Criando um Lens usando o SolidWorks: Passos para criar a base, conexão e detalhes, Notas de estudo de Informática

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SolidWorks 2001

Tutorial

A Basic Introduction

Marie P. Planchard & David C. Planchard

SDC

www.schroff.com

PUBLICATIONS

SolidWorks Tutorial Revolve Features

Project 2

Revolve Features

Below are the desired outcomes and usage competencies based upon the

completion of Project 2.

Project Desired Outcomes Usage Competencies

A comprehensive understanding of

the customer’s design requirements

and desires.

To comprehend the fundamental

definitions and process of Feature-

Based 3D Solid Modeling.

Specific knowledge of Revolve base

features.

Understanding of the Shell feature,

Hole Wizard, Dome feature and

Circular Pattern.

Two key flashlight components:

• LENS
• BULB

Ability to apply Extrude and Fillet

features.

SolidWorks Tutorial Revolve Features

Project 2 – Revolve Features

Project Objective

Create two components of the flashlight. Create the LENS and BULB.

Project Situation

The LENS is a purchase part

utilized in the FLASHLIGHT

assembly, Figure 2.1. Obtain

dimensional information on the

LENS. Review the size,

material and construction.

The BULB is a purchased part,

Figure 2.2. The BULB is a

replacement part and requires a

separate part number and order

number.

Project Overview

Create two parts in this section:

• LENS
• BULB

The LENS and the BULB utilize a Revolve Base feature.

LENS

Determine the key features of the LENS. The Base feature for the LENS is a solid

Revolved feature. A solid Revolved feature adds material. The Revolved Base

feature is the foundation

for the LENS.

A Revolved feature is

geometry created by

rotating a sketched

profile around a

centerline, Figure2.3.

Close the Sketch profile

for a solid Revolved

feature, Figure 2.4. Do not cross the centerline.

Figure 2.3 Figure 2.

Center line

Profile

Figure 2.1 Figure 2.

Revolve Features SolidWorks Tutorial

LENS Feature Overview

Create the LENS. Use the solid Revolved Base

feature, Figure 2.5.

Create uniform wall thickness. Create the Shell

feature, Figure 2.6.

Create an Extruded-Boss feature from the back of

the LENS, Figure 2.7.

Create a Thin-Revolved feature to connect the

LENS to the BATTERYPLATE, Figure 2.8.

Create a Counterbore Hole feature with the HoleWizard, Figure 2.9. The BULB

is located inside the Counterbore Hole.

Create the front LensFlange feature. Add a transparent LensShield feature,

Figure 2.10.

Figure 2.

Figure 2.6 Figure 2.7 (^) Figure 2.

Figure 2.9 Figure 2.

Counter bore

Revolve Features SolidWorks Tutorial

On-line help contains an animation file to create a 3-point arc. Click Help, Index, Arc,

3Point. Run the animation. Click the AVI icon.

6. Create a 3 Point Arc. Click 3Pt Arc

. Create the arc start point. Click the top point on the left vertical line. Hold the left mouse button down. Drag the mouse pointer to the top point on the right vertical line.

Create the arc end point. Release the mouse button.

Click and drag the arc center point below the Origin. Release the left mouse button.

7. Add geometric relationships. Click Add

Relations. The arc is currently selected. Click the arc to remove it from the Select Entities text box. Create an equal relationship. Click the left vertical line. Click the horizontal line. Click the Equal button. Click Apply. Click Close.

8. Add dimensions. Click Dimension. Create a vertical linear dimension for the left line. Enter 2.000. Create a vertical linear dimension for the right line. Enter 0.400. Create a radial dimension for the arc. Enter 4.000. The black Sketch is fully defined.

Centerline

Equal profile lines

Center point for 3Point arc

Drag arc center point below the Origin

SolidWorks Tutorial Revolve Features

9. Revolve the Sketch. Click Revolve from the Feature toolbar. The Revolve Feature dialog box is displayed. Accept the default option values. Create the solid Revolve feature. Click OK.

10. Save the LENS. Click

Save.

Revolve features contain an axis of revolution. The axis is critical to align other features.

11. Display the axis of revolution. Click View from the Main menu. Click Temporary Axis. A check mark is displayed next to the option. Hide the Temporary axis. Click Temporary Axis to remove the check mark. Hide the Planes. Click Planes to remove the check mark.

