AEROPLANE. Create a New Folder in your chosen location called Aeroplane. The four parts that make up the project will be saved here.

Size: px
Start display at page:

Download "AEROPLANE. Create a New Folder in your chosen location called Aeroplane. The four parts that make up the project will be saved here."

Transcription

1 AEROPLANE Prerequisite Knowledge Previous knowledge of the following commands is required to complete this lesson. Sketching (Line, Rectangle, Arc, Add Relations, Dimensioning), Extrude, Assemblies and Creating a drawing from Part/Assembly. Focus of the Lesson On completion of this lesson you will have used: Cut Extrude with a line. Edit Appearance. Variable Fillet. Created an Assembly. Mate with planes. Exploded view of an assembley. Animation of exploded view Commands Used This lesson includes Sketching (line, circle, arc, ellipse Smart Dimension), Cut Extrude with a line, Add relations, Appearance, Variable Fillet, Assemblies, Mates, Exploded View, and Animation. Getting started Create a New Folder in your chosen location called Aeroplane. The four parts that make up the project will be saved here. Design & Communication Graphics 1

2 Part One Aeroplane Body Open New Part from the SolidWorks Document dialog box. Select File. Click Save as on the standard toolbar. Save as aeroplane body. in the Aeroplane folder. Continue to save periodically throughout the exercise. Create sketch Create a sketch on the Front Plane using the dimensions shown. Confirm the sketch. Extrude the sketch to a depth of 30mm. Use Mid Plane End Condition. Rename the extrusion as Main Body. Sketching recess for Back Wing On the front face draw the Rectangle shown. Add the dimensions shown to fully define the sketch. Exit the sketch. Select Extrude Cut, Through All. Sketching the Sloped Tail Section On the front face draw the line shown to the following dimensions. Confirm the sketch. Design & Communication Graphics 2

3 Select Extrude Cut and Through All Flip the side to cut if necessary. Rename Extrusion as Underside. Sketching Recess for Front Wing Draw the Rectangle to the dimensions shown on the front face. Extrude cut, Through all as before. Sketching Front Screen. On the front face sketch the profile to the dimensions shown. In the feature manager select Extrude Cut, Through all. Flip the side to cut if necessary. Sketching the Nose Section Using the Centerline command draw the line as shown. Select the Ellipse command and select the Midpoint of the centerline as the centre of the ellipse. Design & Communication Graphics 3

4 Select the minor and major axis as shown. Use the Trim command to remove the unwanted portion of the ellipse. Using Add Relations make the line and end of the major axis coincident, to fully define the sketch. As before select Extrude Cut and Through all. Flip the side to cut if necessary. Rename the extrusion as Nose Section Shaping front section In the feature manager select Chamfer and apply a 6mm chamfer to the edges shown. Applying Fillets Select Fillet and select Variable radius as shown. Design & Communication Graphics 4

5 Select the edges to fillet as shown. In the variable windows parameter box select Variable radius1 (V1) and type a radius of 6mm as shown. Select the next chain of edges and give them the following radii. Design & Communication Graphics 5

6 Applying the Stopped chamfers Step 1 Set up a plane perpendicular to the chamfer Select plane under Reference Geometry To draw the plane at the required angle, select the top face and the edge to be chamfered. Change the angle to 45 degrees as shown. Step 2 Draw the profile on this plane to the dimensions given. Step 3 Select Extrude Cut as shown Rename the extrusion as Stopped Chamfer Mirroring the Stopped Chamfer Select Mirror Components Design & Communication Graphics 6

7 Select the Front Plane from the design tree, as the mirror plane. Select Stopped chamfer from the design tree as the feature to mirror. Edit Material In the design tree right click on Edit material shown. Apply a pine texture to the object from the wood menu. Apply a grain 2 texture to the faces that contain end grain. Save Design & Communication Graphics 7

8 Part two - Front Wing Open New Part Save part as Front wing in the Aeroplane folder Sketch Sketch on the Top Plane the shape shown. Draw the Centerline and add the following relations. Add the following dimensions. Select Mirror and mirror about the centerline. Accept the sketch and Extrude by 12mm. Rename the extrusion as Front wing. Select chamfer and apply a 3mm chamfer to the four edges shown. Edit Material Apply a pine texture to the wing. Apply a grain 2 texture to the end grain. Save the part Design & Communication Graphics 8

