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Tutorial do Solidworks
Tipologia: Notas de estudo
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SDC
www.schroff-europe.com
David C. Planchard & Marie P. Planchard
INSIDE:
MultiMedia CD
An audio/visual presentation of the tutorial projects
PUBLICATIONS
Engineering Design with SolidWorks 2006
Project 4
Extrude and Revolve Features
Below are the desired outcomes and usage competencies based on the completion of Project 4.
Project Desired Outcomes: Usage Competencies:
Extrude and Revolve Features
Project 4-Extrude and Revolve Features
Project Objective
Design a FLASHLIGHT assembly according to the customer’s requirements. The FLASHLIGHT assembly will be cost effective, serviceable and flexible for future manufacturing revisions.
Design intent is the process in which the model is developed to accept future changes. Build design intent into the FLASHLIGHT sketches, features, parts and assemblies.
Create a custom Part Template. The Part Template is the foundation for the FLASHLIGHT parts.
Create the following parts:
The other parts for the FLASHLIGHT assembly are addressed in Project 5.
Create the Core and Cavity mold tooling required for the BATTERYPLATE.
On the completion of this project, you will be able to:
o Extruded Boss/Base. o Extruded Cut. o Edge and Face Fillets.
Engineering Design with SolidWorks 2006
o Revolved Boss/Base. o Revolved Boss Thin. o Revolved Cut Thin. o Dome. o Shell. o Circular Pattern.
o Draft Analysis. o Scale. o Parting Lines. o Shut-off Surfaces. o Parting Surfaces. o Tooling Split.
Project Overview
In Project 4, you begin the design of a FLASHLIGHT assembly according to the customer’s requirements. The FLASHLIGHT assembly will be cost effective, serviceable and flexible for future manufacturing revisions.
A template is the foundation for a SolidWorks document. A template contains settings for units, dimensioning standards and other properties. Create two part templates for the FLASHLIGHT Project:
Create two parts for the FLASHLIGHT assembly in this Project:
BATTERY part
BATTERY PLATE part
FLASHLIGHT Assembly
Engineering Design with SolidWorks 2006
Utilize the Mold Tools to create the cavity tooling plates for the BATTERYPLATE part.
Design Intent
The SolidWorks definition of design intent is the process in which the model is developed to accept future changes.
Models behave differently when design changes occur. Design for change. Utilize geometry for symmetry, reuse common features and reuse common parts.
Build change into the following areas:
Build the design intent in the sketch as the profile is created.
A profile is determined from the sketch tools, Example: rectangle, circle and arc.
Build symmetry into the profile through a sketch centerline, mirror entity and position about the reference planes and Origin.
Build design intent as you sketch with automatic relationships.
Isometric view Rotated Mold Tools
Cavity
BATTERY PLATE
Extrude and Revolve Features
A rectangle contains horizontal, vertical and perpendicular automatic relations.
Build design intent using added geometric relations. Example: horizontal, vertical, coincident, midpoint, intersection, tangent and perpendicular.
Example A: Develop a square profile.
Build the design intent to create a square profile.
Sketch a rectangle with the Origin approximately in the center. Insert a centerline. Add a midpoint relation. Add an equal relation between the two perpendicular lines. Insert a dimension to define the exact width of the square.
Example B: Develop a rectangular profile.
The bottom horizontal midpoint of the rectangular profile is located at the Origin.
Sketch a rectangle. Add a midpoint relation between the horizontal edge of the rectangle and the Origin. Insert two dimensions to define the width and height of the rectangle.
Build design intent into a feature by addressing symmetry, feature selection and the order of feature creations.
Example A: Extruded feature remains symmetric about a plane.
Utilize the Mid Plane Depth option.
Extrude and Revolve Features
Utilize dimensions, tolerances and notes in parts and assemblies to build the design intent into the Drawing.
Example A: Tolerance and material in the drawing.
Insert an outside diameter tolerance +.000/-.002 into the TUBE part. The tolerance propagates to the drawing.
Additional information on the design process and design intent is available in SolidWorks Help Topics, Introducing SolidWorks.
Project Situation
You work for a company that specializes in providing promotional tradeshow products. The company is expecting a sales order for 100,000 flashlights with a potential for 500,000 units next year. Prototype drawings of the flashlight are required in three weeks.
You are the design engineer responsible for the project. You contact the customer to discuss design options and product specifications. The customer informs you that the flashlights will be used in an international marketing promotional campaign. Key customer requirements:
Engineering Design with SolidWorks 2006
Your company’s standard product line does not address the above key customer requirements. The customer made it clear that there is no room for negotiation on the key product requirements.
You contact the salesperson and obtain additional information on the customer and product. This is a very valuable customer with a long history of last minute product changes. The job has high visibility with great future potential.
In a design review meeting, you present a conceptual sketch. Your colleagues review the sketch. The team’s consensus is to proceed with the conceptual design.
The first key design decision is the battery. The battery type directly affects the flashlight body size, bulb intensity, case structure integrity, weight, manufacturing complexity and cost.
Review two potential battery options:
The two options affect the product design and specification. Think about it.
A single 6-volt lantern battery is approximately 25% higher in cost and 35% more in weight. The 6-volt lantern battery does provide higher current capabilities and longer battery life.
A special battery holder is required to incorporate the four 1.5 volt D cell configuration. This would directly add to the cost and design time of the FLASHLIGHT assembly.
