SOLIDWORKS MODULE PDF

SOLIDWORKS MODULE MOHD AZWIR AZLAN MOHD FAHRUL HASSAN FAKULTI KEJURUTERAAN MEKANIKAL DAN PEMBUATAN UNIVERSITI TUN HUSSEIN ONN MALAYSIA MODULE: SOLIDWORKS FACILITATOR / LECTURER: 1) Name: Mr. Mohd Azwir bin Azlan e-mail: [email protected] Tel: 07-4537727 Room: C16-101-02 2) Name: Mr. Mohd Fahrul bin Hassan e-mail: [email protected] Tel: 07-4538475 Room: CAE 1 Lab A. AIMS The goal of this course is to provide student in skill and design technique to produce 3D modeling by using SolidWorks / Catia software. B. LEARNING OUTCOMES At the end of this course, student will be able to use and appreciate the knowledge and skill had learned to: 1. Draw and produce 3D modeling drawing by using SolidWorks software. 2. Produce detail drawing according to the legal standards of the Engineering drawing practice. 3. Demonstrate the ability to produce a drawing project with proper scale and dimensioning. 4. Communicate and work in a group efficiently and effectively through given assignments and project. C. LEARNING CONTENTS This module consists: Unit 1: Introduction to SolidWorks Software. Unit 2: Sketching Unit 3: Basic Modeling Technique Unit 4: Assembly Parts Unit 5: Detail Drawing A-1 E. REFERENCES 1. SolidWorks Essentials - SolidWorks 2007 Training Manual, Massachusetts, USA. 2. Advanced Part Modeling - SolidWorks 2007 Training Manual, Massachusetts, USA. 3. Advanced Assembly Modeling - SolidWorks 2007 Training Manual, Massachusetts, USA. 4. SolidWorks Drawing - SolidWorks 2007 Training Manual, Massachusetts, USA. A-2 TABLE OF CONTENT UNIT TITLE PAGE UNIT 1 INTRODUCTION TO SOLIDWORKS SOFTWARWE 1.1 Introduction 1-1 1.2 Learning Outcomes 1-1 1.3 Learning Contents 1-1 1.3.1 Wire frame, Surface & Solid Modeling History 1-1 1.3.2 What is SolidWorks 1-2 1.3.3 Terminology and SolidWorks Software 1-2 Characteristics 1.3.3.1 Featured-based 1-2 1.3.3.2 Parametric Solid Modeling 1-5 1.3.3.3 Fully Associative 1-5 1.3.4 Design Intent 1-6 1.3.4.1 Some Examples of Different Design 1-6 Intent in a Sketch 1.3.4.2 How Feature Affect Design Intent 1-7 1.3.5 Open & Exit Program 1-8 1.3.6 Open & Save File 1-9 1.3.7 Parts, Assemblies & Drawings 1-9 1.3.8 Software Interface 1-11 1.3.8.1 Left Side of SolidWorks Window 1-12 1.3.8.2 Right Side of SolidWorks Wndow – 1-13 The Task Pane 1.3.8.3 Toolbar 1-14 1.3.8.4 System Feedback 1-14 1.3.9 Mouse Button 1-14 1.3.10 Customize Option 1-15 1.4 References 1-15 UNIT 2 SKETCHING 2.1 Introduction 2-1 2.2 Learning Outcomes 2-1 2.3 Learning Contents 2-1 2.3.1 Why Needs Sketches? 2-1 2.3.2 Planes 2-3 2.3.3 Sketch Entities and Geometry 2-4 2.3.4 Sketch Complexity 2-5 2.3.5 Mechanics of Sketching 2-6 2.3.6 Beginning a Sketch (Draw Rectangle) 2-6 2.3.7 Rules That Govern Sketches 2-7 2.3.8 The Status of a Sketch 2-8 2.3.9 Making a Fully Define Sketch 2-9 2.3.9.1 Sketch Relation 2-9 2.3.9.2 Add Relation 2-12 2.3.9.3 Dimension 2-12 2.3.9.4 Dimensioning a Sketch 2-12 2.3.10 Others Important 2D Sketch Command 2-14 A-3 2.3.10.1 Fillet 2-14 2.3.10.2 Offset 2-14 2.3.10.3 Convert Entities 2-16 2.3.10.4 Trim Entities 2-16 2.3.10.5 Mirror Entities 2-19 2.4 Activities / Exercise 2-20 2.4.1 Exercise I 2-20 2.4.2 Exercise II 2-21 2.4.3 Exercise III 2-21 2.5 References 2-22 UNIT 3 BASIC MODELING TECHNIQUE 3.1 Introduction 3-1 3.2 Learning Outcomes 3-1 3.3 Learning Contents 3-2 3.3.1 3D Modeling Terminology 3-2 3.3.2 Choosing the Best Profile 3-3 3.3.3 Choosing the Sketch Plane 3-4 3.3.4 Features and Commands 3-4 3.3.5 Views 3-6 3.3.6 Revolve Feature 3-9 3.3.7 Sweep Feature 3-10 3.3.8 Loft Feature 3-10 3.3.9 Fillet Feature 3-12 3.3.10 Chamfer Feature 3-12 3.3.11 Rib Feature 3-13 3.3.12 Draft Feature 3-14 3.3.13 Hole Wizard 3-15 3.3.14 Pattern 3-15 3.3.15 Reference Geometry 3-18 Creating Plane 3-18 Creating Axis 3-20 Creating Coordinate System 3-21 Creating Point 3-22 3.3.16 Families of Parts 3-22 3.4 Activities / Exercise 3-24 3.4.1 Exercise 1 3-24 3.4.2 Exercise 2 3-24 3.4.3 Exercise 3 3-25 3.4.4 Exercise 4 3-26 3.4.5 Exercise 5 3-27 3.4.6 Exercise 6 3-28 3.4.7 Exercise 7 3-29 3.5 References 3-31 UNIT 4 ASSEMBLY PARTS 4.1 Introduction 4-1 4.2 Learning Outcomes 4-1 4.3 Learning Contents 4-1 4.3.1 Assemblies 4-1 A-4 4.3.1.1 Overview 4-1 4.3.1.2 FeatureManager Design Tree 4-2 Conventions 4.3.1.3 Display of Components 4-3 4.3.1.4 Adding Components to an Assembly 4-4 4.3.1.5 Design Method 4-4 4.3.2 Moving and Rotating Components 4-6 4.3.2.1 Moving a Component 4-6 4.3.2.2 Rotating a Component 4-8 4.3.2.3 Triad 4-9 4.3.3 Mates 4-11 4.3.3.1 Suppressing a Mating Relationship 4-12 4.3.3.2 Best Practices for Mates 4-12 4.3.3.3 Types of Mates 4-14 4.3.3.4 View Mates / View Mates Error 4-16 4.3.3.5 Solving Mate Problem 4-19 4.3.4 Interferences Detection 4-20 4.3.5 Exploding an Assembly View 4-22 4.3.5.1 Creating and Editing Exploded Views 4-23 4.3.6 Physical Simulation 4-25 4.3.6.1 Gravity 4-26 4.3.6.2 Linear or Rotary Motor 4-27 4.3.6.3 Linear Springs 4-29 4.3.6.4 Recording and Replaying a Simulation 4-30 4.4 Activities / Exercise 4-31 4.4.1 Activity 4-31 4.4.2 Exercise 1 4-62 4.4.3 Exercise 2 4-64 4.5 References 4-66 UNIT 5 DETAIL DRAWING 5.1 Introduction 5-1 5.2 Learning Outcomes 5-1 5.3 Learning Contents 5-1 5.3.1 Overview 5-1 5.3.2 Sheet Formats and Templates 5-1 5.3.2.1 Properties in The Template 5-2 5.3.2.2 Customizing a Sheet Format 5-3 5.3.2.3 Creating a Drawing 5-4 5.3.2.4 Size of the Sheet 5-5 5.3.2.5 The Drawing Window 5-6 5.3.2.6 Sheet Properties 5-6 5.3.2.7 Sheet Format / Size 5-7 5.3.2.8 Scales in Drawing 5-7 5.3.3 Dimensions 5-8 5.3.3.1 Inserting Dimensions into Drawings 5-11 5.3.3.2 Setting Dimensions Option 5-12 5.3.3.3 AutoDimension a Drawing 5-13 5.3.3.4 Parallel Dimensions 5-13 5.3.3.5 Reference Dimensions 5-14 A-5 5.3.3.6 Baseline Dimensions 5-15 5.3.3.7 Chamfer Dimensions 5-15 5.3.3.8 Modify Dimensions 5-16 5.3.4 Drawing Views 5-17 5.3.4.1 Standard 3 View 5-17 5.3.4.2 Model View 5-19 5.3.4.3 Relative to Model View 5-20 5.3.5 Bill of Materials 5-20 5.3.5.1 Bill of Materials – Rows 5-21 5.3.5.2 Bill of Material – Column 5-22 5.3.5.3 Bill of Material - Contents 5-23 5.3.6 Center Mark & Center Line 5-24 5.3.6.1 Center Mark PropertyManager 5-24 5.3.7 Annotation and Sectioning 5-25 5.3.7.1 Inserting Annotation into Drawings 5-26 5.3.7.2 Annotation Options Overview 5-27 5.4 Activities / Exercise 5-28 5.5 References 5-28 A-6 Unit 1 – Introduction to SolidWorks Software UNIT 1 INTRODUCTION TO SOLIDWORKS SOFTWARE 1.1 INTRODUCTION This Module discusses the wireframe, surface and solid modeling history, terminology and SolidWorks software characteristics, design intent, open & exit program, Software interface, toolbar, mouse button and customize option. 1.2 LEARNINGS OUTCOMES Upon successful completion of this lesson, you will be able to: Describe the key characteristics of a feature-based, parametric solid modeler. Distinguish between sketched and applied features. Identify the principal components of the SolidWorks user interface. Explain how different dimensioning methodologies convey diferent design intents. 1.3 LEARNING CONTENTS 1.3.1 Wire frame, Surface and Solid Modeling History Initial stage – CAD is used to prepare only 2D drawing (Orthographic & Isometric) Then, it develops to a 3D wireframe drawing. It is created by specifying each edge of the physical object where two mathematically continuous smooth surfaces meet, or by connecting an object's constituent vertices using straight lines or curves. Disadvantage – confusing Figure 1.1: Sample rendering of a wireframe cube, icosahedron, and approximate sphere. 