SOLIDWORKS: Lesson III Patterns & Mirrors. UCF Engineering

Size: px
Start display at page:

Download "SOLIDWORKS: Lesson III Patterns & Mirrors. UCF Engineering"

Transcription

1 SOLIDWORKS: Lesson III Patterns & Mirrors UCF Engineering

2 Solidworks Review Last lesson we discussed several more features that can be added to models in order to increase their complexity. We are now going to discuss several ways that SolidWorks can allow us to create properly designed models both easier and faster.

3 Patterns The first feature that we are going to discuss is patterns. Patterns can be placed in two ways: Linear Patterns, or Circular Patterns. Although both are creating copies of an existing feature, the method that they do this is what distinguishes them.

4 Linear Pattern A linear pattern creates a copy of a feature similar to a grid:

5 Linear pattern To define a linear pattern, you must specify the direction of the patterns, (up to 2 directions), the number of copies in each direction, and the distance between copies.

6 Linear Pattern Lets take a look at how we can pattern a simple feature using the linear patterning command Let s begin by creating a NEW PART! Begin by choosing Extruded Boss/Base TOP PLANE Draw a rectangle on the plane that is 2x1using the origin as a starting point Exit the sketch Draw your sketch by starting on the origin

7 Linear Pattern Since we originally used Extrude let s enter 0.05 for the depth and click the green check.

8 Linear Pattern Let s do an EXTRUDED CUT on the top surface of our part. Click Extruded cut, then choose the TOP surface. Change view to NORMAL TO. Choose CIRCLE

9 Linear Pattern Choose SMART DIMENSION, then click on the origin of the circle then the origin of the sketch in the bottom left. Drag the dimension so that it becomes a VERTICAL dimension and enter Do the same for the HORIZONTAL. Then dimension the diameter by simply clicking on the circumference. Enter 0.20.

10 Linear Pattern Exit the sketch to see the hole as a CUT. In property manager choose under DIRECTION choose THROUGH ALL. Click the green check to see our hole.

11 Linear Pattern Select the CUT by either selecting the Cut-Extrude choice in FEATURE MANAGER or simply click on the cut in the design and it should highlight. Choose LINEAR PATTERN from the dynamic toolbar.

12 Linear Pattern You will notice that the extruded cut we made shows up in property manager as a feature we want to pattern. Then above in the DIRECTION we notice it is blank, so highlight this area, then select the bottom horizontal edge to the top face of our rectangle.

13 Linear Pattern In property manager, enter 0.5 for the distance and 4 for the # of instances you want if it isn t already chosen for you.

14 Linear Pattern For Direction 2, highlight the area and choose the left edge of the rectangle. Enter 0.4 for the distance and 2 for the # of instances. Click OK in property manager to see the final pattern

15 Linear Pattern Suppose you discover you made a mistake in the diameter of the circle. Double Click on the original feature then change the dimension of the diameter. Double click on the dimension to change it to Click OK, then OK in property manager. Be sure to click the stoplight to re-build the part.

16 Circular Pattern The circular pattern is very similar to the linear, however, instead of patterning along two dimensions, it patterns about an axis.

17 Circular Pattern For a circular pattern, you must define the axis of revolution, the total revolution angle, and the number of copies to make.

18 Circular Pattern Lets take a look at how we can pattern a simple feature using the circular patterning command Let s begin by: Create a New Part Choose Extruded Boss/Base Choose Top Plane to sketch on Make a Circle with the origin of the sketch as the origin of the circle Dimension the circle so that the diameter is 1 Exit the sketch Extrude the circle to 0.05

19 Circular Pattern Let s now make an extruded cut on the top face of the circle. Choose Extruded Cut, select the top plane and change view to normal to. Draw a circle vertically above the origin. You will see a vertical line to assist you in centering the line properly. Dimension the circle so that it is 0.25 away from the origin of our cylindrical base with a diameter of 0.2.

20 Circular Pattern Now you may notice that our small circular sketch is under defined. Even though we placed it vertically above the origin we really haven t defined it as such. Click on the origin of the small circle, hold down CTRL, then select the origin of our base. Add a vertical relation to these points in property manager.

21 Circular Pattern Exit the sketch, change your view to isometric, then choose through all in the direction section of property manager to finish the cut.

22 Circular Pattern To make a circular pattern we need an axis of revolution. We know it is the center of our base but we can t see the axis. To see this axis, choose VIEW at the top then choose temporary axis You probably won t see the axis unless you ZOOM in to look at the origin.

23 Circular Pattern Click on the feature you want to pattern either by clicking on the feature in feature manager or clicking on the feature in the design. Click on circular pattern ( you may need to expand your button by clicking on the small arrow on the right of the toolbar).

24 Circular Pattern You should see that in property manager that the axis space is highlighted. Choose the axis at the center of your design as you want the pattern to revolve around that axis. You can now make your pattern TWO different ways. If equal spacing is checked simply specify the number of patterns you want. Or you can uncheck equal spacing and specify the number of patterns as well as the angle between them. Click Equal Spacing and make 5 copies! Click OK to exit property manager

25 Circular Pattern If you need to change anything, you can simply click on the feature, click on the dimension you want to change such as the radius of the cut or its dimension from the axis. Then click the stoplight button to re-build the part.

26 Mirrors Mirroring is another way that SolidWorks can create a copy of a feature. When mirroring, you must choose a feature to mirror, and a plane to mirror about.

27 Mirrors Oftentimes the plane that you wish to mirror about is not one of the standard planes (front, top, or right). To create a new plane, you must use the Features > Reference Geometry > Plane command to define a new reference plane.

28 Mirrors Lets take a look at how we can copy a simple feature using the mirror command Make a new part. Choose: Extruded Boss/Base Choose Top Plane Make a rectangle with the ORIGIN at the middle. To ensure that the origin is at the center of our rectangle we must make sure that the origin lies on a line that lines up with the MIDPOINT of each edge of our rectangle. RIGHT CLICK on the top horizontal line of our rectangle and CHOOSE MIDPOINT

29 Mirrors Click on the MIDPOINT, hold CTRL, and select the origin. In property add the relation, VERTICAL.

30 Mirrors Right click on a vertical edge to select the MIDPOINT. Hold CTRL, select the origin, then add the relation HORIZONTAL in property manager.