Solid Revolve features must contain a closed profile. Each revolved profile requires an individual sketched centerline.

Create the LENS - Shell Feature

The Shell feature removes face material from a solid. The Shell feature requires a

face and thickness. Use the Shell feature to create thin-walled parts.

Create the Shell feature.

12. Select the face. Click the front face of the Base-Revolve feature. Click Shell from the Feature toolbar. Enter 0.250 in the Thickness text box. Display the Shell feature. Click OK.

SolidWorks Tutorial Revolve Features

Create the Counterbore Hole. Click HoleWizard. The Hole Definition dialog box is displayed. Click the Counterbore tab.

21. Define the parameters. Click the Parameter 1 Binding in the Screw type property text box. The Parameter 1 and Parameter 2 text boxes are displayed.

22. Enter Hex Bolt from the drop down list for Screw type. Select ½ from the drop down list for Size. Click Through All from the drop down list for End Condition & Depth. Accept the Hole Fit and Diameter value. Click the C-Bore Diameter value. Enter 0.600. Click the C-Bore Depth value. Enter 0.200.

23. Add the new hole type to the favorites list. Click the Add button. Enter CBORE FOR BULB. Click OK.

Revolve Features SolidWorks Tutorial

24. Click Next from the Hole Definition dialog box. Position the hole coincident with the Origin. Click Add Relations

. Click the center point of the Counterbore hole. Click the

Origin. Click Coincident. Complete the hole. Click Finish from the Hole Wizard.

25. Expand the Hole. Click Plus Sign to the left of the Hole feature. Sketch3 and Sketch4 are used to create the Hole feature.

26. Display the Section view of BulbHole through the Right plane. Click the Right plane from the FeatureManager. Click View from the Main menu. Click Display, SectionView. Click the Flip Side to View check box. Click OK. Display the Isometric View. Click Isometric.

27. Display the Full view. Click View, Display, SectionView.

28. Rename CboreHole1 to BulbHole.

29. Save the LENS. Click Save.

Create the LENS - Boss Revolve Thin Feature

Create a Boss Revolve Thin feature. Rotate an open sketched profile around a

centerline. The sketch profile must be open and cannot cross the centerline. The

Tangent Arc sketch tool utilizes extracted geometry created with the Convert

Entities sketch tool. Delete the extracted geometry after the Tangent Arc is

created.

Use the Boss Revolve Thin feature to physically connect the LENS to the

BATTERYPLATE in the FLASHLIGHT.

Create the Boss Revolve Thin feature.

30. Select the Sketch plane. Click the Right plane. Display the Right view. Click Right

.

31. Create the Sketch. Click Sketch. Sketch the centerline. Click Centerline. Sketch a horizontal centerline collinear to the Top plane through the Origin. The new centerline is collinear with the Temporary axis.

Revolve Features SolidWorks Tutorial

37. Add geometric relations.

Click Add Relations. Click the arc center point. Click the horizontal line (silhouette edge) of the Base-Revolve feature. Click the Coincident button. Click Apply. Click Close.

The black Sketch is fully defined.

38. Revolve the Sketch. Click Revolve. A warning message appears:

39. Keep the Sketch open. Click No. The Thin Feature check box is active.

40. Create the Thin-Revolved feature on both sides of the Sketch. Select Mid-Plane from the Type list box. Enter 0.050 for Wall Thickness. Display the Boss-Revolve-Thin feature. Click OK.

41. Rename Boss-Revolve-Thin1 to LensConnector.

42. Save the LENS. Click Save.

43. Turn off the Temporary Axis. Click Views. Click Temporary Axis to uncheck.

Silhouette Edge

SolidWorks Tutorial Revolve Features

Create the LENS - Extruded Boss Feature

Use the Extruded-Boss feature to create the front LensCover. The feature extracts

the front outside circular edge from the Base-Revolve feature. The front

LensCover is a key feature for designing the mating component. The mating

component is the LENSCAP.

Create the Extruded Boss feature.

44. Select the Sketch plane. Click the front circular face. Display the Front view. Click Front.

45. Create the Sketch. Click Sketch. Click the outside circular edge. Click the Offset Entities. Click the Bi-directional check box. Enter 0.250.