1-1 SolidWorks Module Unit 1 – Introduction to SolidWorks Software For visualization of the underlying design structure of a 3D model, surface modeling is introduced. o Advantages – more realistic view o Disadvantages - powerful computer needed - cannot do engineering analysis because no mass created Then Solid Modeling is develops to create an engineering drawing and also to produce advanced engineering analysis (FEA). o Disadvantages – any mistake can cause modeling work had to be redo. Recently, new advance modeling is develops based on parametric modeling and features based modeling to make modeling work become easier. 1.3.2 What is SolidWorks? SolidWorks is design automation software. In SolidWorks, you sketch ideas and experiment with different designs to create 3D models. SolidWorks is used by students, designers, engineers, and other professionals to produce simple and complex parts, assemblies, and drawings. 1.3.3 Terminology and SolidWorks Software Characteristics 1.3.3.1 Featured-based Made up of a number of individual piece part Figure 1.2: Concept of featured based modeling 1-2 SolidWorks Module Unit 1 – Introduction to SolidWorks Software 1-3 SolidWorks Module Unit 1 – Introduction to SolidWorks Software Applied Applied 1-4 SolidWorks Module Unit 1 – Introduction to SolidWorks Software Figure 1.3: Different plane on Figure 1.4: Multiple feature sketch featured based. on many plane. Can be classified as either sketched or applied 9 Sketched Feature: Is based upon a 2D sketch. Generally that sketch is transformed into a solid by extrusion, rotation, sweeping or lofting. 9 Applied Feature: Created directly on the solid model. Fillets and chamfers are examples of this type of feature. 1.3.3.2 Parametric solid modeling Enable you to quickly and easily make changes to the model 1.3.3.3 Fully associative Model is fully associative to the drawings and assemblies that reference it. Any model changes will reflect the associated drawings and assembly. Figure 1.5: File references 1-5 SolidWorks Module Unit 1 – Introduction to SolidWorks Software 1.3.4 Design Intent Is your plan as to how the model should behave when it is changed. For example: if you model a boss with a blind hole in it, the hole should move when the boss is moved. Several factors contribute to how you capture design intent: o Automatic relations o Equations o Added relations o Dimensioning 1.3.4.1 Some examples of different design intent in a sketch (a) Dimensioned like this will keep the holes 20 mm from each end regardless of how the overall plate width is changed. (b) Dimensioned like this will keep the holes positioned relative to the left edge of the plate. The positions of the holes are not affected by changes in the overall width of the plate. (c) Dimensioning from the edge and center to center will maintain the distance between the hole centers and allow it to be changed that way. 1-6 SolidWorks Module Unit 1 – Introduction to SolidWorks Software 1.3.4.2 How feature affect Design Intent The choice of features and the modeling methodology are also important. For example, consider the case of a simple stepped shaft as shown below. There are several ways a part like this could be built. o The “Layer Cake” Approach o The Manufacturing Approach o The “Potter’s Wheel” Approach The “Layer Cake” Approach Builds the part one pieces at a time, adding each layer, or feature, onto the previous one. The Manufacturing Approach Modeling mimics the way the part would be manufactured. For example, if this stepped shaft was turned on a lathe, you would start with a piece of bar stock and remove material using a series of cuts. The “Potter’s Wheel” Approach Builds the part as a single, revolved feature. 1-7 SolidWorks Module Unit 1 – Introduction to SolidWorks Software 1.3.5 Open & Exit Program Running Programs The quickest way to start a program is to double-click on a desktop shortcut. Some programs may not have desktop shortcuts. The Programs menu lists the entire application programs resident on the computer. Exit a Program Select or click File, Exit to end a program. If the file has unsaved changes, you have the chance to save them before exiting. 1-8 SolidWorks Module Unit 1 – Introduction to SolidWorks Software 1.3.6 Open & Save File Opening a File The quickest way to open a file is to double-click on it. The File menu displays your most recently used files. Display most recently used files Saving and Copying Files Saving a file preserves the changes that you have made to it. Use File, Save As to copy a file. File, Save As creates an exact duplicate of the file as it existed at the moment that you copied it. 1.3.7 Parts, Assemblies & Drawings The SolidWorks model is made up of: o Parts ο Assemblies ο Drawings Parts are single three-dimensional (3D) objects. Parts are the basic building blocks of 3D modeling. Parts can be included as components in assemblies and represented in drawings. Assemblies are logical collections of components. These components can be parts or other assemblies. An assembly within an assembly is called a subassembly. Drawings are 2D representations of 3D parts or assemblies. Drawings are needed for manufacturing, quality assurance, supply chain management, and other functions. 1-9 SolidWorks Module Unit 1 – Introduction to SolidWorks Software Parts, assemblies, and drawings are associative. This means that changes in one place are reflected in all of the places that they need to be reflected. Changes that you make to an assembly are reflected in the drawings of that assembly. Changes that you make to a part are reflected in the assembly. Typically, you design each part, combine the parts into assemblies, and generate drawings in order to manufacture the parts and assemblies. The following illustration shows the relationship among parts, assemblies, and drawings. Figure 1.6: Relationship among parts, assemblies, and drawings 1 - 10 SolidWorks Module Unit 1 – Introduction to SolidWorks Software 1.3.8 Software Interface The first thing you may notice about the user interface is that it looks like Windows. That is because it is Windows! The interface is how you interact with the computer in the following ways: Use windows to view files. Use the mouse to select buttons, menus, and model elements. Run programs — like SolidWorks mechanical design software. Find, open, and work with files. Create, save, and copy files. Menu provides access to many of the commands hat the SolidWorks software offers. Figure 1.7: SolidWorks Interface 1 - 11 SolidWorks Module Unit 1 – Introduction to SolidWorks Software 1.3.8.1 Left Side of SolidWorks Window Feature Manager Property Configuration design tree™ Manager Manager FeatureManager Design Tree Displays all the features in a part or assembly As features are created they are added to the FeatureManager design tree. Represents the chronological sequence of modeling operations. PropertyManager Menus Most SolidWorks commands are executed through PropertyManager menus. 1 - 12 SolidWorks Module Unit 1 – Introduction to SolidWorks Software Configuration Manager To create, select, and view multiple configurations of parts and assemblies in a document. 1.3.8.2 Right Side of SolidWorks Window - The Task Pane The Task Pane appears when you open the SolidWorks software. It contains the following tabs: SolidWorks Groups of commands for Getting Started, Resources Community, and Online Resources, plus Tip of the Day. Design Library Reusable parts, assemblies, and other elements, including Library Features. File Explorer Duplicate of Windows Explorer on your computer, plus Recent Documents and Open in SolidWorks. The Task Pane can be in the following states: 1 - 13 SolidWorks Module Unit 1 – Introduction to SolidWorks Software 1.3.8.3 Toolbar Buttons for frequently used commands. You can select the toolbars to display. Toolbars are displayed at the top and sides of the window. You can also access the toolbars from the Command Manager. 