31 Mirrors Exit the sketch, change view to isometric and extrude to some distance. Click on extruded boss/base Click on extruded boss/base and choose the top surface of your rectangular cube and change the view to normal to. Draw a simple triangle using line, on the surface

32 Mirrors Exit the sketch and switch your view to isometric. Extrude the triangle to a depth of 0.02, then click ok to see the extruded triangular feature.

33 Mirror So if we want to mirror this triangle, we simply click on the feature in feature manager or the part in our design. From the dynamic toolbar choose MIRROR

34 Mirror In property manager, we see it is asking for a mirror face or plane. In our design field, we see our part which we can expand to view various things. Expand and select right plane as this is the plane we want to mirror about. Notice that this plane is right on our origin.

35 Mirror You should see a preview of the mirror. Click OK in property manager to finish the mirror.

36 Patterns and Mirrors This is all well and good, but couldn t we simply have drawn all of these patterned or mirrored features ourselves? Yes, we could have, but there are several major advantages to creating the copies in the proper fashion.

37 Patterns and Mirrors First, and probably the most obvious, is that it saves time; drawing all of those copied features can be quite time consuming and there is no reason to do it if we don t have to. Second, and most importantly, is that if you change the original feature in a pattern or mirror, all of the children also change.

38 Patterns and Mirrors Performing patterns and mirrors properly is an important part of maintaining design intent If the features in your part are intended to be If the features in your part are intended to be the same, then it is important that your modeling practice reflects that.

39 Solidworks Exercise Lets use what we have learned to model the following part:

40 Solidworks Exercise It is always useful to think about HOW you might design this part. Upon inspection we see that this is basically 3 rectangles. One front plate with 2 side plates. You might notice that the side plates are symmetrical about the center plate. So we can use mirror to build one side. We can use pattern, to place the smaller holes on the front plate.

41 Solidworks Exercise Right click on the part in feature manager and choose DOCUMENT PROPERTIES. Lets click UNITS and change the units to IPS to dimension the part in INCHES.

42 Solidworks Exercise Let s begin by selecting a NEW PART, then extruded boss base. Choose the FRONT PLANE. Change view to normal to if not already seen.

43 Solidworks Exercise Begin by drawing a rectangle about the origin. Add relations to the rectangle edges of vertical and horizontal using midpoints and the origin. See slides to remember how to do this.

44 Solidworks Exercise Dimension the rectangle according to our original design sketch. We see the bottom edge is 5 inches and a side is 4 inches. Exit the sketch, and extrude the part according to the design, which is 0.3.

45 Solidworks Exercise Now lets add the circle in the middle. Choose Extruded CUT, choose top face, change view to normal to. Place a circle using the origin to begin and dimension the circle with a diameter of 2.40 in.

46 Solidworks Exercise Exit the sketch, then change to isometric view to see the 3D design. Choose through all in property manager to extrude the cut.

47 Solidworks Exercise Now lets pattern the outer circles. Choose Extruded CUT, the top face, change view to normal view. Place a circle in the bottom right corner and dimension with a radius of 0.4 in.

48 Solidworks Exercise We need this circle to be at an angle of 45 degrees to the vertical. One way to do this is to use a centerline. Choose Centerline and draw a line from the origin to the center of our small circle. Draw a second center line from the origin straight down. Make sure you see 90 degrees as well as a vertical line icon.

49 Solidworks Exercise Lets dimension the centerline from the origin to our circle as 1.90 or you can enter 3.80/2. Then you can dimension the ANGLE. Click on your first centerline, then click the second centerline and the angle will appear. Change this to 45 degrees.

50 Solidworks Exercise Exit the sketch, switch view to isometric and extrude the cut using through all. Click OK in property manager to see the result.

51 Solidworks Exercise Enable your temporary axis (Choose view at top). Then select the feature you want to pattern, which was our small circle. Click CIRCULAR PATTERN. In property manager, the axis field is highlighted so choose the temporary axis you made at the origin Make 4 instances for 4 holes, then click OK.

52 Solidworks Exercise Now we have 4 equally spaced holes.

53 Solidworks Exercise Now lets make our side which we will mirror. Choose Extruded Boss Base and choose the right side face. One thing that may be useful is using the GRID. To see the grid, right click out in the design field and choose it. It helps you visualize WHERE you are sketching.

54 Solidworks Exercise Turn off the grid and change your view to normal to. Using the line tool, sketch the basic shape. Hit escape to get out of the line tool.

55 Solidworks Exercise Now lets dimension the shape according to our original design. We also need 3 circles. So add 3 circle in the general area.

56 Solidworks Exercise To dimension the circle we can select ALL by holding down CTRL. Then add the relation EQUAL. The diameter of the circles are Finish the dimensioning then exit the sketch and switch to isometric view.

57 Solidworks Exercise Click on the button for BLIND to reverse the direction of the EXTRUDE. We want to extrude inward!!! You should see the arrow switch to inward. Extrude the selection to 0.3 also so that the thickness is the same as the front piece. Click OK in property manager.

58 Solidworks Exercise You should now see your finished side panel. Now click on the new extruded side in feature manager. Next choose MIRROR. Expand the part in the DESIGN FIELD, chose right plane.

59 Solidworks Exercise The last thing we need to do is FILLET the front edges. Hold down CTRL and select the OUTER and INNER edges. Select 0.5 inches Select 0.5 inches for the radius. Then Click OK.

60 Solidworks Exercise

SOLIDWORKS: Lesson 1 - Basics and Modeling. UCF Engineering

SOLIDWORKS: Lesson 1 - Basics and Modeling. UCF Engineering SOLIDWORKS: Lesson 1 - Basics and Modeling Fundamentals UCF Engineering SolidWorks SolidWorks is a 3D solid modeling package which allows users to develop full solid models in a simulated environment for

More information

Battery Holder. Chapter 9. Boat. A. Front Extrude. Step 1. Click File Menu > New, click Part and OK. SolidWorks 10 BATTERY HOLDER AA BOAT Page 9-1

Battery Holder. Chapter 9. Boat. A. Front Extrude. Step 1. Click File Menu > New, click Part and OK. SolidWorks 10 BATTERY HOLDER AA BOAT Page 9-1 Chapter 9 Boat Battery Holder A. Front Extrude. Step 1. Click File Menu > New, click Part and OK. AA Step 2. Click Front (plane) in the Feature Manager and click Sketch from the Content toolbar, Fig. 1.