9 Part three - Horizontal Tail Wing Open New Part Save part as Horizontal tail wing in the Aeroplane folder. Sketch Sketch a Rectangle on the Front Plane as shown. Extrude using Mid Plane a distance of 110mm. On the top surface draw the rectangle to the measurements given. Accept the sketch. Extrude cut the rectangles through all. Mirror the feature about the Front Plane as shown. Accept. Apply a 4mm chamfer to the following edges. Edit Material Apply a pine texture to the part Apply a grain 2 texture to the end grain. Save the part. Design & Communication Graphics 9

10 Part Four - Vertical Tail Wing Open New Part Save part as Vertical tail wing in the Aeroplane folder. Sketch On the Front Plane sketch the Rectangle to the following dimensions. Extrude by 12mm. Apply a Chamfer of 15mm to the top edge. Sketch another rectangle on the front face. Extrude cut, Through all. Apply 4mm chamfers to the following edges. Edit Material Apply a pine texture to the part Apply a grain 2 texture to the end grain. Save the part. Design & Communication Graphics 10

11 Aeroplane Assembly The part files for this assembly are saved in the folder titled Aeroplane. Open an existing part Open the part called Aeroplane body. Click Make Assembly from Part/Assembly. Insert component dialog box appears with Aeroplane body displayed. Click on in the property manager. The part origin will snap to the origin of the assembly. Save Select File, Save as on the standard toolbar. Save the assembly as Aeroplane Assembly in the same folder as its parts. Adding Component Select Insert component from the Assembly toolbar. Choose Browse from the Insert Component dialog box. Choose Front Wing and click in the graphics area to place it in as shown. Insert Mates Select the mate toolbar. Mate the front face of the trench on the aeroplane body with the bottom of the trench on the wing. A Coincident Mate will be selected by default. Accept. Design & Communication Graphics 11

12 Mate the bottom of the trench on the body with the underside of the wing. Accept Finally mate the side of the body with the side of the trench on the wing Accept Select OK again to exit the property manager. Adding Further Parts Select Insert Component from the assembly toolbar. Choose the horizontal tail wing. Insert Mates Mate the front of the horizontal tail with the shoulder shown A Concentric Mate will be chosen by default. Accept this mate. Mate the underside of the tail wing with the recess Additional Mates The horizontal tail wing has to be centered on the plane body One way to do this is as follows. Expand the design trees of the two parts and mate the Front planes of each as shown.. Design & Communication Graphics 12

13 A coincident mate is selected by default Accept the mate. Select OK again to exit the property manager. Adding Vertical Tail Wing Select Insert Component from the assembly toolbar Choose the Vertical tail wing and drag it into position. Insert Mates Mate the bottom of each trench. Accept. Mate the side of the vertical tail with the side of the trench on the horizontal wing Accept Mate the side of the trench on the vertical tail with the side of the horizontal wing Accept. Select OK again to exit the property manager. Follow the process again to insert the other vertical tail wing. Design & Communication Graphics 13

14 Exploded View Click the Exploded View button on the Assembly toolbar. The Exploded view dialog box appears. Exploding Front wing To move the front wing, select it as shown Explode View Explode by one of two methods: 1) Dragging the relevant arrow (in this instance the green one) to the required distance. 2) By scrolling down the explode property manager and selecting the part to explode as shown. Select the direction (x, y or z) by clicking the relevant arrow, and insert the distance Select Apply to preview the selection. Select Done to accept. Select ok to exit the property manager. Design & Communication Graphics 14

15 Exploding the Vertical Tail Wings Select the Explode View button again. Select the two vertical tail wings. The move manipulator arrows appear. Select the X direction arrow and drag outwards or insert a distance of 80mm as shown. Accept Explode the Horizontal Tail Wing Select Exploded view as before. Select the horizontal tail wing. Drag the green arrow away from the assembly. Insert the distance of 80mm. Click Apply and Done. Accept Design & Communication Graphics 15

16 Saving the desired Exploded view Press the space bar to show the Orientation dialog box. Select New View as shown. Name it as Front Pictorial This view is now added to the list of views. Animating the Exploded View The Animation Controller can be used to animate the explode or collapse motion. Right click on Aeroplane Assembly as shown and select Animation collapse. The animation controller display appears. Select play or loop. The Collapse motion will be shown. Design & Communication Graphics 16

17 To show the Animation Explode motion, Select the animation explode in the same way. Save Save AEROPLANE ASSEMBLY in the Collapsed View Creating the Drawing To make drawing from Part/Assembly see the notes on Creating Drawings from R6 in-service. Click on Make Drawing in the Standard Icon Toolbar as shown. Choosing a Drawing Template Select the A3L template Select OK Model View The Model View property manager is displayed In the property manager make sure the front view is selected. Tick the preview button. Design & Communication Graphics 17