1.3.8.4 System Feedback Provided by a symbol attached to the cursor arrow indicating what are you selecting or what the system is expecting you to select. The illustration at the right shows some of the symbols. 1.3.9 Mouse Button Middle Dynamically rotates – pans or zooms a part or assembly. Press + move mouse – rotate a part or assembly. Left Right Activates a context sensitive Select object such as shortcut menu. geometry, menu buttons and objects in the Feature Manager design tree. 1 - 14 SolidWorks Module Unit 1 – Introduction to SolidWorks Software 1.3.10 Customize Option o Use to customize the SolidWorks software to reflect such things as your company drafting standards as well as your individual preferences and work environment. o Control settings like: 9 Units: English (inches) or Metric (millimeters) 9 Colours, Material Properties and Image Quality o Located on the Tools menu or click icon o Several levels of customization:- 9 System Option – will affect every document and every times you open your SolidWorks session. 9 Document properties – applied to the individual document. 1.4 REFERENCES 1. SolidWorks Essentials - SolidWorks 2007 Training Manual, Massachusetts, USA. 2. SolidWorks 2007 Online User’s Guide – SP0.0 3. SolidWorks 2005 – Hand-on Quick Start 1 - 15 SolidWorks Module Unit 2 – Sketching UNIT 2 SKETCHING 2.1 INTRODUCTION This Module introduces 2D Sketching, the basic of modeling in SolidWorks. It discusses the Planes, sketch entities and geometry (Line, Box, Circle, Centerpoint Arc, Tangent Arc, Three point Arc, Ellipse, Spline, Point, Fillet and Center lines), Sketch status, Sketch relations, Dimensioning, Fillet, Offset, Trim, Convert and Mirror. 2.2 LEARNINGS OUTCOMES Upon successful completion of this lesson, you will be able to: Insert a new sketch. Add sketch geometry. Establish sketch relation between pieces of geometry. Understand the state of the sketch. Use sketch tools to add fillets. Extrude the sketch into a solid. 2.3 LEARNING CONTENTS 2.3.1 Why needs sketches? Solid models are built from features. Shape features have sketches. Sketched features are built from 2D profiles. Illustration below shows how a given sketch can form the basis of several different types of features. 2-1 SolidWorks Module Unit 2 – Sketching Example 1 Example 2 2-2 SolidWorks Module Unit 2 – Sketching 2.3.2 Planes Since sketches are flat, or planar, it needs a plane on which to sketch. A SolidWorks part contains three default sketch planes. Default planes - Front, Top, and Right Figure 2.1: Three default references planes intersect at the origin Correspond to the standard principle drawing views: o Front = Front or Back view o Top = Top or Bottom view o Right = Right or Left view Figure 2.2: Selecting a plane according to the model 2-3 SolidWorks Module Unit 2 – Sketching 2.3.3 Sketch Entities and Geometry SolidWorks offers a rich variety of sketch tool for creating profile geometry. Table below shows some of the sketch entities that are available on the sketch toolbar. 2-4 SolidWorks Module Unit 2 – Sketching 2.3.4 Sketch Complexity In many cases, you can produce the same result by creating an extruded feature with a complex profile, or an extruded feature with a simpler profile and some additional features. For example, if the edges of an extrusion need to be rounded, you can draw a complex sketch that contains sketch fillets (A), or draw a simple sketch and add the fillets as separate features later (B). A) Complex sketch Extrude B) Simple sketch Add fillet feature Consider your design intent: o Complex sketches rebuild faster. Sketch fillets can be recalculated much faster than fillet features, but complex sketches can be harder to create and edit. o Simple sketches are more flexible and easier to manage. Individual features can be reordered and suppressed, if necessary. 2-5 SolidWorks Module Unit 2 – Sketching 2.3.5 Mechanics of Sketching To sketch geometry, there are two techniques can be used: Click-Click Select line. Position the cursor where you want the line to start. Click (press and release) the left mouse button. Move the cursor to where you want the line to end. A preview of the sketch entity will follow the cursor like a rubber band. Click the left mouse button a second time. Click and Drag Select line. Position the cursor where you want the line to start. Press and hold the left mouse button. Drag the cursor to where you want the sketch entity to end. A preview of the sketch entity will follow the cursor like a rubber band. Release the left mouse button. 2.3.6 Beginning a Sketch (Draw Rectangle) i) Click Sketch on the Sketch toolbar. ii) Select the Front plane as a sketch plane. iii) Click Rectangle on the Sketch Tools toolbar. iv) Move the pointer to the origin and click the left mouse button. vi) Drag the pointer up and to the right Click the left mouse button. Sketch tool Rectangle tool Sketch origin 2-6 SolidWorks Module Unit 2 – Sketching 2.3.7 Rules That Govern Sketches Different types of sketches will yield different results. Several different types are summarized in the table below. It is important to note that some of the techniques shown in the table below are advanced techniques that are not covered here and need more experience user. Sketch Type Description Special Considerations A typical “standard” None required. sketch that is a neatly closed contour. Multiple nested None required. contours create a boss with an internal cut. Open contour creates None required. a thin feature with constant thickness. Corners are not neatly Rebuilt Error. Unable to create closed. feature due to geometry condition. Sketch contains a self Use the Contour Select Tool. If intersecting contour. both contour are selected, this type of sketch will create a Multibody Solid. Although this will work, multibodies are an advanced modeling technique that you should not use until you have more experience. This sketch of the first This type of sketch will create a feature contains Multibody Solid. disjoint contours. Although this will work, multibodies are an advanced modeling technique that you should not use until you have more experience. 2-7 SolidWorks Module Unit 2 – Sketching 2.3.8 The Status of a Sketch Under defined o There is inadequate definition of the sketch. o You can drag endpoints, lines, or curves until the sketch entity changes shape. o Additional dimensions or relations are required. o Under defined sketch entities are blue (by default). Fully defined o The sketch has complete information. o No additional dimensions or relationships are required. o Fully defined sketch entities are black (by default). Over defined o Contains duplicate dimensions or conflicting relations and it should not be used until repaired. o Over defined sketch entities are red (by default). 2-8 SolidWorks Module Unit 2 – Sketching 2.3.9 Making a Fully Define Sketch Design intent in a sketch is captured and controlled by a combination of two things: o Sketch Relation Create geometric relationships such as parallel, collinear, perpendicular, or coincident between sketch elements. o Dimensions Dimension are used to define the size and location of the sketch geometry. Linear, radial, diameter and angular dimensions can be added. To fully define a sketch and capture the desired design intent requires understanding and applying a combination of relations and dimension. 2.3.9.1 Sketch Relation 2-9 SolidWorks Module Unit 2 – Sketching 2 - 10 SolidWorks Module Unit 2 – Sketching Concentric between two or more arcs or circle. Coradial between two or more arcs or circle. Tangen between line with arc/circle or between arc/circle with arc/circle. 