More information

Delta Dart. Socket. (L) on the Sketch toolbar. Fig. 1. (S) on the Sketch toolbar. on the Sketch toolbar. on the Standard Views toolbar.

Delta Dart. Socket. (L) on the Sketch toolbar. Fig. 1. (S) on the Sketch toolbar. on the Sketch toolbar. on the Standard Views toolbar. Chapter 6 Delta Dart Socket A. Sketch. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Front Plane in the Feature Manager and click Sketch from the Content toolbar, Fig. 1. Step

More information

Body. Chapter 2. CO2 Rail Car E. A. Save as "BODY RAIL E". Step 1. Open your BLANK file.

Body. Chapter 2. CO2 Rail Car E. A. Save as BODY RAIL E. Step 1. Open your BLANK file. Chapter 2 A. Save as "BODY RAIL E". Step 1. Open your BLANK file. Step 2. Click File Menu > Save As. Step 3. Key-in BODY RAIL E for the filename and press ENTER. CO2 Rail Car E Body B. Appearance. Step

More information

CO2 Shell Car. Axle Retainer. in the Feature Manager and click Sketch from the Content toolbar, Fig. 1. (L) on the Sketch toolbar. Fig.

CO2 Shell Car. Axle Retainer. in the Feature Manager and click Sketch from the Content toolbar, Fig. 1. (L) on the Sketch toolbar. Fig. Chapter 17 CO2 Shell Car Axle Retainer A. Sketch. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Top Plane in the Feature Manager and click Sketch from the Content toolbar, Fig.

More information

Skateboard. Hanger. in the Feature Manager and click Sketch on the Context toolbar, Fig. 1. Fig. 2

Skateboard. Hanger. in the Feature Manager and click Sketch on the Context toolbar, Fig. 1. Fig. 2 Chapter 3 Skateboard Hanger A. Sketch1 Lines. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Right Plane in the Feature Manager and click Sketch on the Context toolbar, Fig. 1.

More information

SOLIDWORKS 2016 and Engineering Graphics

SOLIDWORKS 2016 and Engineering Graphics SOLIDWORKS 2016 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

More information

SOLIDWORKS: Lesson 1 - Basics and Modeling. Introduction to Robotics

SOLIDWORKS: Lesson 1 - Basics and Modeling. Introduction to Robotics SOLIDWORKS: Lesson 1 - Basics and Modeling Fundamentals Introduction to Robotics SolidWorks SolidWorks is a 3D solid modeling package which allows users to develop full solid models in a simulated environment

More information

Nose Cone. Chapter 4. Rocket 3D Print. A. Revolve. Step 1. Click File Menu > New, click Part and OK. SOLIDWORKS 16 Nose Cone ROCKET 3D PRINT Page 4-1

Nose Cone. Chapter 4. Rocket 3D Print. A. Revolve. Step 1. Click File Menu > New, click Part and OK. SOLIDWORKS 16 Nose Cone ROCKET 3D PRINT Page 4-1 Chapter 4 Rocket 3D Print Nose Cone A. Revolve. Step 1. Click File Menu > New, click Part and OK. Step 2. Click Front Plane in the Feature Manager and click Sketch on the content toolbar, Fig. 1. Step

More information

Autodesk Fusion 360: Model. Overview. Modeling techniques in Fusion 360

Autodesk Fusion 360: Model. Overview. Modeling techniques in Fusion 360 Overview Modeling techniques in Fusion 360 Modeling in Fusion 360 is quite a different experience from how you would model in conventional history-based CAD software. Some users have expressed that it

More information

Glider. Wing. Top face click Sketch. on the Standard Views. (S) on the Sketch toolbar.

Glider. Wing. Top face click Sketch. on the Standard Views. (S) on the Sketch toolbar. Chapter 5 Glider Wing 4 Panel Tip A. Open and Save As "WING 4 PANEL". Step 1. Open your WING BLANK file. Step 2. Click File Menu > Save As. Step 3. Key-in WING 4 PANEL for the filename and press ENTER.

More information

SolidWorks 2013 and Engineering Graphics

SolidWorks 2013 and Engineering Graphics SolidWorks 2013 and Engineering Graphics An Integrated Approach Randy H. Shih SDC PUBLICATIONS Schroff Development Corporation Better Textbooks. Lower Prices. www.sdcpublications.com Visit the following

More information

Memo Block. This lesson includes the commands Sketch, Extruded Boss/Base, Extruded Cut, Shell, Polygon and Fillet.

Memo Block. This lesson includes the commands Sketch, Extruded Boss/Base, Extruded Cut, Shell, Polygon and Fillet. Commands Used New Part This lesson includes the commands Sketch, Extruded Boss/Base, Extruded Cut, Shell, Polygon and Fillet. Click File, New on the standard toolbar. Select Part from the New SolidWorks

More information

ME009 Engineering Graphics and Design CAD 1. 1 Create a new part. Click. New Bar. 2 Click the Tutorial tab. 3 Select the Part icon. 4 Click OK.

ME009 Engineering Graphics and Design CAD 1. 1 Create a new part. Click. New Bar. 2 Click the Tutorial tab. 3 Select the Part icon. 4 Click OK. PART A Reference: SolidWorks CAD Student Guide 2014 2 Lesson 2: Basic Functionality Active Learning Exercises Creating a Basic Part Use SolidWorks to create the box shown at the right. The step-by-step

More information

Body. Chapter 1. Simple Machines. A. New Part. Step 1. Click File Menu > New.

Body. Chapter 1. Simple Machines. A. New Part. Step 1. Click File Menu > New. Chapter 1 A. New Part. Step 1. Click File Menu > New. Simple Machines Body Step 2. Click Part from the list and click OK, Fig. 1. B. Sketch Construction Rectangle. Step 1. Click Right Plane in the Feature

More information

Chapter 4 Feature Design Tree

Chapter 4 Feature Design Tree 4-1 Chapter 4 Feature Design Tree Understand Feature Interactions Use the FeatureManager Design Tree Modify and Update Feature Dimensions Perform History-Based Part Modifications Change the Names of Created

More information

Skateboard. Hanger. in the Feature Manager and click Sketch. (S) on the Sketch. Line

Skateboard. Hanger. in the Feature Manager and click Sketch. (S) on the Sketch. Line Chapter 3 Skateboard Hanger A. Sketch 1. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Right Plane from the Content toolbar, Fig. 1. in the Feature Manager and click Sketch Step

More information

SolidWorks Intro Part 1b

SolidWorks Intro Part 1b SolidWorks Intro Part 1b Dave Touretzky and Susan Finger 1. Create a new part We ll create a CAD model of the 2 ½ D key fob below to make on the laser cutter. Select File New Templates IPSpart If the SolidWorks

More information

Delta Dart. Propeller. in the Feature Manager and click Sketch from the Content toolbar, Fig. 1. on the Sketch toolbar.