18 Scale Set the scale to 1:1.5. Ensure that start projected view is ticked so that further views are projected once the first one is positioned. Positioning the Views Position the front view on the sheet. Drag the courser to the right to project an end view. Drag down to project a plan. Project an isometric view by dragging the courser to the top corner of the front view shown. To position this isometric view in the required location hold down the ctrl key while dragging. Change the scale of this view by selecting the box shown and changing the scale to 1:3 Change its display style to Shaded with Edges. Design & Communication Graphics 18

19 Inserting Dimensions Select Model items from the Annotations toolbar. Choose the entire model as the source. Tick select all dimensions. Select ok to accept. Delete some of the dimensions that are not needed. In the Annotation toolbar select Note and name the views. Drawing Exploded View Adding Sheet2 Right click on Sheet 1 tab (located at bottom left of graphics area) and select Add Sheet Change the scale to 1:1. Accept. Design & Communication Graphics 19

20 Sheet2 now becomes the current sheet Select the Drawings toolbar and Model views IN the Model view command manager select browse and open Aeroplane Assembly. The front view is selected by default. To select the desired view tick Front Pictorial as shown. Tick the preview box also. Scroll down the property manager and change the display to shaded with edges. Change the scale to 1:1 Place the drawing on the sheet. Design & Communication Graphics 20

21 To show the Exploded view right click on the box and select properties as shown. In the Properties dialog box tick the show in exploded state box. Select ok. Save. To switch between sheet 1 and sheet 2 just select sheet1 or sheet2 at the bottom of the drawing area. Exercise Complete! Design & Communication Graphics 21

22 Design & Communication Graphics 22

23 Design & Communication Graphics 23

Introduction to Parametric Modeling AEROPLANE. Design & Communication Graphics 1

AEROPLANE Design & Communication Graphics 1 Object Analysis sheet Design & Communication Graphics 2 Aeroplane Assembly The part files for this assembly are saved in the folder titled Aeroplane. Open an

Purlin Roof. Create a New Folder in your chosen location called Purlin Roof. The nine parts that make up the project will be saved here.

Purlin Roof Prerequisite Knowledge Previous knowledge of the following commands is required to complete this lesson. Sketching (Line, Rectangle, Add Relations, Dimensioning), Inserting Planes, Extrude,

Digital Camera Exercise

Commands Used New Part This lesson includes Sketching, Extruded Boss/Base, Extruded Cut, Fillet, Chamfer and Text. Click File, New on the standard toolbar. Select Part from the New SolidWorks Document

Engineering Technology

Engineering Technology Introduction to Parametric Modelling Engineering Technology 1 See Saw Exercise Part 1 Base Commands used New Part This lesson includes Sketching, Extruded Boss/Base, Hole Wizard,

Introduction to Circular Pattern Flower Pot

Prerequisite Knowledge Previous knowledge of the sketching commands Line, Circle, Add Relations, Smart Dimension is required to complete this lesson. Previous examples of Revolved Boss/Base, Cut Extrude,

SolidWorks Part I - Basic Tools SDC. Includes. Parts, Assemblies and Drawings. Paul Tran CSWE, CSWI

SolidWorks 2015 Part I - Basic Tools Includes CSWA Preparation Material Parts, Assemblies and Drawings Paul Tran CSWE, CSWI SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered

SOLIDWORKS 2016 Basic Tools

SOLIDWORKS 2016 Basic Tools Getting Started with Parts, Assemblies and Drawings Paul Tran CSWE, CSWI SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org)

Toothbrush Holder. A drawing of the sheet metal part will also be created.

Prerequisite Knowledge Previous knowledge of the following commands is required to complete this lesson; Sketch (Line, Centerline, Circle, Add Relations, Smart Dimension,), Extrude Boss/Base, and Edit

Spatula. Spatula SW 2015 Design & Communication Graphics Page 1

Spatula Introduction: The model shown in the picture is made of three parts, - the base, the washer and the handle. The base requires the use of Spline and Style Spline command, Slot command and Mirror

Introduction to Sheet Metal Features SolidWorks 2009

SolidWorks 2009 Table of Contents Introduction to Sheet Metal Features Base Flange Method Magazine File.. 3 Envelopment & Development of Surfaces.. 14 Development of Transition Pieces.. 23 Conversion to

SolidWorks Design & Technology

SolidWorks Design & Technology Training Course at PHSG Ex 5. Lego man Working with part files 8mm At first glance the Lego man looks complicated but I hope you will see that if you approach a project one

Introduction to Revolve - A Glass

Introduction to Revolve - A Glass Design & Communication Graphics 1 Object Analysis sheet Design & Communication Graphics 2 Prerequisite Knowledge Previous knowledge of the following commands are required

On completion of this exercise you will have:

Prerequisite Knowledge To complete this exercise you will need; to be familiar with the SolidWorks interface and the key commands. basic file management skills the ability to rotate views and select faces

Chair. Bottom Rail. on the Command Manager. on the Weldments toolbar.