2 - 11 SolidWorks Module Unit 2 – Sketching 2.3.9.2 Add Relations Appears when you click Add Relation on the Dimensions/Relations toolbar. Appears when you select multiple sketch entities in the graphics area. Or, right-click the entity or entities, and select Add Relation from the short-cut menu. Or, click Tools, Relations, Add… 2.3.9.3 Dimension It is used to define the size. In SolidWorks, dimensions are not just static numbers that tell you the size of something. Instead, the dimensions are used to change the size and shape of the model. The type of dimension is determined by the items on which you click. For example, if you pick an arc the system creates a radial dimension. If you pick a circle, you get a diameter dimension, while selecting two parallel lines creates a linear dimension between them. 2.3.9.4 Dimensioning a Sketch i) You dimension 2D or 3D sketch entities with the Smart Dimension tool. ii) You can drag or delete a dimension while the Smart Dimension tool is active. iii) Click Smart Dimension on the Dimensions/Relations toolbar, or click Tools, Dimensions, Smart. The default dimension type is Parallel. iv) Select the items to dimension, as shown in the table 1. v) As you move the pointer, the dimension snaps to the closest orientation. vi) Click to place the dimension. 2 - 12 SolidWorks Module Unit 2 – Sketching Table 1: Item to be Dimensioning To dimension the... Click... Note: Length of a line or edge The line. Angle between two lines Two lines, or a line and Placement of the a model edge. dimension affects the way the angle is measured. Distance between two Two parallel lines or a lines line and a parallel model edge. Perpendicular distance The point and the line or from a point to a line model edge. Distance between two Two points. One of the points can be points a model vertex. Radius of an arc The arc. True length of an arc The arc, then the two end points. Diameter of a circle The circumference. Displayed as linear or diameter, depending on placement. Distance when one or The centerpoint or the By default, distance is both entities is an arc or circumference of the arc measured to the a circle or circle, and the other centerpoint of the arc or entity (line, edge, point, circle, even when you etc.). select the circumference. Midpoint of a linear Right-click the edge You can also dimension edge whose midpoint you to midpoints when you want to dimension and add baseline or ordinate click Select Midpoint. dimensions. Then select the second entity to dimension. 2 - 13 SolidWorks Module Unit 2 – Sketching 2.3.10 Others Important 2D Sketch Command 2.3.10.1 Fillet Rounds the corner at the intersection of two sketch entities, creating a tangent arc. before after Figure 3.3: Before and after fillet command The radius value stays in effect until you change it. Therefore, you can draw any number of fillets with the same radius. i. In an open sketch, click Sketch Fillet on the Sketch toolbar, or Tools, Sketch Tools, Fillet. ii. Set the properties in the Sketch Fillet PropertyManager. iii. Select the sketch entities to fillet. To select the sketch entities, you can: i. Hold Ctrl and select two sketch entities. ii. Select a corner. Click OK to accept the fillet, or click Undo to remove the fillet. You can undo a sequence of fillets in reverse order. 2.3.10.2 Offset Adds sketch entities by offsetting faces, edges, curves, or sketch entities a specified distance. To create a sketch offset: i. In an open sketch, select one or more sketch entities, a model face, or a model edge. ii. Click Offset Entities on the Sketch toolbar, or click Tools, Sketch Tools, Offset Entities. iii. In the PropertyManager, under Parameters, set the following: 2 - 14 SolidWorks Module Unit 2 – Sketching ¾ When you click in the graphics area, the Offset Entity is complete. Set the Parameters before you click in the graphics area. ¾ Offset Distance. Set a value to offset the sketch entity by a specified distance. To see a dynamic preview, hold down the mouse button and drag the pointer in the graphics area. When you release the mouse button, the Offset Entity is complete. ¾ Add dimensions. Include the Offset Distance in the sketch. This does not affect any dimensions included with the original sketch entity. ¾ Reverse. Change the direction of a one-directional offset. ¾ Select chain. Create an offset of all adjacent sketch entities. ¾ Bi-directional. Create offset entities in two directions. o ¾ Make base construction. Convert the original sketch entity to a construction line. ¾ Cap ends. Extend the original non-intersecting sketch entities by selecting Bi-directional, and adding a cap. You can create Arcs or Lines as extension cap types. iv. Click OK or click in the graphics area. 2 - 15 SolidWorks Module Unit 2 – Sketching To change the size of a sketch offset: Double-click the offset’s dimension and change the value. In a bi- directional offset, change the dimensions of the two offsets individually. 2.3.10.3 Convert Entities Converts selected model edges or sketch entities into sketch segments by projecting selected edge, loop, face and curve onto the sketch plane. Rather than drawing the outlines by hand, they are “copied” from existing geometry. This technique is: o Fast and easy– select the face and click the tool. o Accurate – sketch entities are “cloned” directly from existing geometry. o Intelligent – if the solid body changes shape, the sketch updates. Automatically. To convert an entity: i. In an open sketch, click a model edge, loop, face, curve, external sketch contour, set of edges, or set of curves. ii. Click Convert Entities on the Sketch toolbar, or click Tools, Sketch Tools, Convert Entities. 2.3.10.4 Trim Entities Trim or extends a sketch entity to be coincident to another, or deletes a sketch entity. There are five trim options: o Power trim ο Trim away outside o Corner ο Trim to closest o Trim away inside 2 - 16 SolidWorks Module Unit 2 – Sketching Power Trim Use Power trim to: o Trim multiple, adjacent sketch entities by dragging the pointer across each sketch entity. o Extend sketch entities along their natural paths. To trim with the Power trim option: i. Right-click the sketch and select Edit Sketch. ii. Click Trim Entities Sketch toolbar) or Tools, Sketch Tools, Trim. iii. Select Options, Power trim. iv. Click in the graphics area next to the first entity, and drag across the sketch entity to trim. vi. Continue to hold down the pointer and drag across each sketch entity you want to trim. vii. Release the pointer when finished trimming the sketch, then click OK. To extend with the Power trim option: i. Follow steps 1 - 3 from the preceding procedure. ii. Select anywhere along the sketch entity to extend. iii. Click and drag the pointer as far as you want to extend the sketch entity. iv. Release the pointer when finished extending the sketch entity, then click OK. 2 - 17 SolidWorks Module Unit 2 – Sketching Corner Extends or trims two sketch entities until they intersect at a virtual corner. To trim with the Corner option: i. Right-click the sketch and select Edit Sketch. ii. Click Trim Entities on the Sketch toolbar, or click Tools, Sketch Tools, Trim. iii. Select Options, Corner. iv. Select the two sketch entities you want to joined. v. Click OK. Trim Away Inside Trims open sketch entities that lie inside two bounding entities. To trim with the Trim away inside option: i. Right-click the sketch and select Edit Sketch. ii. Click Trim Entities on the Sketch toolbar, or click Tools, Sketch Tools, Trim. iii. Select Options, Trim away inside. iv. Select two bounding sketch entities. v. Select the sketch entities to trim. vi. Click OK. 2 - 18 SolidWorks Module Unit 2 – Sketching Trim Away