Delta Dart. Propeller. in the Feature Manager and click Sketch from the Content toolbar, Fig. 1. on the Sketch toolbar. Chapter 8 Delta Dart Propeller A. Base for Blade. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Top Plane in the Feature Manager and click Sketch from the Content toolbar, Fig.

More information

Wheel GT-F. Chapter 5. CO2 Shell Car. A. Sketch. Step 1. Click File Menu > New, click Part Metric and OK.

Wheel GT-F. Chapter 5. CO2 Shell Car. A. Sketch. Step 1. Click File Menu > New, click Part Metric and OK. Chapter 5 CO2 Shell Car Wheel GT-F A. Sketch. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Front Plane in the Feature Manager and click Sketch on the context toolbar, Fig. 1.

More information

JSS. Ping Pong Ball. in the Feature Manager and click Sketch on the Context toolbar, Fig. 1. on the Sketch toolbar.

JSS. Ping Pong Ball. in the Feature Manager and click Sketch on the Context toolbar, Fig. 1. on the Sketch toolbar. Chapter 18 JSS Ping Pong Ball A. Half Circle Sketch. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Front Plane in the Feature Manager and click Sketch on the Context toolbar, Fig.

More information

CO2 Rail Car. Wheel Rear Px. on the Command Manager toolbar.

CO2 Rail Car. Wheel Rear Px. on the Command Manager toolbar. Chapter 6 CO2 Rail Car Wheel Rear Px A. Sketch Construction Lines. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Front (plane) in the Feature Manager (left panel), Fig. 1. Step

More information

Propeller. Chapter 13. Airplane. A. Base for Blade. Step 1. Click File Menu > New, click Part and OK.

Propeller. Chapter 13. Airplane. A. Base for Blade. Step 1. Click File Menu > New, click Part and OK. Chapter 13 Airplane Propeller A. Base for Blade. Step 1. Click File Menu > New, click Part and OK. Step 2. Click Top Plane in the Feature Manager and click Sketch toolbar, Fig. 1. from the Content Step

More information

Speedway. Body. (S) on the Sketch toolbar. Fig. 1

Speedway. Body. (S) on the Sketch toolbar. Fig. 1 Chapter 1 A. New Part. Step 1. Click File Menu > New. Speedway Body Step 2. Click Part from the list and click OK, Fig. 1. B. Sketch Construction Rectangle. Step 1. Click Right Plane in the Feature Manager

More information

H Stab and V Stab. Chapter 6. Glider. A. Open and Save as "H STAB". Step 1. Open your STABILIZER BLANK file.

H Stab and V Stab. Chapter 6. Glider. A. Open and Save as H STAB. Step 1. Open your STABILIZER BLANK file. Chapter 6 Glider H Stab and V Stab A. Open and Save as "H STAB". Step 1. Open your STABILIZER BLANK file. Step 2. Click File Menu > Save As. Step 3. Key-in H STAB for the filename and press ENTER. B. Sketch

More information

Autodesk Inventor - Basics Tutorial Exercise 1

Autodesk Inventor - Basics Tutorial Exercise 1 Autodesk Inventor - Basics Tutorial Exercise 1 Launch Inventor Professional 2015 1. Start a New part. Depending on how Inventor was installed, using this icon may get you an Inch or Metric file. To be

More information

Introduction to SolidWorks for Technology. No1: Childs Toy

Introduction to SolidWorks for Technology. No1: Childs Toy Introduction to SolidWorks for Technology No1: Childs Toy Table of Contents Table of Contents... 1 Introduction... 2 Part Modelling: Cab... 3 Part Modelling: Base... 6 Part Modelling: Wheel... 12 Assembly:

More information

SolidWorks 2½D Parts

SolidWorks 2½D Parts SolidWorks 2½D Parts IDeATe Laser Micro Part 1b Dave Touretzky and Susan Finger 1. Create a new part In this lab, you ll create a CAD model of the 2 ½ D key fob below to make on the laser cutter. Select

More information

CO 2 Shell Car. Body. in the Feature Manager and click Sketch from the context toolbar, Fig. 1. on the Standard Views toolbar.

CO 2 Shell Car. Body. in the Feature Manager and click Sketch from the context toolbar, Fig. 1. on the Standard Views toolbar. CO 2 Shell Car Chapter 2 Body A. Save as "BODY". Step 1. If necessary, open your BLANK file. Step 2. Click File Menu > Save As. Step 3. Key-in BODY for the filename and press ENTER. B. FRONT Wheel Shell.

More information

Battery Holder 2 x AA

Battery Holder 2 x AA Chapter 22 JSS Battery Holder 2 x AA A. Front Extrude. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Front Plane in the Feature Manager and click Sketch from the Context toolbar,

More information

Introduction to SolidWorks Basics Materials Tech. Wood

Introduction to SolidWorks Basics Materials Tech. Wood Introduction to SolidWorks Basics Materials Tech. Wood Table of Contents Table of Contents... 1 Book End... 2 Introduction... 2 Learning Intentions... 2 Modelling the Base... 3 Modelling the Front... 10

More information

Autodesk Inventor 2019 and Engineering Graphics

Autodesk Inventor 2019 and Engineering Graphics Autodesk Inventor 2019 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

More information

F-1 Car. Blank. in the Feature Manager and click Sketch from the Content toolbar, Fig. 3. Origin. on the Features toolbar.