46. Extrude the Sketch. Click Extrude Boss/Base. Enter 0.250 for Depth.

47. Display the Boss-Extrude feature. Click OK.

48. Rename Boss-Extrude to LensCover.

49. Save the LENS. Click Save.

Extrude Direction

SolidWorks Tutorial Revolve Features

54. Add transparency to the LensShield. Right-click the LensShield in the Graphics window. Click Feature Properties. The Feature Properties dialog box is displayed.

55. Click the Color button. The Entity Property dialog box is displayed. Click the Advanced button.

56. Set the transparency for the feature. Drag the Transparency slider to the far right side. Click OK from the Material Properties dialog box. Click OK from the Entity Property dialog box. Click OK from the Feature Properties box.

Revolve Features SolidWorks Tutorial

57. Display the transparent faces.

Click Shaded. When the LensShield is selected, the faces are not transparent. Click in the Graphics window to display the face transparency.

58. Save the LENS. Click

Save.

BULB

The BULB is contained within the LENS assembly.

The BULB is a purchased part. The BULB utilizes

the Revolved feature as the Base feature.

BULB Feature Overview

Create the Revolved Base feature from a sketched

profile on the Right plane, Figure 2.11a.

Create a Revolved Boss feature using a B-Spline sketched profile. A B-Spline is a

complex curve, Figure 2.11b.

Create a Revolved Cut Thin feature at the base of the BULB, Figure 2.11c.

Create a Dome feature at the base of the BULB, Figure 2.11d.

Create a Circular Pattern feature from an Extruded Cut, Figure 2.11e.

Modify the BULB to practice Edit Definition and Edit Sketch after a design

change.

Figure 2.11a 2.11b 2.11c 2.11d 2.11e

Revolve Features SolidWorks Tutorial

63. Add dimensions. Click Dimension.

Create a vertical linear dimension. Click the right line. Enter .200.

Create a vertical linear dimension. Click the left line. Enter .295.

Create a horizontal linear dimension. Click the top left line. Enter 0.100.

Create a horizontal linear dimension. Click the top right line. Enter 0.500.

64. Revolve the Sketch. Click Revolve from the Feature toolbar. The Revolve Feature dialog box is displayed. Accept the default option values. Click OK.

65. Save the BULB. Click Save.

Create the BULB - Revolved Boss Feature

The bulb requires a second solid Revolve feature. The profile utilizes a complex

curve called a B-Spline (Non-Uniform Rational B-Spline or NURB). B-Splines

are drawn with control points. Adjust the shape of the curve by dragging the

control points.

Create the Revolved Boss feature.

66. Turn the Grid Snap off. Click Grid. Uncheck the Snap to points check box.

67. Select the Sketch plane. Click the Right plane. Display the Right view. Click Right

.

.

SolidWorks Tutorial Revolve Features

68. Create the Sketch. Click Sketch. Sketch the centerline. Click Centerline. Sketch a horizontal centerline collinear to the Top plane,

coincident to the Origin.

Sketch the profile. Click B-Spline. Sketch the start point. Click the left vertical edge of the Base feature.

Sketch the control point. Drag the mouse pointer to the left of the Base feature and below the first point. Release the mouse button.

Sketch the end point. Click the control point. Drag the mouse pointer to the centerline. Release the mouse button.

69. Adjust the B-Spline. Click Select. Position the mouse pointer over the B-Spline control point. Drag the mouse pointer upward. Release the mouse button.

Note: SolidWorks does not require dimensions to create a feature.

70. Complete the profile. Sketch two lines. Click Line. Create a horizontal line. Sketch a horizontal line from the B-Spline endpoint to the left edge of the Base-Revolved feature. Create a vertical line. Sketch a vertical line to the B-Spline start point, collinear with the left edge of the Base- Revolved feature.

71. Revolve the Sketch. Click Revolve from the Feature toolbar. The Revolve Feature dialog box is displayed. Accept the default options. Display the Revolve feature. Click OK.

72. Save the BULB. Click Save.

Create the BULB - Revolved Cut Thin Feature

A Revolved Cut Thin feature removes material by

rotating an open sketch profile around a centerline.

Create the Revolved Cut Thin feature.

73. Select the Sketch plane. Click the Right plane.

End point Control point Start

Horizontal and Vertical lines