Outside Trims open sketch entities outside of two bounding entities. The same rules that govern the Trim away inside option govern the Trim away outside option. Trim to Closest i. Right-click the sketch and select Edit Sketch. ii. Click Trim Entities on the Sketch toolbar, or click Tools, Sketch Tools, Trim. iii. Select Options, Trim to closest. The pointer changes to. iv. Select each sketch entity you want trimmed or extended to the closest intersection: v. Click OK. 2.3.10.5 Mirror Entities Create a symmetric entities corresponding to the mirrored lines. If you change a mirrored entity, its mirror image also changes. To mirror existing sketch entities: i. In an open sketch, click Mirror Entities on the Sketch toolbar, or click Tools, Sketch Tools, Mirror. ii. In the PropertyManager: a. Select sketch entities for Entities to Mirror. b. Clear Copy to remove the original sketch entities or Select Copy to include the original sketch entities. c. Select an edge or a line to Mirror about. iii. Click OK. 2 - 19 SolidWorks Module Unit 2 – Sketching Mirror line Mirror entities 2.4 ACTIVITIES Exercise 1 Create this sketch on the front plane using, lines, automatic relation and dimension. Fully define the sketch. All dimensions are in inches. Next select sketch fillet and set the Radius to 0.1875”. Select all of the endpoints in the sketch. 2 - 20 SolidWorks Module Unit 2 – Sketching Exercise 2 Create this sketch on the front plane using, lines, automatic relation and dimension. Fully define the sketch. All dimensions are in mm. Exercise 3 Create this sketch on the front plane using, lines, automatic relation and dimension. Fully define the sketch. All dimensions are in mm. Ellipse Major axis 149 Minor axis 75 2 - 21 SolidWorks Module Unit 2 – Sketching 2.5 REFERENCES 1. SolidWorks Essentials - SolidWorks 2007 Training Manual, Massachusetts, USA. 2. SolidWorks 2007 Online User’s Guide – SP0.0 3. SolidWorks 2005 – Hand-on Quick Start 2 - 22 SolidWorks Module Unit 3 – Basic Modeling Technique UNIT 3 BASIC MODELING TECHNIQUE 3.1 INTRODUCTION This Module discusses 3D Modeling Terminology, Profile selection, Views, Extruded boss/base, Extruded cut, Revolved boss/base, Revolved cut, Swept boss/base, Lofted boss/base, Fillet, Chamfer, Rib, Mirror, Shell, Draft, Hole wizard, linear pattern, circular pattern, Reference, Helix/Spiral, Sectioning, editing and repairing problem, Configuration. 3.2 LEARNINGS OUTCOMES Upon successful completion of this lesson, you will be able to: Choose the best profile for sketching. Choose the proper sketch plane. Create a new part. Extrude a sketch as a boss. Extrude a sketch as a cut. Create hole wizard holes. Create revolved features. Create a sweep features. Create a loft features. Perform shelling operations to hollow out a part. Use rib tool. Use geometry pattern (linear, circular and mirror) properly. Insert fillets on a solid. Diagnose various problems in a part. Repair sketch geometry problems. Repair dangling relations and dimensions. Create reference planes. Use configurations to represent different versions of a part within a single SolidWorks file. Suppress and unsuppress features. Change dimension values by configuration. 3-1 SolidWorks Module Unit 3 – Basic Modeling Technique 3.3 LEARNING CONTENTS 3.3.1 3D Modeling Terminology 3-2 SolidWorks Module Unit 3 – Basic Modeling Technique 3.3.2 Choosing the Best Profile Choose the “best” profile. This profile, when extrude, will generate more of the model than any other. Look at these models as examples. 3-3 SolidWorks Module Unit 3 – Basic Modeling Technique 3.3.3 Choosing the Sketch Plane Profile will contact or be parallel to one of the three planes. Things to consider when choosing the sketch planes. o The part appearance in standard views o The part orientation in an assembly o The part appearance in detail drawing profile Figure 3.1: View of finalize model if selecting different Plane orientation 3.3.4 Features and Commands Base Feature o The first feature that is created. o The foundation of the part. o The base feature geometry for the box is an extrusion. o The extrusion is named Extrude1. o Tip: Keep the base feature simple. 3-4 SolidWorks Module Unit 3 – Basic Modeling Technique Features Used to Build Extruded Boss Feature o Adds material to the part. o Requires a sketch. Extruded Cut Feature o Removes material from the part. o Requires a sketch. Fillet Feature o Rounds the edges or faces of a part to a specified radius. Shell Feature o Removes material from the selected face. o Creates a hollow block from a solid block. o Very useful for thin-walled, plastic parts. o You are required to specify a wall thickness when using the shell feature. 3-5 SolidWorks Module Unit 3 – Basic Modeling Technique 3.3.5 Views 3-6 SolidWorks Module Unit 3 – Basic Modeling Technique 3-7 SolidWorks Module Unit 3 – Basic Modeling Technique 3-8 SolidWorks Module Unit 3 – Basic Modeling Technique 3.3.6 Revolve Feature A Revolve feature is created by rotating a 2D profile sketch around an axis of revolution. The profile sketch can use a sketch line or a centerline as the axis of revolution. The profile sketch cannot cross the axis of revolution. To Create a Revolve Feature: 1. Select a sketch plane. 2. Sketch a 2D profile. 3. (Optional) Sketch a centerline. 9 The axis of revolution must be in the sketch with the profile. It cannot be in a separate sketch. 9 The profile must not cross the centerline. 4. Click Revolved Boss/Base. 5. Specify the angle of rotation and click OK. The default angle is 360°. 6. The sketch is revolved around the axis of revolution, creating the feature. centerline 3-9 SolidWorks Module Unit 3 – Basic Modeling Technique 3.3.7 Sweep Feature The Sweep feature is created by moving a 2D profile along a path. A Sweep feature is used to create the handle on the candlestick. The Sweep feature requires two sketches: o Sweep Path o Sweep Profile Sweep Overview – Rules The sweep path is a set of sketched curves contained in a sketch, a curve, or a set of model edges. The sweep profile must be a closed contour. The start point of the path must lie on the plane of the sweep section. The section, path or the resulting solid cannot be self-intersecting. 3.3.8 Loft Feature Blends multiple profiles together. A Loft feature can be a base, boss, or cut. 3 - 10 SolidWorks Module Unit 3 – Basic Modeling Technique To Create a Simple Loft Feature: 1. Create the planes required for the profile sketches. Each sketch should be on a different plane. 2. Sketch a profile on the first plane. 3. Sketch the remaining profiles on their corresponding planes. 4. Click Loft on the Features toolbar. 5. Select each profile. 6. Examine the preview curve and the connectors. 7. Click OK. 3 - 11 SolidWorks Module Unit 3 – Basic Modeling Technique 3.3.9 Fillet Feature Fillet/Round creates a rounded internal or external face on the part. You can fillet all edges of a face, selected sets of faces, selected edges, or edge loops. To create fillets: 1. Click Fillet on the Features toolbar, or click Insert, Features, Fillet/Round. 2. Set the PropertyManager options. For constant radius fillets only, you can use the FilletXpert to add or modify fillets. 3. Click OK 3.3.10 Chamfer Feature Creates a beveled feature on selected edges, faces, or a vertex. To create a chamfer: 1. Click Chamfer on the Features toolbar, or click Insert, Features, Chamfer. 