F-1 Car. Blank. in the Feature Manager and click Sketch from the Content toolbar, Fig. 3. Origin. on the Features toolbar. Chapter 1 A. New Metric Part. Step 1. Click File Menu > New. F-1 Car Blank Step 2. Click Part Metric from the list of templates and click OK, Fig. 1. If you are not using SOLIDWORKS templates (you should

More information

F1 Car. Wheel. in the Feature Manager and click Sketch on the Context toolbar, Fig. 1. (S) on the

F1 Car. Wheel. in the Feature Manager and click Sketch on the Context toolbar, Fig. 1. (S) on the Chapter 3 F1 Car Wheel A. Sketch Lines. Step 1. Click File Menu > New, click Part Metric and OK. Step 2. Click Front Plane in the Feature Manager and click Sketch on the Context toolbar, Fig. 1. Step 3.

More information

Solar Car. Chassis. in the Feature Manager and click Sketch from the Content toolbar, Fig. 2. Origin. on the Command Manager toolbar. Fig.

Solar Car. Chassis. in the Feature Manager and click Sketch from the Content toolbar, Fig. 2. Origin. on the Command Manager toolbar. Fig. Chapter 1 A. New Part. Step 1. Click File Menu > New. Solar Car Chassis Step 2. Click Part from the list and click OK, Fig. 1. B. Sketch Chassis. Step 1. Click Right Plane in the Feature Manager and click

More information

Boat. Battery Holder AA

Boat. Battery Holder AA Chapter 9 Boat Battery Holder AA A. Front Extrude. Step 1. Click File Menu > New, click Part and OK. Step 2. Click Front Plane in the Feature Manager and click Sketch context toolbar, Fig. 1. Step 3. Click

More information

Fuselage and Sharks Tooth

Fuselage and Sharks Tooth Chapter 4 Glider Fuselage and Sharks Tooth A. Save as "FUSELAGE". Step 1. Open your FUSELAGE BLANK file. Step 2. Click File Menu > Save As. Step 3. Key-in FUSELAGE for the filename and press ENTER. B.

More information

Doctor Walt s Solid Edge Version 19 Workbook 137

Doctor Walt s Solid Edge Version 19 Workbook 137 Still using the SMART DIMENSION Tool, click on the left vertical edge of the sketch. Move the cursor to the left and click to set the text position. Type 1.5 for the value and hit the ENTER Key. Next,

More information

Chair. Top Rail. on the Standard Views toolbar. (Ctrl-7) on the Weldments toolbar. at bottom left corner of display to deter- mine sketch plane.

Chair. Top Rail. on the Standard Views toolbar. (Ctrl-7) on the Weldments toolbar. at bottom left corner of display to deter- mine sketch plane. Chapter 7 A. 3D Sketch. Step 1. If necessary, open your CHAIR file. Chair Top Rail Step 2. Click Isometric on the Standard Views toolbar. (Ctrl-7) Step 3. Zoom in around top of back leg, Fig. 1. To zoom,

More information

Blank. Chapter 1. CO2 Rail Car. A. New Metric Part. Step 1. Click File Menu > New. B. Body. Step 1. Click Right Plane

Blank. Chapter 1. CO2 Rail Car. A. New Metric Part. Step 1. Click File Menu > New. B. Body. Step 1. Click Right Plane Chapter 1 A. New Metric Part. Step 1. Click File Menu > New. CO2 Rail Car Blank Step 2. Click Part Metric from the list and click OK, Fig. 1. If you are not using SolidWorks templates (you should be),

More information

3D Design with 123D Design

3D Design with 123D Design 3D Design with 123D Design Introduction: 3D Design involves thinking and creating in 3 dimensions. x, y and z axis Working with 123D Design 123D Design is a 3D design software package from Autodesk. A

More information

Inventor 201. Work Planes, Features & Constraints: Advanced part features and constraints

Inventor 201. Work Planes, Features & Constraints: Advanced part features and constraints Work Planes, Features & Constraints: 1. Select the Work Plane feature tool, move the cursor to the rim of the base so that inside and outside edges are highlighted and click once on the bottom rim of the

More information

Simple Machines. Body. Step 4. Start at Origin and sketch the 8 lines, Fig. 2. Fig. 1. Origin

Simple Machines. Body. Step 4. Start at Origin and sketch the 8 lines, Fig. 2. Fig. 1. Origin Chapter 1 Simple Machines Body A. Sketch. Step 1. Click File Menu > New, click Part and OK. Step 2. Click Right Plane in the Feature Manager and click Sketch on the context toolbar, Fig. 1. Step 3. Click

More information

Simple Machines. Wheel. in the Feature Manager and click Sketch. on the Command Manager toolbar.

Simple Machines. Wheel. in the Feature Manager and click Sketch. on the Command Manager toolbar. Chapter 3 Simple Machines Wheel A. Wheel. Step 1. Click File Menu > New, click Part and OK. Step 2. Click Right Plane from the Content toolbar, Fig. 1. in the Feature Manager and click Sketch Step 3. Click

More information

Exercise Guide. Published: August MecSoft Corpotation

Exercise Guide. Published: August MecSoft Corpotation VisualCAD Exercise Guide Published: August 2018 MecSoft Corpotation Copyright 1998-2018 VisualCAD 2018 Exercise Guide by Mecsoft Corporation User Notes: Contents 2 Table of Contents About this Guide 4

More information

Modeling a Gear Standard Tools, Surface Tools Solid Tool View, Trackball, Show-Hide Snaps Window 1-1

Modeling a Gear Standard Tools, Surface Tools Solid Tool View, Trackball, Show-Hide Snaps Window 1-1 Modeling a Gear This tutorial describes how to create a toothed gear. It combines using wireframe, solid, and surface modeling together to create a part. The model was created in standard units. To begin,

More information

Chapter 2 Parametric Modeling Fundamentals

Chapter 2 Parametric Modeling Fundamentals 2-1 Chapter 2 Parametric Modeling Fundamentals Create Simple Extruded Solid Models Understand the Basic Parametric Modeling Procedure Create 2-D Sketches Understand the Shape before Size Approach Use the

More information

TUTORIAL 2. OBJECTIVE: Use SolidWorks/COSMOS to model and analyze a cattle gate bracket that is subjected to a force of 100,000 lbs.

TUTORIAL 2. OBJECTIVE: Use SolidWorks/COSMOS to model and analyze a cattle gate bracket that is subjected to a force of 100,000 lbs. TUTORIAL 2 OBJECTIVE: Use SolidWorks/COSMOS to model and analyze a cattle gate bracket that is subjected to a force of 100,000 lbs. GETTING STARTED: 1. Open the SolidWorks program. 2. Open a new part file.