Chapter 2 Chair Bottom Rail A. Weldments Toolbar. Step 1. Click File Menu > New, click Part and OK. Step 2. Right click Sketch on the Command Manager toolbar and select Weldments, Fig. 1. Step 3. Click

Introduction to Autodesk Inventor for F1 in Schools (Australian Version)

Introduction to Autodesk Inventor for F1 in Schools (Australian Version) F1 in Schools race car In this course you will be introduced to Autodesk Inventor, which is the centerpiece of Autodesk s Digital

Clock Exercise (Inserting Planes)

Clock Exercise (Inserting Planes) Prerequisite Knowledge To complete this exercise you will need to be familiar with Sketching, Applying relations, Extrude Boss/ Base, Extrude cut, Applying Textures, Renaming

Lab 3 Introduction to SolidWorks I Silas Bernardoni 10/9/2008

1 Introduction This lab is designed to provide you with basic skills when using the 3D modeling program SolidWorks. You will learn how to build parts, assemblies and drawings. You will be given a physical

Hydro Hull. Chapter 21. Boat. A. Save as "HYDRO". Step 1. Open your HULL MID PLANE file (Chapter 2).

Chapter 21 Boat Hydro Hull A. Save as "HYDRO". Step 1. Open your HULL MID PLANE file (Chapter 2). Step 2. Click File Menu > Save As. Step 3. Key-in HYDRO for the filename and press ENTER. B. Delete Loft1,

Sash Clamp. Sash Clamp SW 2015 Design & Communication Graphics Page 1.

Sash Clamp 1 Introduction: The Sash clamp consists of nine parts. In creating the clamp we will be looking at the improvements made by SolidWorks in linear patterns, adding threads and in assembling the

Lesson 6 2D Sketch Panel Tools

Lesson 6 2D Sketch Panel Tools Inventor s Sketch Tool Bar contains tools for creating the basic geometry to create features and parts. On the surface, the Geometry tools look fairly standard: line, circle,

Bottom Rail. Chapter 2. Chair. A. Weldments Toolbar. Step 1. Click File Menu > New, click Part and OK. B. 3D Sketch.

Chapter 2 Chair Bottom Rail A. Weldments Toolbar. Step 1. Click File Menu > New, click Part and OK. Step 2. Right click Sketch on the Command Manager toolbar and select Weldments, Fig. 1. Step 3. Click

The premium provider of learning products and solutions www.cadartifex.com EVALUATION CHAPTER 2 Drawing Sketches with SOLIDWORKS In this chapter: Invoking the Part Modeling Environment Invoking the Sketching

SolidWorks 103: Barge Design Challenge

SolidWorks 103: Barge Design Challenge Note: This tutorial was created using SolidWorks 2009. If you are using another version of SolidWorks, you may notice some variation in display states and configuration.

EXERCISE ONE: BEACH BUGGY.

EXERCISE ONE: BEACH BUGGY. Prerequisite knowledge Students should have completed Exercises from the file: Introduction to Assemblies Concept Mates Focus of lesson Commands Used This lesson will focus on

SolidWorks Basics SolidWorks Navigation Command Bar Feature Tree Model Window Simple Box Select the Front plane Create a new sketch Create a Center Rectangle from the origin Smart Dimension the length

Beginner s Guide to SolidWorks Alejandro Reyes, MSME Certified SolidWorks Professional and Instructor SDC PUBLICATIONS

Beginner s Guide to SolidWorks 2008 Alejandro Reyes, MSME Certified SolidWorks Professional and Instructor SDC PUBLICATIONS Schroff Development Corporation www.schroff.com www.schroff-europe.com Part Modeling

Quick Start for Autodesk Inventor

Quick Start for Autodesk Inventor Autodesk Inventor Professional is a 3D mechanical design tool with powerful solid modeling capabilities and an intuitive interface. In this lesson, you use a typical workflow

10/14/2010. Chevy Malibu. Vehicle Design with Solidworks. Start SolidWorks Create a New SolidWorks Document. Miles, Rowardo B

Chevy Malibu Vehicle Design with Solidworks Start SolidWorks Create a New SolidWorks Document Miles, Rowardo B 1 Click: Part and then OK Now you are ready to make a Part. 2 Right Toolbar: Document Properties:

Chapter 2. Drawing Sketches for Solid Models. Learning Objectives

Chapter 2 Drawing Sketches for Solid Models Learning Objectives After completing this chapter, you will be able to: Start a new template file to draw sketches. Set up the sketching environment. Use various

Engineering & Computer Graphics Workbook Using SolidWorks 2014

Engineering & Computer Graphics Workbook Using SolidWorks 2014 Ronald E. Barr Thomas J. Krueger Davor Juricic SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org)

SolidWorks 95 User s Guide

SolidWorks 95 User s Guide Disclaimer: The following User Guide was extracted from SolidWorks 95 Help files and was not originally distributed in this format. All content 1995, SolidWorks Corporation Contents

Engineering & Computer Graphics Workbook Using SOLIDWORKS

Engineering & Computer Graphics Workbook Using SOLIDWORKS 2017 Ronald E. Barr Thomas J. Krueger Davor Juricic SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org)

Shaft Hanger - SolidWorks

ME-430 INTRODUCTION TO COMPUTER AIDED DESIGN Shaft Hanger - SolidWorks BY: DR. HERLI SURJANHATA ASSIGNMENT Submit TWO isometric views of the Shaft Hanger with your report, 1. Shaded view of the trimetric

Introduction to CATIA V5

Introduction to CATIA V5 Release 17 (A Hands-On Tutorial Approach) Kirstie Plantenberg University of Detroit Mercy SDC PUBLICATIONS Schroff Development Corporation www.schroff.com Better Textbooks. Lower

Revit Structure 2012 Basics:

SUPPLEMENTAL FILES ON CD Revit Structure 2012 Basics: Framing and Documentation Elise Moss autodesk authorized publisher SDC PUBLICATIONS www.sdcpublications.com Schroff Development Corporation Structural

SolidWorks 2005 Tutorial. and MultiMedia CD. A Step-by-step Project Based Approach Utilizing 3D Solid Modeling

INSIDE: MultiMedia CD An audio/visual presentation of the tutorial projects SolidWorks 2005 Tutorial and MultiMedia CD A Step-by-step Project Based Approach Utilizing 3D Solid Modeling David C. Planchard

CREO.1 MODELING A BELT WHEEL

CREO.1 MODELING A BELT WHEEL Figure 1: A belt wheel modeled in this exercise. Learning Targets In this exercise you will learn: Using symmetry when sketching Using pattern to copy features Using RMB when

Explanation of buttons used for sketching in Unigraphics

Explanation of buttons used for sketching in Unigraphics Sketcher Tool Bar Finish Sketch is for exiting the Sketcher Task Environment. Sketch Name is the name of the current active sketch. You can also

SOLIDWORKS 2018 Intermediate Skills

SOLIDWORKS 2018 Intermediate Skills Expanding on Solids, Surfaces, Multibodies, Configurations, Drawings, Sheet Metal and Assemblies Paul Tran CSWE, CSWI SDC PUBLICATIONS Better Textbooks. Lower Prices.

ME Week 2 Project 2 Flange Manifold Part

1 Project 2 - Flange Manifold Part 1.1 Instructions This project focuses on additional sketching methods and sketching commands. Revolve and Work features are also introduced. The part being modeled is

Engineering Design. with SolidWorks A Step-by-Step Project Based Approach Utilizing 3D Solid Modeling

INSIDE: MultiMedia CD An audio/visual presentation of the tutorial projects Engineering Design with SolidWorks 2010 A Step-by-Step Project Based Approach Utilizing 3D Solid Modeling Introductory Level

SDC. SolidWorks Tutorial 2001Plus. A Competency Project Based Approach Utilizing 3D Solid Modeling. David C. Planchard & Marie P.

2001Plus A Competency Project Based Approach Utilizing 3D Solid Modeling David C. Planchard & Marie P. Planchard SDC PUBLICATIONS www.schroff.com www.schroff-europe.com Project 2 Below are the desired

Introducing SolidWorks

Introducing SolidWorks SAAST Robotics 2008 SolidWorks Software Visually-based 3-D Mechanical design software Engineers and Designers use it to: Quickly sketch out ideas Experiment with features, dimensions

Lesson 10: Loft Features

10 Goals of This Lesson Your students will be able to create the following part: profiles chisel This lesson plan corresponds to the Loft Features chapter of SolidWorks Getting Started. SolidWorks Student

SolidWorks Reference Geometry

SolidWorks Reference Geometry IDeATe Laser Micro Part 2 Dave Touretzky and Susan Finger 1. Symmetry and Reference Geometry Today, you ll make this part bear-like face and then cut it on the laser cutter:

Alternatively, the solid section can be made with open line sketch and adding thickness by Thicken Sketch.