2. Under Chamfer Parameters: Select an entity in the graphics area for Edges and Faces or Vertex. Select one of the following: Angle distance Distance distance Vertex 3 - 12 SolidWorks Module Unit 3 – Basic Modeling Technique Choose Select through faces to enable selection of edges through faces that hide the edges. Select Equal Distance to specify a single value for distance or vertex. Select Keep features to retain features such as cuts or extrudes that would otherwise be removed when you apply the chamfer. Original part Keep features cleared Keep features checked Select Tangent propagation to extend the chamfer to faces or edges that are tangent to the selected entity. Select a preview mode: Full preview, Partial preview, or No preview. 3. Click OK 3.3.11 Rib Feature 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. 3 - 13 SolidWorks Module Unit 3 – Basic Modeling Technique 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 on the Features toolbar, or click Insert, Features, Rib. 3. Set the PropertyManager options. 4. Click OK 3.3.12 Draft Feature Tapers model faces by a specified angle, using a neutral pane or a parting line.. Use to make a molded part easier to remove from the mold. To draft a model face: 1. Click Draft (Features toolbar) or Insert, Features, Draft. 2. Set the options in the PropertyManager. 3. Click OK 3 - 14 SolidWorks Module Unit 3 – Basic Modeling Technique 3.3.13 Hole Wizard Insert a hole using a pre-defined cross-section. Two tabs appear at the Hole Wizard propertymanager: Type (default). Sets the hole type parameters. Positions. Locates the Hole Wizard holes on planar or non-planar faces. Use the dimension and other sketch tools to position the hole centers. Hole type Counterbore Countersink Hole Tap Pipe tap Legacy Hole To create Hole Wizard holes: 1. Create a part and select a planar surface. 2. Click Hole Wizard on the Features toolbar or Insert, Features, Hole, Wizard. 3. Set the options in the PropertyManager. 4. Click OK 3.3.14 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. Mirror copies the selected features or all features, mirroring them about the selected plane or face 3 - 15 SolidWorks Module Unit 3 – Basic Modeling Technique 3 - 16 SolidWorks Module Unit 3 – Basic Modeling Technique 3 - 17 SolidWorks Module Unit 3 – Basic Modeling Technique 3.3.15 Reference Geometry The Reference Geometry toolbar provides tools for creating and using reference geometry. Plane Axis Coordinate System Point Creating Plane 1. Click Plane on the Reference Geometry toolbar, or click Insert, Reference Geometry, Plane. The Plane PropertyManager appears. 2. Under Selections, select the type of plane you want to create and the items to create the plane: ¾ Through Lines/Points. Create a plane through an edge, axis, or sketch line, and a point, or through three points. ¾ Parallel Plane at Point. Create a plane through a point parallel to a plane or face. Select a face or planar face. Then select a midpoint. The new plane is parallel to the selected face through the chosen midpoint. 3 - 18 SolidWorks Module Unit 3 – Basic Modeling Technique ¾ At Angle. Create a plane through an edge, axis, or sketch line at an angle to a face or plane. If the selected line is in the same plane If the selected line is parallel to the selected as the selected plane, the new plane plane, the new plane moves to the parallel rotates around the selected line. line and rotates around the line. ¾ Offset Distance. Create a plane parallel to a plane or face, offset by a specified distance. This is the default plane created. ¾ Normal to Curve. Create a plane through a point and perpendicular to an edge or curve. In this example, you select just the helix to A circle is swept along the create the new plane. Plane 4 is perpendicular helix to create a spring. to the end of the tapered helix. 3 - 19 SolidWorks Module Unit 3 – Basic Modeling Technique ¾ On Surface. Create a plane on a non-planar face or angular surface. a. Select a surface. b. Select a sketch point on the surface ¾ Drag and Drop. You can also drag and drop to create a plane. The selected items appear in the Reference Entities box. A preview of the new plane appears in the graphics area. 3. Click OK to create the plane. Creating 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. ¾ One Line/Edge/Axis. Select a sketch line, an edge, or select View, Temporary Axes and then select the axis that is displayed. ¾ Two Planes. Select two planar faces, or select View, Planes, and then select two planes. ¾ Two Points/Vertices. Select two vertices, points, or midpoints. ¾ Cylindrical/Conical Face. Select a cylindrical or conical face. ¾ Point and Face/Plane. Select a surface or plane and a vertex point, or midpoint. The resultant axis is normal to the selected surface or plane through the selected vertex, point, or midpoint. If the surface is non-planar, the point must be on the surface. 3 - 20 SolidWorks Module Unit 3 – Basic Modeling Technique 3. Verify that the items listed in Reference Entities correspond to your selections. 4. Click OK. 5. Click View, Axes to see the new axis. Display Temporary Axis You can use an axis in creating sketch geometry or in a circular pattern. Every cylindrical and conical face has an axis. Temporary axes are those created implicitly by cones and cylinders in the model. To display temporary axes: Click View, Temporary Axes. Creating Coordinate System You can define a coordinate system for a part or assembly. Use this coordinate system with the Measure and Mass Properties tools, and for exporting SolidWorks documents to IGES, STL, ACIS, STEP, Parasolid, VRML, and VDA. To create a coordinate system: 1. Click Coordinate System on the Reference Geometry toolbar, or click Insert, Reference Geometry, Coordinate System. 2. Use the Coordinate System PropertyManager to create the coordinate system. 3. Click OK 3 - 21 SolidWorks Module Unit 3 – Basic Modeling Technique Creating Point Use as construction objects. Can also create multiple reference points that are a specified distance apart on curves. Click View, Points to toggle the display of reference points. 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. Click OK 3.3.16 Families of Parts Many times parts come in a variety of sizes. This is called a family of parts. It is not efficient to build each version individually. Design Tables simplify making families of parts. 3 - 22 SolidWorks Module Unit 3 – Basic Modeling Technique What is a Configuration? A configuration is a way to create a family of similar parts within one file. Each configuration represents one version of the part. Suppress / Unsuppress (also known as revolved) Feature Suppress is used to temporarily remove a feature. When a feature is suppressed, the system treats it as if it doesn’t exist. That means other features that are dependent on it will be suppressed also. In addition, suppressed features are removed from memory, freeing up system resources. Suppressed features can be unsuppressed at any time. To create a configuration manually: 1. In either a part or assembly document, click the ConfigurationManager tab at the top of the FeatureManager design tree to change to the ConfigurationManager. 2. In the ConfigurationManager, right-click the part or assembly name and select Add Configuration. 3. In the Add Configuration PropertyManager, type a Configuration Name and specify properties for the new configuration. You can specify a configuration specific color. 4. Click. 5. Click the FeatureManager design tree tab to return to the FeatureManager design tree. 6. Modify the model as needed to create the design variation. 7. Save the model. To activate a different configuration: 1. Click the ConfigurationManager tab to change to the ConfigurationManager. 2. Right-click the name of the configuration you want to view and select Show Configuration or Double-click the configuration name. The named configuration becomes the active configuration, and the view of the model updates to reflect the newly selected configuration. 