More information

Solidworks Tutorial #1: How to create USB head

Solidworks Tutorial #1: How to create USB head This Solidworks tutorial composes using the exact format and delivery as Solidworks 2008/2009 Tutorials : Beginner e-book. Solidworks Tutorial #1: How to create USB head You can find almost all PC devices

More information

Tail Hook. Chapter 14. Airplane. A. Construction Rectangle. Step 1. Click File Menu > New, click Part and OK.

Tail Hook. Chapter 14. Airplane. A. Construction Rectangle. Step 1. Click File Menu > New, click Part and OK. Chapter 14 Airplane Tail Hook A. Construction Rectangle. Step 1. Click File Menu > New, click Part and OK. Step 2. Click Right (plane) in the Feature Manager and click Sketch from the Content toolbar,

More information

On the ribbon bar, click the Select from Sketch button.

On the ribbon bar, click the Select from Sketch button. On the Features toolbar, click the Revolved Protrusion command. On the ribbon bar, click the Select from Sketch button. In the part window, select the Sketch, and on the ribbon bar click the Accept button.

More information

Module 1: Basics of Solids Modeling with SolidWorks

Module 1: Basics of Solids Modeling with SolidWorks Module 1: Basics of Solids Modeling with SolidWorks Introduction SolidWorks is the state of the art in computer-aided design (CAD). SolidWorks represents an object in a virtual environment just as it exists

More information

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

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

More information

Technique or Feature Where Introduced

Technique or Feature Where Introduced Part 6: Keypad 4 Mirrored features Patterned features First extrusion Rounded corners In the earpiece part, you defined a radial pattern, one that created new instances of a feature at intervals around

More information

SOLIDWORKS 2018 Reference Guide

SOLIDWORKS 2018 Reference Guide SOLIDWORKS 2018 Reference Guide A comprehensive reference guide with over 250 standalone tutorials David C. Planchard, CSWP, SOLIDWORKS Accredited Educator SDC PUBLICATIONS Better Textbooks. Lower Prices.

More information

Structural & Thermal Analysis Using the ANSYS Workbench Release 12.1 Environment

Structural & Thermal Analysis Using the ANSYS Workbench Release 12.1 Environment ANSYS Workbench Tutorial Structural & Thermal Analysis Using the ANSYS Workbench Release 12.1 Environment Kent L. Lawrence Mechanical and Aerospace Engineering University of Texas at Arlington SDC PUBLICATIONS

More information

Lesson 1: Creating T- Spline Forms. In Samples section of your Data Panel, browse to: Fusion 101 Training > 03 Sculpt > 03_Sculpting_Introduction.

Lesson 1: Creating T- Spline Forms. In Samples section of your Data Panel, browse to: Fusion 101 Training > 03 Sculpt > 03_Sculpting_Introduction. 3.1: Sculpting Sculpting in Fusion 360 allows for the intuitive freeform creation of organic solid bodies and surfaces by leveraging the T- Splines technology. In the Sculpt Workspace, you can rapidly

More information

3 AXIS STANDARD CAD. BobCAD-CAM Version 28 Training Workbook 3 Axis Standard CAD

3 AXIS STANDARD CAD. BobCAD-CAM Version 28 Training Workbook 3 Axis Standard CAD 3 AXIS STANDARD CAD This tutorial explains how to create the CAD model for the Mill 3 Axis Standard demonstration file. The design process includes using the Shape Library and other wireframe functions

More information

Glider. Clay. Fig. 1 Side face. Step 5. In the Convert Entities Property Manager: click side face, Fig. 3 click OK twice, Fig. 3. Fig. 3.

Glider. Clay. Fig. 1 Side face. Step 5. In the Convert Entities Property Manager: click side face, Fig. 3 click OK twice, Fig. 3. Fig. 3. Chapter 9 A. Open Assembly File. Step 1. Open your GLIDER ASSEMBLY file. Glider Clay B. New Component Part. Step 1. Click Insert Menu > Component > New Part. Step 2. Click the side face of the Fuselage,

More information

Autodesk Inventor Design Exercise 2: F1 Team Challenge Car Developed by Tim Varner Synergis Technologies

Autodesk Inventor Design Exercise 2: F1 Team Challenge Car Developed by Tim Varner Synergis Technologies Autodesk Inventor Design Exercise 2: F1 Team Challenge Car Developed by Tim Varner Synergis Technologies Tim Varner - 2004 The Inventor User Interface Command Panel Lists the commands that are currently

More information

Autodesk Inventor 2016

Autodesk Inventor 2016 Parametric Modeling with Autodesk Inventor 2016 Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following websites to learn

More information

ME 120: Impeller Model in Solidworks 1/6

ME 120: Impeller Model in Solidworks 1/6 ME 120: Impeller Model in Solidworks 1/6 Steps to Draw Pump Impeller: The steps below show one way to draw the impeller. You should make sure that your impeller is not larger than the one shown or it may

More information

Rocket 1. Fin. in the Feature Manager and click Sketch from the Content toolbar, Fig. 1. (L) on the Sketch toolbar. Fig. 1. Fig. 2

Rocket 1. Fin. in the Feature Manager and click Sketch from the Content toolbar, Fig. 1. (L) on the Sketch toolbar. Fig. 1. Fig. 2 Chapter 2 Rocket 1 Fin A. Sketch. Step 1. Click File Menu > New, click Part and OK. Step 2. Click Right Plane in the Feature Manager and click Sketch from the Content toolbar, Fig. 1. Step 3. Click Line

More information

CATIA V5 Parametric Surface Modeling

CATIA V5 Parametric Surface Modeling CATIA V5 Parametric Surface Modeling Version 5 Release 16 A- 1 Toolbars in A B A. Wireframe: Create 3D curves / lines/ points/ plane B. Surfaces: Create surfaces C. Operations: Join surfaces, Split & Trim

More information

Parametric Modeling. With. Autodesk Inventor. Randy H. Shih. Oregon Institute of Technology SDC PUBLICATIONS

Parametric Modeling. With. Autodesk Inventor. Randy H. Shih. Oregon Institute of Technology SDC PUBLICATIONS Parametric Modeling With Autodesk Inventor R10 Randy H. Shih Oregon Institute of Technology SDC PUBLICATIONS Schroff Development Corporation www.schroff.com www.schroff-europe.com 2-1 Chapter 2 Parametric

