiple instances of existing blocks or browse for blocks to retrieve blocks in parts, assemblies, or blocks. Add/Remove Adds or removes sketch entities from a block. Rebuild Rebuilds and updates parent sketches by the block. Save Block Saves and adds an.sldblk extension. Explode Block Dissolves the block. Exploding one instance of a block only affects that instance of the block. Belt/Chain Creates continuous tangent lines and arcs to represent the belt or chain path. To make blocks : 1) Create a sketch. 2) Click Make Block (Blocks toolbar) or Tools > Block > Make. 3) Select the sketch entities you want to make as a block for Block Entities. 4) Click. 5) Save the part. 2.9 Splines The SOLIDWORKS software supports the following two types of splines : 1) B-splines : You can use B-splines to create complex curves. You can define and modify them using several controls, including spline points, spline handles, and control polygons. A single B-spline can have multiple through points and spans. 2) Style splines :. They are a good option when it is important to have a smooth curve. You define and control the curves using control vertices. There are no through points, so a style spline has only one span between the endpoints. 31 To create multiple point splines : 1) Click Spline (Sketch toolbar) or Tools > Sketch Entities > Spline. 2) The pointer changes to. 3) Click to place the first point and drag out the first segment. 4) Click the next point and drag out the second segment. 5) Repeat for each segment, then double-click when the spline is complete. 6) Click. To sketch the style spline : 1) Click Style Spline (Sketch toolbar) or Tools > Sketch Entities > Style Spline. 2) In the graphics area, click the first endpoint. 3) The first click creates the first control vertex point in the style spline. 4) Continue adding more control vertices. 5) Repeat for each vertex, then double-click when the spline is complete. 6) Click. 2.10 Editing an Existing Sketch To edit an existing sketch, do one of the following: 1) Click Sketch on the Sketch toolbar, or click Insert > Sketch. Select an existing sketch to edit. 2) Right-click a sketch in the FeatureManager design tree, or right-click a sketch entity in the graphics area, and select Edit Sketch. 32  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 Y