Sketcher All feature creation begins with two-dimensional drawing in the sketcher and then adding the third dimension in some way. The sketcher has many menus to help create various types of sketches.

Starting a 3D Modeling Part File

1 How to Create a 3D Model and Corresponding 2D Drawing with Dimensions, GDT (Geometric Dimensioning and Tolerance) Symbols and Title Block in SolidWorks 2013-2014 By Edward Locke This tutorial will introduce

From the above fig. After sketching the path and profile select the sweep command First select the profile from property manager tree And then select

Chapter 5 In sweep command there is a) Two sketch profiles b) Two path c) One sketch profile and one path The sweep profile is used to create threads springs circular things and difficult geometry. For

Module 2: Radial-Line Sheet-Metal 3D Modeling and 2D Pattern Development: Right Cone (Regular, Frustum, and Truncated)

Inventor (5) Module 2: 2-1 Module 2: Radial-Line Sheet-Metal 3D Modeling and 2D Pattern Development: Right Cone (Regular, Frustum, and Truncated) In this tutorial, we will learn how to build a 3D model

Modeling Basic Mechanical Components #1 Tie-Wrap Clip

Modeling Basic Mechanical Components #1 Tie-Wrap Clip This tutorial is about modeling simple and basic mechanical components with 3D Mechanical CAD programs, specifically one called Alibre Xpress, a freely

Feature-Based Modeling and Optional Advanced Modeling. ENGR 1182 SolidWorks 05

Feature-Based Modeling and Optional Advanced Modeling ENGR 1182 SolidWorks 05 Today s Objectives Feature-Based Modeling (comprised of 2 sections as shown below) 1. Breaking it down into features Creating

Product Modelling in Solid Works

Product Modelling in Solid Works In the following exercise you will use solid works to construct the computer mouse shown opposite. In this exercise you will use a number of advanced features to achieve

SolidWorks Training. Introductory course for staff and students from the School of Physics and Astronomy

SolidWorks Training Introductory course for staff and students from the School of Physics and Astronomy i) Introductory presentation SolidWorks Training ii) The SolidWorks GUI The SolidWorks Graphical

Siemens NX11 tutorials. The angled part

Siemens NX11 tutorials The angled part Adaptation to NX 11 from notes from a seminar Drive-to-trial organized by IBM and GDTech. This tutorial will help you design the mechanical presented in the figure

Modeling an Airframe Tutorial

EAA SOLIDWORKS University p 1/11 Difficulty: Intermediate Time: 1 hour As an Intermediate Tutorial, it is assumed that you have completed the Quick Start Tutorial and know how to sketch in 2D and 3D. If

Creo Parametric Primer

PTC Creo Parametric - Primer Student and Academic Editions 02 Helpful hints are enclosed in red brackets or round bubbles like this one! Creo Parametric Primer THIS VERSION OF THE CREO PRIMER HAS BEEN

Part 8: The Front Cover

Part 8: The Front Cover 4 Earpiece cuts and housing Lens cut and housing Microphone cut and housing The front cover is similar to the back cover in that it is a shelled protrusion with screw posts extruding

Foreword. If you have any questions about these tutorials, drop your mail to

Foreword The main objective of these tutorials is to give you a kick start using Solidworks. The approach to write this tutorial is based on what is the most important knowledge you should know and what

Module 1G: Creating a Circle-Based Cylindrical Sheet-metal Lateral Piece with an Overlaying Lateral Edge Seam And Dove-Tail Seams on the Top Edge

Inventor (10) Module 1G: 1G- 1 Module 1G: Creating a Circle-Based Cylindrical Sheet-metal Lateral Piece with an Overlaying Lateral Edge Seam And Dove-Tail Seams on the Top Edge In Module 1A, we have explored

g. Click once on the left vertical line of the rectangle.