More information

SOLIDWORKS 2016: A Power Guide for Beginners and Intermediate Users

SOLIDWORKS 2016: A Power Guide for Beginners and Intermediate Users SOLIDWORKS 2016: A Power Guide for Beginners and Intermediate Users The premium provider of learning products and solutions www.cadartifex.com Table of Contents Dedication... 3 Preface... 15 Part 1. Introducing

More information

Extrusion Revolve. ENGR 1182 SolidWorks 02

Extrusion Revolve. ENGR 1182 SolidWorks 02 Extrusion Revolve ENGR 1182 SolidWorks 02 Today s Objectives Creating 3D Shapes from 2D sketches using: Extrusion Revolve SW02 In-Class Activity Extrude a Camera Revolve a Wheel SW02 Out-of-Class Homework

More information

Clay. Chapter 9. Glider. A. Open Assembly File. Step 1. Open your GLIDER ASSEMBLY file.

Clay. Chapter 9. Glider. A. Open Assembly File. Step 1. Open your GLIDER ASSEMBLY file. Chapter 9 A. Open Assembly File. Step 1. Open your GLIDER ASSEMBLY file. Glider Clay B. New Component Part. Step 1. Click Insert Menu > Component > New Part. C. Sketch. Step 1. Click the side face of the

More information

Lesson 1 Parametric Modeling Fundamentals

Lesson 1 Parametric Modeling Fundamentals 1-1 Lesson 1 Parametric Modeling Fundamentals Create Simple Parametric Models. Understand the Basic Parametric Modeling Process. Create and Profile Rough Sketches. Understand the "Shape before size" approach.

More information

Advanced CAD Modelling Course (SolidWorks 2009)

Advanced CAD Modelling Course (SolidWorks 2009) Advanced CAD Modelling Course (SolidWorks 2009) Published by: The National Centre for Technology in Education And T4 Technology Subjects Support Service National Centre for Technology in Education Dublin

More information

Creating T-Spline Forms

Creating T-Spline Forms 1 / 28 Goals 1. Create a T-Spline Primitive Form 2. Create a T-Spline Revolve Form 3. Create a T-Spline Sweep Form 4. Create a T-Spline Loft Form 2 / 28 Instructions Step 1: Go to the Sculpt workspace

More information

Workshop name: CAD Strategies for 3D Printing

Workshop name: CAD Strategies for 3D Printing Page 1 of 9 Workshop name: CAD Strategies for 3D Printing Presented by James Novak: Griffith University Lecturer, PhD Candidate, Industrial Designer Activity 1 Parametric Test Models Discussion: Additive

More information

Panel. Chapter 16. Solar Car. A. Sketch. Step 1. Click File Menu > New, click Part and OK. B. Save as "PANEL". Step 1. Click File Menu > Save As.

Panel. Chapter 16. Solar Car. A. Sketch. Step 1. Click File Menu > New, click Part and OK. B. Save as PANEL. Step 1. Click File Menu > Save As. Chapter 16 Solar Car Panel A. Sketch. Step 1. Click File Menu > New, click Part and OK. Step 2. Click Top Plane in the Feature Manager and click Sketch from the Content toolbar, Fig. 1. Step 3. Click Center

More information

Module 4A: Creating the 3D Model of Right and Oblique Pyramids

Module 4A: Creating the 3D Model of Right and Oblique Pyramids Inventor (5) Module 4A: 4A- 1 Module 4A: Creating the 3D Model of Right and Oblique Pyramids In Module 4A, we will learn how to create 3D solid models of right-axis and oblique-axis pyramid (regular or

More information

Revit Architecture 2015 Basics

Revit Architecture 2015 Basics Revit Architecture 2015 Basics From the Ground Up 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

More information

Structural & Thermal Analysis using the ANSYS Workbench Release 11.0 Environment. Kent L. Lawrence

Structural & Thermal Analysis using the ANSYS Workbench Release 11.0 Environment. Kent L. Lawrence ANSYS Workbench Tutorial Structural & Thermal Analysis using the ANSYS Workbench Release 11.0 Environment Kent L. Lawrence Mechanical and Aerospace Engineering University of Texas at Arlington SDC PUBLICATIONS

More information

Solidworks 2006 Surface-modeling

Solidworks 2006 Surface-modeling Solidworks 2006 Surface-modeling (Tutorial 2-Mouse) Surface-modeling Solid-modeling A- 1 Assembly Design Design with a Master Model Surface-modeling Tutorial 2A Import 2D outline drawing into Solidworks2006

More information

VERO UK TRAINING MATERIAL

VERO UK TRAINING MATERIAL VERO UK TRAINING MATERIAL VISI Basic 2-D Modelling course (V-16) VISI Modelling 2D Design Introduction Many component designs follow a similar route, beginning with a 2D design, part modelled using solids

More information

Project 3. Top Down Design In Context. Below are the desired outcomes and usage competencies based upon the completion of this Project.

Project 3. Top Down Design In Context. Below are the desired outcomes and usage competencies based upon the completion of this Project. Assembly Modeling with SolidWorks Project 3 Below are the desired outcomes and usage competencies based upon the completion of this Project. Project Desired Outcomes: 2AXIS-TRANSFER Assembly. PLATE-B Part.

More information

Parametric Modeling Design and Modeling 2011 Project Lead The Way, Inc.

Parametric Modeling Design and Modeling 2011 Project Lead The Way, Inc. Parametric Modeling Design and Modeling 2011 Project Lead The Way, Inc. 3D Modeling Steps - Sketch Step 1 Sketch Geometry Sketch Geometry Line Sketch Tool 3D Modeling Steps - Constrain Step 1 Sketch Geometry

More information

Parametric Modeling with. Autodesk Fusion 360. First Edition. Randy H. Shih SDC. Better Textbooks. Lower Prices.