3 - 23 SolidWorks Module Unit 3 – Basic Modeling Technique 3.4 ACTIVITIES Exercise 1 Create this part using the information and dimensions provided. Sketch and extrude profiles to create the part. Exercise 2 Use the following graphics to create the part. 3 - 24 SolidWorks Module Unit 3 – Basic Modeling Technique Exercise 3 Use the following graphics to create the part. Holes are concentric to circular edges created by fillets and rounds. 3 - 25 SolidWorks Module Unit 3 – Basic Modeling Technique Exercise 4 Create this part using the dimension provided. Use relations and equations where applicable to maintain the design intent. Give careful thought to the best location for the origin. Design intent The design intent for this part is as follow: 1. The part is symmetrical. 2. Front holes on centerline. 3. All fillets and round are R 3mm unless noted. 4. Center holes in Front and Right share a common centerpoint. Dimension in mm: SECTION A-A 3 - 26 SolidWorks Module Unit 3 – Basic Modeling Technique Exercise 5 Build this part in SolidWorks. Material: 6061 Alloy. Density = 0.0027g/mm^3 Unit system: MMGS (millimeter, gram, second) Decimal places: 2. A = 100. All holes through all, unless otherwise specified. What is the overall mass of the part in grams? (2040.57 gram) 3 - 27 SolidWorks Module Unit 3 – Basic Modeling Technique Exercise 6 Build this part in SolidWorks. Unit system: MMGS (millimeter, gram, second) Decimal places: 2. Part origin: Arbitrary A = 63mm, B = 50mm, C = 100mm. All holes through all. Part material: Copper Density = 0.0089 g/mm^3 What is the overall mass of the part in grams? (1280 gram) 3 - 28 SolidWorks Module Unit 3 – Basic Modeling Technique Exercise 7 These questions are the Parametric Part Modeling. Use configuration to create these parts. ADVICE You should be able to answer all four questions correctly within 20 to 30 minutes. Read through every question first. This will help you save time and make correct decisions when choosing which sketch plane to use and which sketch profile is best. Avoid sketch fillets in this particular design. Design this part in SolidWorks. Unit system: MMGS (millimeter, gram, second) Decimal places: 2 Part origin: Arbitrary Part material: Brass Material Density: 0.0085 g/mm^3 Design note: the part is shelled throughout (single open face as shown) Question 7a: A = 60 B = 64 C = 140 D = 19 What is the overall mass of the part (in grams)? Question 7b: A = 50 B = 70 C = 160 D = 23 What is the overall mass of the part (in grams)? 3 - 29 SolidWorks Module Unit 3 – Basic Modeling Technique Update part with new features/dimensions. Unit system: MMGS (millimeter, gram, second) Decimal places: 2 Part material: Brass Material Density: 0.0085 g/mm^3 Design note: no shell remaining Question 7c: A = 60 B = 64 C = 140 D = 19 E = 25 What is the overall mass of the part (in grams)? Question 7d: A = 70 B = 80 C = 130 D = 15 E = 40 What is the overall mass of the part (in grams)? ANSWERS 7a) 1006.91 grams 7b) 1230.82 grams 7c) 2859.51 grams 7d) 3218.14 grams 3 - 30 SolidWorks Module Unit 3 – Basic Modeling Technique 3.5 REFERENCES 1. SolidWorks Essentials - SolidWorks 2007 Training Manual, Massachusetts, USA. 2. SolidWorks 2007 Online User’s Guide – SP0.0 3. SolidWorks 2005 – Hand-on Quick Start 3 - 31 SolidWorks Module Unit 4 – Assembly Parts UNIT 4 ASSEMBLY PARTS 4.1 INTRODUCTION This module will examine assembly modeling through the construction of a universal joint. The joint consists of several components and one sub- assembly. Bottom-Up assembly will be used in this module. This type of assemblies is created by adding and orienting existing parts in an assembly. Parts added to the assembly appear as Component Parts. Component parts are oriented and positioned in the assembly using Mates. Mates relate faces and edges of component parts to planes and other faces/edges. The contents of this module are Insert component, Apply Toolbox components, Move Component, Rotate Component, Mating, Interference detection, Components explode, Animation and simulation. 4.2 LEARNING OUTCOMES Upon successful completion of this module, you would be able to: create a new assembly insert components into an assembly using all available techniques. add mating relationships between components. utilize the assembly-specific aspects of the FeatureManager design tree to manipulate and manage the assembly. insert sub-assemblies. use part configurations in an assembly. 4.3 LEARNING CONTENTS 4.3.1 Assemblies 4.3.1.1 Overview You can build complex assemblies consisting of many components, which can be parts or other assemblies, called sub-assemblies. For most operations, the behavior of components is the same for both types. Adding 4-1 SolidWorks Module Unit 4 – Assembly Parts 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. The document name extension for assemblies is.sldasm. To create an assembly from a part: 1) Click Make Assembly from Part/Assembly (Standard toolbar) or File, Make Assembly from Part. An assembly opens with the Insert Component PropertyManager active. 2) Click in the graphics area to add the part to the assembly. SolidWorks makes the first component fixed. 4.3.1.2 FeatureManager Design Tree Conventions The FeatureManager design tree displays these items for assemblies: ¾ Top-level assembly (the first item) ¾ Various folders, for example, Annotations and Mates ¾ Assembly planes and origin ¾ Components (sub-assemblies and individual parts) ¾ Assembly features (cuts or holes) and component patterns You can expand or collapse each component to view its details by clicking beside the component name. To collapse all the items in the tree, right- click anywhere in the tree and select Collapse Items. You can use the same component multiple times within an assembly. For each occurrence of the component in the assembly, the suffix is incremented. In the FeatureManager design tree, a component name can have a prefix that provides information about the state of its relationships to other components. The prefixes are: 4-2 SolidWorks Module Unit 4 – Assembly Parts ¾ (-) under defined ¾ (+) over defined ¾ (f) fixed ¾ (?) not solved The absence of a prefix indicates that the component’s position is fully defined. See Mate Errors for information about mate symbols and error messages. 4.3.1.3 Display of Components Sometimes you want to focus on the structure or hierarchy of the design rather than the details of the sketches and features. In addition, you might want to focus on the design of the assembly without viewing all of the features of the components. Each of these ways of viewing the assembly affects only the level of detail displayed in the FeatureManager design tree, not the assembly itself. To display the assembly hierarchy: ¾ Right-click the assembly name in the FeatureManager design tree, and select Show Hierarchy Only. The FeatureManager design tree displays only the components (both parts and sub-assemblies), but no lower level detail. ¾ To display the detail again, repeat the procedure, selecting Show Feature Detail. To view an assembly by dependencies: ¾ To display the dependencies, right-click the assembly name in the FeatureManager design tree and select Tree Display, View Mates and Dependencies or click View, FeatureManager Tree, By Dependencies. Dependent items (instead of features) are listed under each component. Dependent items include mates and component patterns. To view a component's features and planes, expand the Features folder under the component. 4-3 SolidWorks Module Unit 4 – Assembly Parts ¾ To display the features again, right-click the assembly name in the FeatureManager design tree and select Tree Display, View Features or click View, FeatureManager Tree, By Features. 