This drawing will require you to a model of a truck as a Solidworks Part. Please be sure to read the directions carefully before constructing the truck in Solidworks. Before submitting you will be required

Using Siemens NX 11 Software. The connecting rod

Using Siemens NX 11 Software The connecting rod Based on a Catia tutorial written by Loïc Stefanski. At the end of this manual, you should obtain the following part: 1 Introduction. Start NX 11 and open

Solidworks Tutorial Pencil

The following instructions will be used to help you create a Pencil using Solidworks. These instructions are ordered to make the process as simple as possible. Deviating from the order, or not following

Getting Started. Chapter. Objectives

Chapter 1 Getting Started Autodesk Inventor has a context-sensitive user interface that provides you with the tools relevant to the tasks being performed. A comprehensive online help and tutorial system

Model House Exercise-( Extrude)

-( Extrude) Prerequisite knowledge Focus of the lesson Commands Used This lesson requires an understanding of using the sketch commands including Inserting a new sketch Adding sketch geometry Understanding

Introduction to 3D CAD with SolidWorks. Jianan Li

Introduction to 3D CAD with SolidWorks Jianan Li Create a New Part The first time you launch SolidWorks, it asks you to set the default units and dimension standard. Make sure you have IPS and ANSI selected,

Conquering the Rubicon

Autodesk Inventor R10 Fundamentals: Conquering the Rubicon Elise Moss SDC PUBLICATIONS Schroff Development Corporation www.schroff.com www.schroff-europe.com Schroff Development Corporation P.O. Box 1334

ENGINEERING & COMPUTER GRAPHICS WORKBOOK Using SolidWorks 2005 Ronald E. Barr Thomas J. Krueger Theodore A. Aanstoos Davor Juricic SDC PUBLICATIONS Schroff Development Corporation www.schroff.com www.schroff-europe.com

1. Create a 2D sketch 2. Create geometry in a sketch 3. Use constraints to position geometry 4. Use dimensions to set the size of geometry

2.1: Sketching Many features that you create in Fusion 360 start with a 2D sketch. In order to create intelligent and predictable designs, a good understanding of how to create sketches and how to apply

ENGINEERING & COMPUTER GRAPHICS WORKBOOK Using SolidWorks 2008 Ronald E. Barr Thomas J. Krueger Theodore A. Aanstoos Davor Juricic SDC PUBLICATIONS Schroff Development Corporation www.schroff.com Better

Creo Revolve Tutorial

Creo Revolve Tutorial Setup 1. Open Creo Parametric Note: Refer back to the Creo Extrude Tutorial for references and screen shots of the Creo layout 2. Set Working Directory a. From the Model Tree navigate

NX Lesson 1 Getting Started Pre-reqs/Technical Skills Basic computer use Expectations Read lesson material Implement steps in software while reading through lesson material Complete quiz on Blackboard

Ball Valve Assembly. On completion of the assembly, we will create the exploded view as shown on the right.

Ball Valve Assembly Supplied are the main components of a ball valve. In this exercise you will assemble the valve as shown below Left. (N.B. Socket head cap screws are not supplied these will be created

< Then click on this icon on the vertical tool bar that pops up on the left side.

Pipe Cavity Tutorial Introduction The CADMAX Solid Master Tutorial is a great way to learn about the benefits of feature-based parametric solid modeling with CADMAX. We have assembled several typical parts

Introduction to SolidWorks Introduction to SolidWorks

Introduction to SolidWorks Introduction to SolidWorks SolidWorks is a powerful 3D modeling program. The models it produces can be used in a number of ways to simulate the behaviour of a real part or assembly

for Solidworks TRAINING GUIDE LESSON-9-CAD Mastercam for SolidWorks Training Guide Objectives You will create the geometry for SolidWorks-Lesson-9 using SolidWorks 3D CAD software. You will be working

MECH 130 CAD LAB 5 SPRING 2017 due Friday, April 21, 2016 at 4:30 PM All of LAB 5 s hardcopies will be working drawing layouts. Do not print out from the part file. We will be using the ME130DRAW drawing

SOLIDWORKS 2015 and Engineering Graphics

SOLIDWORKS 2015 and Engineering Graphics An Integrated Approach Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following

Understanding Projection Systems

Understanding Projection Systems A Point: A point has no dimensions, a theoretical location that has neither length, width nor height. A point shows an exact location in space. It is important to understand

Introduction to 3D Printing. Activity 1: Design a keychain using computer-aided design software

Introduction to 3D Printing Activity 1: Design a keychain using computer-aided design software 1 In this activity we ll design a keychain name tag and learn the fundamentals of computer-aided design, the

Module 1H: Creating an Ellipse-Based Cylindrical Sheet-metal Lateral Piece

Inventor (10) Module 1H: 1H- 1 Module 1H: Creating an Ellipse-Based Cylindrical Sheet-metal Lateral Piece In this Module, we will learn how to create an ellipse-based cylindrical sheetmetal lateral piece

LAB 1A: Intro to SolidWorks: 2D -> 3D Brackets

LAB 1A: Intro to SolidWorks: 2D -> 3D Brackets Set units Create Sketch Add relations Linear patterns Mirror Fillet Extrude Extrude cut First, set units. click Option on top of main menu Open Document Properties