Parametric Modeling with. Autodesk Fusion 360. First Edition. Randy H. Shih SDC. Better Textbooks. Lower Prices. Parametric Modeling with Autodesk Fusion 360 First Edition Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following websites

More information

Alibre Design Tutorial - Simple Revolve Translucent Glass Lamp Globe

Alibre Design Tutorial - Simple Revolve Translucent Glass Lamp Globe Alibre Design Tutorial - Simple Revolve Translucent Glass Lamp Globe Part Tutorial Exercise 2: Globe-1 In this Exercise, We will set System Parameters first. Then, in sketch mode, we will first Outline

More information

A Comprehensive Introduction to SolidWorks 2011

A Comprehensive Introduction to SolidWorks 2011 A Comprehensive Introduction to SolidWorks 2011 Godfrey Onwubolu, Ph.D. SDC PUBLICATIONS www.sdcpublications.com Schroff Development Corporation Chapter 2 Geometric Construction Tools Objectives: When

More information

Tutorial Second Level

Tutorial Second Level AutoCAD 2018 Tutorial Second Level 3D Modeling Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following websites to learn

More information

Chapter 2 Parametric Modeling Fundamentals

Chapter 2 Parametric Modeling Fundamentals 2-1 Chapter 2 Parametric Modeling Fundamentals Create Simple Extruded Solid Models Understand the Basic Parametric Modeling Procedure Create 2-D Sketches Understand the "Shape before Size" Approach Use

More information

REVIT ARCHITECTURE 2016

REVIT ARCHITECTURE 2016 Page 1 of 6 REVIT ARCHITECTURE 2016 Revit Architecture 2016: CREATE A CHAMFERED COLUMN COMPONENT About creating a chamfered column family typical to the Victorian cottage style. Add the column to your

More information

Parametric Modeling with UGS NX 4

Parametric Modeling with UGS NX 4 Parametric Modeling with UGS NX 4 Randy H. Shih Oregon Institute of Technology SDC PUBLICATIONS Schroff Development Corporation www.schroff.com www.schroff-europe.com 2-1 Chapter 2 Parametric Modeling

More information

Tutorial 3: Constructive Editing (2D-CAD)

Tutorial 3: Constructive Editing (2D-CAD) (2D-CAD) The editing done up to now is not much different from the normal drawing board techniques. This section deals with commands to copy items we have already drawn, to move them and to make multiple

More information

The Rectangular Problem

The Rectangular Problem C h a p t e r 2 The Rectangular Problem In this chapter, you will cover the following to World Class standards: The tools for simple 2D Computer Aided Drafting (CAD) The Command Line and the Tray The Line

More information

Designing Simple Buildings

Designing Simple Buildings Designing Simple Buildings Contents Introduction 2 1. Pitched-roof Buildings 5 2. Flat-roof Buildings 25 3. Adding Doors and Windows 27 9. Windmill Sequence 45 10. Drawing Round Towers 49 11. Drawing Polygonal

More information

3ds Max Cottage Step 1. Always start out by setting up units: We re going with this setup as we will round everything off to one inch.

3ds Max Cottage Step 1. Always start out by setting up units: We re going with this setup as we will round everything off to one inch. 3ds Max Cottage Step 1 Always start out by setting up units: We re going with this setup as we will round everything off to one inch. File/Import the CAD drawing Be sure Files of Type is set to all formats

More information

We can use square dot paper to draw each view (top, front, and sides) of the three dimensional objects:

We can use square dot paper to draw each view (top, front, and sides) of the three dimensional objects: Unit Eight Geometry Name: 8.1 Sketching Views of Objects When a photo of an object is not available, the object may be drawn on triangular dot paper. This is called isometric paper. Isometric means equal

More information

PLAY VIDEO. Fences can be any shape from a simple rectangle to a multisided polygon, even a circle.

PLAY VIDEO. Fences can be any shape from a simple rectangle to a multisided polygon, even a circle. Chapter Eight Groups PLAY VIDEO INTRODUCTION There will be times when you need to perform the same operation on several elements. Although this can be done by repeating the operation for each individual

More information

Terminal. Chapter 16. E-Car. A. Component from Design Library. SOLIDWORKS 17 Terminal E-CAR Page 16-1

Terminal. Chapter 16. E-Car. A. Component from Design Library. SOLIDWORKS 17 Terminal E-CAR Page 16-1 Chapter 16 E-Car Terminal A. Component from Design Library. Step 1. Click the Design Library tab in the Task Pane (right side of graphics area), Fig. 1. Step 2. Expand routing and click electrical folder

More information

UNIT 11: Revolved and Extruded Shapes

UNIT 11: Revolved and Extruded Shapes UNIT 11: Revolved and Extruded Shapes In addition to basic geometric shapes and importing of three-dimensional STL files, SOLIDCast allows you to create three-dimensional shapes that are formed by revolving

More information

Design and Communication Graphics

Design and Communication Graphics An approach to teaching and learning Design and Communication Graphics Solids in Contact Syllabus Learning Outcomes: Construct views of up to three solids having curved surfaces and/or plane surfaces in

More information

SolidWorks 2001 Getting Started

SolidWorks 2001 Getting Started SolidWorks 2001 Getting Started 1995-2001, SolidWorks Corporation 300 Baker Avenue Concord, Massachusetts 01742 USA All Rights Reserved. U.S. Patent 5,815,154 SolidWorks Corporation is a Dassault Systemes

More information

Module 5: Creating Sheet Metal Transition Piece Between a Square Tube and a Rectangular Tube with Triangulation

Module 5: Creating Sheet Metal Transition Piece Between a Square Tube and a Rectangular Tube with Triangulation 1 Module 5: Creating Sheet Metal Transition Piece Between a Square Tube and a Rectangular Tube with Triangulation In Module 5, we will learn how to create a 3D folded model of a sheet metal transition

More information

Lesson 2 Constructive Solid Geometry Concept. Parametric Modeling with I-DEAS 2-1

Lesson 2 Constructive Solid Geometry Concept. Parametric Modeling with I-DEAS 2-1 Lesson 2 Constructive Solid Geometry Concept Parametric Modeling with I-DEAS 2-1 2-2 Parametric Modeling with I-DEAS Introduction In the 1980s, one of the main advancements in Solid Modeling was the development

More information

Mastercam X6 for SolidWorks Toolpaths

Mastercam X6 for SolidWorks Toolpaths Chapter 14 Spinning Top Mastercam X6 for SolidWorks Toolpaths A. Insert Handle in New Assembly. Step 1. Click File Menu > New, click Assembly and OK. Step 2. Click Browse in the Property Manager, Fig.

More information