Time is critical. For the prototype, you decide to use a standard 6-volt lantern battery. This eliminates the requirement to design and procure a special battery holder. However, you envision the four D cell battery model for the next product revision.
Engineering Design with SolidWorks 2006
Activity: Part Template
Create the PART-IN-ANSI Template.
Click File, New from the Main menu.
Double-click Part from the default Templates tab.
Set the Dimensioning Standard to ANSI.
Click Tools, Options from the Main menu.
Click the Document Properties tab.
Select ANSI from the Dimensioning Standard list box.
Click the System Options tab.
Click Spin Box Increments.
Click the English units text box.
Enter .100.
Click the Metric units text box.
Enter 2.5.
Click the Document Properties tab.
Set the part units for inch.
Click Units.
Select IPS for Unit system.
Select 3 for Length units Decimal places.
Select millimeters for Dual units.
Select 2 for Decimal places.
Select 0 for Angular units Decimal places.
Click OK.
Save the part template.
Click File, Save As from the Main menu.
Click Part Templates (*.prtdot) from the Save As type list box.
Select ENGDESIGN-W-SOLIDWORKS\MY-TEMPLATES from the Save in list.
Extrude and Revolve Features
Enter PART-IN-ANSI in the File name text box.
Click Save.
Utilize the PART-IN-ANSI template to create the PART-MM-ISO template.
Click Tools, Options from the Main menu.
Click the Document Properties Tab.
Select ISO from the Dimensioning standard list box.
Set the part units for millimeter.
Click Units.
Select MMGS for Unit system.
Select 2 for Length units Decimal places.
Select 0 for Angular units Decimal places.
Click OK.
Save the part template.
Click File, Save As from the Main menu.
Click Part Templates (*.prtdot) from the Save As type list box.
Select My Documents\ENGDESIGN-W- SOLIDWORKS\MY- TEMPLATES from the Save in list.
Enter PART-MM-ISO in the File name text box.
Click Save.
Set the System Options for File Locations to display in the New dialog box.
Click Tools, Options from the Main menu.
Click File Locations from the System Options tab.
Extrude and Revolve Features
Select Toolbars, Features in SolidWorks Help Topic to review the function of each tool in the Features toolbar.
Additional information on System Options, Document Properties, File Locations and Templates is found in SolidWorks Help Topics. Keywords: Options (detailing, units), templates, Files (locations), menus and toolbars (features, sketch).
Review of the Part Templates.
You created two Part Templates: PART-MM-ISO and PART-IN-ANSI. The Document Properties Dimensioning Standard, Units and Decimal Places were stored in the Part Templates.
The File Locations System Option, Document Templates option controls the reference to the MY-TEMPLATES folder.
Note: In some network locations and school environments, the File Locations option must be set to MY-TEMPLATES for each session of SolidWorks.
You can exit SolidWorks at any time during this project. Save your document. Select File, Exit from the Main menu.
Engineering Design with SolidWorks 2006
BATTERY Part
The BATTERY is a simplified representation of a purchased OEM part. Represent the battery terminals as cylindrical extrusions. The battery dimensions are obtained from the ANSI standard 908D.
A 6-Volt lantern battery weighs approximately 1.38 pounds, (0.62kg). Locate the center of gravity closest to the center of the battery.
Create the BATTERY part.
Use features to create parts. Features are building blocks that add or remove material.
Utilize the Extruded Base feature. The Extrude Base features add material. The Base feature is the first feature of the part.
Utilize symmetry. Sketch a rectangle profile on the Top plane, centered at the Origin.
Extend the profile perpendicular (⊥) to the Top plane.
Utilize the Fillet feature to round four vertical edges.
The Extruded Cut feature removes material from the top face. Utilize the top face for the Sketch plane. Utilize the Offset Entity Sketch tool to create the profile.
Engineering Design with SolidWorks 2006
Activity: BATTERY Part-Extruded Base Feature
Create a new part.
Click File, New from the Main menu.
Click the MY-TEMPLATES tab.
Double-click PART-IN-ANSI, [PART-MM-ISO].
Save the empty part.
Click Save.
Select PROJECTS for Save in folder.
Enter BATTERY for file name.
Enter BATTERY, 6-VOLT for Description.
Click Save.
Select the Sketch plane.
Sketch the profile.
Click Sketch from the Sketch toolbar.
Click Top view.
Click Rectangle from the Sketch toolbar.
Click the first point in the lower left quadrant.
Drag and click the second point in the upper right quadrant. The Origin is approximately in the middle of the Rectangle.
First Point
Extrude and Revolve Features
Sketch the Centerline.
Click Centerline from the Sketch Tools toolbar.
Sketch a diagonal centerline from the upper left corner to the lower right corner. The endpoints of the centerline are coincident with the corner points of the Rectangle.
Add a Midpoint Relation.
Right-click Select in the Graphics window.
Click the centerline.
Hold the Ctrl key down.
Click the Origin.
Release the Ctrl key.
Click Midpoint from the Add Relations box.
Click OK from the Properties PropertyManager. Note: The Line# may be different than the line numbers above. The Line# is dependent on the line number order creation.
To clear entities from the Selected Entities box, right-click Clear Selections.
Create a square. Add an Equal Relation.
Click the top horizontal line.
Hold the Ctrl key down.
Click the left vertical line.
Release the Ctrl key.
Click Equal from the Add Relations box.
Click OK from the Properties PropertyManager.