Lesson 4 Holes and Rounds

Lesson 4 Holes and Rounds 111 Figure 4.1 Breaker OBJECTIVES Sketch arcs in sections Create a straight hole through a part Complete a Sketched hole Understand the Hole Tool Use Info to extract information

1.6.7 Add Arc Length Dimension Modify Dimension Value Check the Sketch Curve Connectivity

Contents 2D Sketch... 1 1.1 2D Sketch Introduction... 1 1.1.1 2D Sketch... 1 1.1.2 Basic Setting of 2D Sketch... 2 1.1.3 Exit 2D Sketch... 4 1.2 Draw Common Geometry... 5 2.2.1 Points... 5 2.2.2 Lines

Revit Structure 2014 Basics

Revit Structure 2014 Basics Framing and Documentation Elise Moss Authorized Author SDC P U B L I C AT I O N S Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit

DEPARTMENT OF MECHANICAL AND INDUSTRIAL ENGINEERING NORTHEASTERN UNIVERSITY

DEPARTMENT OF MECHANICAL AND INDUSTRIAL ENGINEERING NORTHEASTERN UNIVERSITY CAPSULE PROGRAM Funded by NSF grant #0833636 Tutorial 02 3D Part Modeling SolidWorks 2010 Copyright 2010 Prof. Zeid 3D Part Modeling

and Engineering Graphics

SOLIDWORKS 2018 and Engineering Graphics An Integrated Approach Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following

Working With Drawing Views-I

Chapter 12 Working With Drawing Views-I Learning Objectives After completing this chapter you will be able to: Generate standard three views. Generate Named Views. Generate Relative Views. Generate Predefined

Computer Aided Design Module 2. Lesson Toblerone Bar

Computer Aided Design Module 2 Lesson Toblerone Bar Lesson? Toblerone Bar New Commands used: Polygon, Add Relations, Smart Dimension, Extrude Boss/Base (Mid Plane), Fillet, Line, Extrude-Cut, Linear Pattern

SolidWorks 2013 Part I - Basic Tools

SolidWorks 2013 Part I - Basic Tools Parts, Assemblies and Drawings Paul Tran CSWE, CSWI Supplemental Files SDC PUBLICATIONS Schroff Development Corporation Better Textbooks. Lower Prices. www.sdcpublications.com

Revit Structure 2013 Basics

Revit Structure 2013 Basics Framing and Documentation Elise Moss Supplemental Files SDC P U B L I C AT I O N S Schroff Development Corporation Better Textbooks. Lower Prices. www.sdcpublications.com Tutorial

Engineering Design with SolidWorks A Step-by-Step Project Based Approach Utilizing 3D Solid Modeling. David C. Planchard & Marie P.

Engineering Design with SolidWorks 2003 A Step-by-Step Project Based Approach Utilizing 3D Solid Modeling David C. Planchard & Marie P. Planchard SDC PUBLICATIONS www.schroff.com www.schroff-europe.com

SolidWorks 2014 Part I - Basic Tools

SolidWorks 2014 Part I - Basic Tools Parts, Assemblies and Drawings Paul Tran CSWE, CSWI SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit

LABORATORY MANUAL COMPUTER AIDED DESIGN LAB

LABORATORY MANUAL COMPUTER AIDED DESIGN LAB Sr. No 1 2 3 Experiment Title Setting up of drawing environment by setting drawing limits, drawing units, naming the drawing, naming layers, setting line types

Below are the desired outcomes and usage competencies based on the completion of Project 4.

Engineering Design with SolidWorks Project 4 Below are the desired outcomes and usage competencies based on the completion of Project 4. Project Desired Outcomes: An understanding of the customer s requirements

Lesson 4 Extrusions OBJECTIVES. Extrusions

Lesson 4 Extrusions Figure 4.1 Clamp OBJECTIVES Create a feature using an Extruded protrusion Understand Setup and Environment settings Define and set a Material type Create and use Datum features Sketch

Beginner s Guide to SolidWorks Level I

Beginner s Guide to SolidWorks 2014 - Level I Parts, Assemblies, Drawings, PhotoView 360 and Simulation Xpress Videos Now includes SolidWorks training videos Alejandro Reyes MSME, CSWP, CSWI Multimedia

Solidworks: Lesson 4 Assembly Basics and Toolbox. UCF Engineering

Solidworks: Lesson 4 Assembly Basics and Toolbox UCF Engineering Solidworks We have now completed the basic features of part modeling and it is now time to begin constructing more complex models in the