4.3.1.4 Adding Components to an Assembly When you place a component (either an individual part or a sub-assembly) in an assembly, the component file is linked to the assembly file. The component appears in the assembly; the component data remains in the source component file. Any changes you make to the component file update the assembly. There are many ways to add components to a new or existing assembly: ¾ Use the Insert Component PropertyManager. ¾ Drag from the File Explorer tab in the Task Pane. ¾ Drag from an open document window. ¾ Drag from Windows Explorer. ¾ Drag a hyperlink from Internet Explorer. ¾ Drag within the assembly for additional instances of existing components. ¾ Drag from the Design Library in the Task Pane. ¾ Use Insert, Smart Fasteners to add bolts, screws, nuts, pins, and washers. 4.3.1.5 Design Method You can create assemblies using bottom-up design, top-down design, or a combination of both methods. Bottom-up Design 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. 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. 4-4 SolidWorks Module Unit 4 – Assembly Parts Top-down Design In Top-down design, parts' shapes, sizes, and locations can be designed in the assembly. For example: ¾ 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. You can also use top-down design on certain features (such as locating pins) of otherwise bottom-up parts. ¾ The design of photocopier can be laid out in a layout sketch, whose elements represent the pulleys, drums, belts, and other components of the photocopier. You create the 3D components based on this sketch. As you move or resize elements in the sketch, SolidWorks automatically moves or resizes the 3D components in the assembly. The speed and flexibility of the sketch allows you to try several versions of the design before building any 3D geometry, and to make many types of changes in one central location. 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. You can use top-down design techniques on certain features of a part, complete parts, or entire assemblies. In practice, designers typically use top-down techniques to lay out their assemblies and to capture key aspects of custom parts specific to their assemblies. 4-5 SolidWorks Module Unit 4 – Assembly Parts 4.3.2 Moving and Rotating Components 4.3.2.1 Moving a Component To move components by dragging: ¾ Drag a component in the graphics area. ¾ The component moves within its degrees of freedom. To prevent this behavior, click Tools, Options, System Options, Assemblies. Clear Move components by dragging, then click OK. To move components with a triad: 1) Right-click a component and select Move with Triad Figure 4.1: Move with Triad 2) Drag elements of the triad: ¾ Dragging the center ball drags the component freely. ¾ Dragging an arm drags the component along that axis of the arm. ¾ Dragging a wing drags the component along the plane of the wing. 3) To type specific coordinates or distances, right-click the center sphere and select from the following: ¾ Show Translate XYZ Box. Moves the component to a specific XYZ coordinate. ¾ Show Translate Delta XYZ Box. Moves the component by a specific amount. 4) Click in the graphics area to turn off the triad. See Triad for information about moving and aligning the triad. 4-6 SolidWorks Module Unit 4 – Assembly Parts To move components with the PropertyManager: 1) Click Move Component (Assembly toolbar) or Tools, Component, Move. The Move Component PropertyManager appears, and the pointer changes to. 2) Select one or more components in the graphics area. 3) Select an item from the Move list to move the components in one of following manners: ¾ Free Drag - Select a component and drag in any direction. ¾ Along Assembly XYZ - Select a component and drag in the X, Y, or Z direction of the assembly. The coordinate system appears in the graphics area to help orient you. To select the axis you want to drag along, click near that axis before dragging. ¾ Along Entity - Select an entity, then select a component to drag along that entity. If the entity is a line, an edge, or an axis, the component you move has one degree of freedom. If the entity is a plane or a planar face, the component you move has two degrees of freedom. ¾ By Delta XYZ - Type an X, Y, or Z value in the PropertyManager, and click Apply. The component moves by the amount you specify. ¾ To XYZ Position - Select a point of a component, type an X, Y, or Z coordinate in the PropertyManager, and click Apply. The component’s point moves to the coordinate you specify. If you select something other than a vertex or point, the component’s origin is placed at the coordinate you specify. You can select and move one component or group of components after another while the Move Component tool is active. 4) Under Advanced Options, select This configuration to apply the movement of the components to only the active configuration. 5) Click or click Move Component again when finished. 4-7 SolidWorks Module Unit 4 – Assembly Parts 4.3.2.2 Rotating a Component To rotate a component by dragging: ¾Right-click a component, hold down the right mouse button, and drag the component. ¾The component rotates within its degrees of freedom. To prevent this behavior, click Tools, Options, System Options, Assemblies. Clear Move components by dragging, then click OK. To rotate a component with a triad: 1) Right-click a component and select Move with Triad. 2) Select a ring and drag. Also: ¾ To snap, right-click the selected ring and choose Snap while Dragging. Close to the ring, the snap increment is 90°. The increment decreases as the pointer moves further away from the ring. Figure 4.2: Select a ring and drag ¾ To rotate in pre-set increments, right-click the selected ring and choose Rotate 90° or Rotate 180°. ¾ To type specific increments, right-click the center sphere and select Show Rotate Delta XYZ Box. 3) Click in the graphics area to turn off the triad. See Triad for information about moving and aligning the triad. 4-8 SolidWorks Module Unit 4 – Assembly Parts To rotate a component with the PropertyManager: i) Click Rotate Component (Assembly toolbar) or Tools, Component, Rotate. The Rotate Component PropertyManager appears, and the pointer changes to. ii) Select one or more components in the graphics area. iii) Select an item from the Rotate list to rotate the components in one of the following manners: ¾ Free Drag - Select a component and drag in any direction. ¾ About Entity - Select a line, an edge, or an axis, then drag a component around the selected entity. ¾ By Delta XYZ - Type an X, Y, or Z value in the PropertyManager, and click Apply. The component moves around the assembly’s axes by the angular value you specify. You can rotate one component or group of components after another; the tool remains active until you click it again, or select another tool. iv) Under Advanced Options, select This configuration to apply the rotation of the components to only the active configuration. v) Click or click Rotate Component again when finished. NOTES: ¾ You cannot rotate a component whose position is fixed or fully defined. ¾ You can only rotate a component within the degrees of freedom allowed by its mating relationships. 4.3.2.3 Triad The triad facilitates manipulating various objects such as 3D sketch entities, parts, certain features, and components in assemblies. 4-9 SolidWorks Module Unit 4 – Assembly Parts Figure 4.3: The Triad The rings and wings are displayed when rotation and dragging along the wings' planes are possible. Triad actions: ¾ Dragging the center ball drags the object freely. ¾ Alt + d

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