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Solidworks exercicios desenhos
Tipologia: Exercícios
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Workbook (Bring to each workshop)
Partially funded by the Engineering Excellence Fund.
College of Engineering and Applied Science University of Colorado at Boulder October 2003
Introduction REPRODUCIBLE
vi Student Workbook
Printing the Tutorials If you like, you can print the Online Tutorials by following this procedure: 1 On the tutorial navigation toolbar, click Show. This displays the table of contents for the Online Tutorials. 2 Right-click the book representing the lesson you wish to print and select Print from the shortcut menu. The Print Topics dialog box appears. 3 Select Print the selected heading and all subtopics , and click OK. 4 Repeat this process for each lesson that you want to print.
REPRODUCIBLE
2
Lesson 2: Basic Functionality
Goals of This Lesson
Upon successful completion of this lesson, you will understand the basic functionality of SolidWorks software and be able to create the following part:
REPRODUCIBLE Lesson 2: Basic Functionality
When other commands are active, the confirmation corner displays two symbols: a check mark and an X. The check mark executes the current command. The X cancels the command.
Overview of the SolidWorks Window
A sketch origin appears in the center of the graphics area. The Sketch Tools and Sketch Relations toolbars are displayed. “Editing Sketch” appears in the status bar at the bottom of the screen. Sketch1 appears in the FeatureManager design tree. The status bar shows the position of the pointer, or sketch tool, in relation to the sketch origin.
Sketch a Rectangle
6 Click on the Sketch Tools toolbar. 7 Click the sketch origin to start the rectangle. 8 Move the pointer up and to the right, to create a rectangle. 9 Click the mouse button again to complete the rectangle.
Sketch toolbar
Sketch Relations toolbar
Pointer
Status bar
Graphics area
Sketch origin
Menu bar
FeatureManager design tree
Sketch Tools toolbar
Confirmation Corner with sketch indicator
Reference Triad
Lesson 2: Basic Functionality REPRODUCIBLE
Add Dimensions
1 Click Dimension on the Sketch Relations toolbar. The pointer shape changes to. 2 Click the top line of the rectangle. 3 Click the dimension text location above the top line. The Modify dialog box is displayed.
4 Enter 100. Click or press Enter.
5 Click the right edge of the rectangle. 6 Click the dimension text location. Enter 65. Click. The top segment and the remaining vertices are displayed in black. The status bar in the lower- right corner of the window indicates that the sketch is fully defined.
Changing the Dimension Values
The new dimensions for the box are 100mm x 60mm. Change the dimensions. Use the Select tool.
7 Click Select on the Sketch toolbar. 8 Double-click 65. The Modify dialog box appears. 9 Enter 60 in the Modify dialog box.
10 Click.
Extrude the Base Feature.
The first feature in any part is called the Base Feature. In this exercise, the base feature is created by extruding the sketched rectangle.
11 Click Extruded Boss/Base on the Features toolbar. The Extrude Feature PropertyManager appears. The view of the sketch changes to isometric.
Lesson 2: Basic Functionality REPRODUCIBLE
15 Click the plus sign beside Extrude1 in the FeatureManager design tree. Notice that Sketch1 — which you used to extrude the feature — is now listed under the feature.
View Display
Change the display mode. Click Hidden Lines Visible on the View toolbar. Hidden Lines Visible allows you to select hidden back edges of the box.
Save the Part
1 Click Save on the Standard toolbar, or click File, Save. The Save As dialog box appears. 2 Type box for the filename. Click Save. The .sldprt extension is added to the filename. The file is saved to the current directory. You can use the Windows browse button to change to a different directory.
Round the Corners of the Part
Round the four corner edges of the box. All rounds have the same radius (10mm). Create them as a single feature.
3 Click Fillet on the Features toolbar. The Fillet PropertyManager appears. 4 Enter 10 for the Radius. Leave the remaining settings at their default values.
Click here
REPRODUCIBLE Lesson 2: Basic Functionality
5 Click the first corner edge. The faces, edges, and vertices are highlighted as you move the pointer over them. When you select the edge, a callout appears. 6 Identify selectable objects. Notice how the pointer changes shapes:
Edge: Face: Vertex:
7 Click the second, third and fourth corner edges.
8 Click. Fillet1 appears in the FeatureManager design tree.
Hollow Out the Part
Remove the top face using the Shell feature.
9 Click on the Features toolbar. The Shell Feature PropertyManager appears. 10 Enter 5 for Thickness.
Note: Normally, a callout only appears on the first edge you select. This illustration has been modified to show callouts on each of the four selected edges. This was done simply to better illustrate which edges you are supposed to select.
REPRODUCIBLE Lesson 2: Basic Functionality
Sketch the Circle
1 Click on the Sketch Tools toolbar. 2 Position the pointer where you want the center of the circle. Click the left mouse button. 3 Drag the pointer to sketch a circle. 4 Click the left mouse button again to complete the circle.
Dimension the Circle
Dimension the circle to determine its size and location.
5 Click on the Sketch Relations toolbar. 6 Dimension the diameter. Click on the circumference of the circle. Click a location for the dimension text in the upper right corner. Enter 10. 7 Create a horizontal dimension. Click the circumference of the circle. Click the left most vertical edge. Click a location for the dimension text below the bottom horizontal line. Enter 25. 8 Create a vertical dimension. Click the circumference of the circle. Click the bottom most horizontal edge. Click a location for the dimension text to the right of the sketch. Enter 40.
Extrude the Sketch
1 Click on the Features toolbar. The Extrude Cut Feature PropertyManager appears. 2 Select Through All for the end condition.
3 Click.
Lesson 2: Basic Functionality REPRODUCIBLE
4 Results. The cut feature is displayed.
Rotate the View
Rotate the view in the graphics area to display the model from different angles. 5 Rotate the part in the graphics area. Press and hold the middle mouse button. Drag the pointer up/down or left/right. The view rotates dynamically.
6 Display the Isometric view. Click on the Standard Views toolbar.
Save the Part
1 Click on the Standard toolbar 2 Click File, Exit on the Main menu.
REPRODUCIBLE Lesson 2: Basic Functionality
7 Create a simplified duplex outlet cover plate. The filename for the part is outletplate. 8 Save the parts. They will be used in later lessons.
REPRODUCIBLE Lesson 2: Basic Functionality
Lesson Summary
SolidWorks is design automation software. The SolidWorks model is made up of: Parts Assemblies Drawings Features are the building blocks of a part.
REPRODUCIBLE
3
Lesson 3: The 40-Minute Running Start
Goals of This Lesson
You will be able to create and modify the following part:
Before Beginning This Lesson
Complete the previous lesson — Basic Functionality.
Resources for This Lesson
This lesson plan corresponds to Lesson 1 – Parts in the SolidWorks Online Tutorials. For more information about the Online Tutorials, See “Online Tutorials” on page v.
Top View
Front View Right View
Isometric View
Lesson 3: The 40-Minute Running Start REPRODUCIBLE
Active Learning Exercise — Create a Part
Follow the instructions in Lesson 1 – Parts of the SolidWorks Online Tutorial. In this lesson you will create the part shown at the right. The part name is Tutor1.sldprt.
5 Minute Assessment
1 What features did you use to create Tutor1? ________________________________
2 What does the Fillet feature do?____________________________________________
3 What does the Shell feature do? ____________________________________________
4 Name three view commands in SolidWorks. __________________________________
5 Where are the display buttons located? ______________________________________
6 Name the three SolidWorks default planes. ___________________________________
7 The SolidWorks default planes correspond to what principle drawing views? ________
8 True or False. In a fully defined sketch, geometry is displayed in black. ____________
9 True or False. It is possible to make a feature using an over defined sketch. _________
10 Name the primary drawing views used to display a model._______________________
