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Lego block - SolidWorks 2009

By Justin Cunningham,2014-03-09 01:01
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Lego block - SolidWorks 2009

Introduction to SolidWorks 2009

Introduction to SolidWorks 2009

RD9 DCG Design & Communication Graphics 1

Introduction to SolidWorks 2009

Getting started

    The first part that you will build is a Lego Brick. To begin building the part, you need to open a new SolidWorks part document. The new part document will be created based on a template. A template forms the foundation of a new document. The template can include user-defined parameters, annotations, or geometry. Templates allow you to define your only specific parameters, and then open new documents with those customised settings already set. In this way, you define parameters only once and the new documents are created with the customised settings. This saves a lot of repetitive work each time you use SolidWorks

    Note: The Sensors (only available in SW’s 2009) tool located in the FeatureManager

    monitors selected properties in a part or assembly and alerts you when they deviate from a pre-specified limit. There are four sensor types: Mass properties, Measurement,

    Interference Detection and Simulation data.

Starting SolidWorks and Opening a New Part

    Start the SolidWorks application.

    Click the Start menu from the Windows interface.

    Click All Programs, SolidWorks 2008, SolidWorks 2008.

    Tip: You can quickly start a SolidWorks session by double-clicking the left mouse button on the desktop shortcut, if there is a shortcut icon on the system desktop.

Open a new part.

    Click New from the Menu Bar toolbar. The New

    SolidWorks Document dialog box is displayed.

    Note: When SolidWorks 2008/09 is installed it

    automatically references the templates from 2006.

Click the Part template

    Click OK from the New SolidWorks Document

    dialog box. A new Part document window is

    displayed.

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Set System units.

    Click Options , Document Properties tab

    from the Menu Bar toolbar. The Document

    Properties - Drafting Standard dialog box is

    displayed.

    ANSI is the default Overall drafting standard.

    Click Units. Select MMGS, (millimeter, gram, second).

    Click inside the Length Decimals box. Select .12

    decimal places from the dropdown menu for Basic unit

    length. Accept the default settings.

    Click OK from the Document Properties - Units dialog box. Return to the SolidWorks Graphics area.

Begin Sketching

    Solid models are built from features. Initially, features are based on 2D sketches. The sketch is the basis for a

    3D model. Create a 2D sketch that you will later make into a 3D solid.

    Sketches are flat or planar. In the same way as we need a sheet of paper on which to sketch you need to choose a plane on which to sketch in SolidWorks. A SolidWorks part contains three default sketch planes. They represent the Front, Top, and Right planes.

Left click on the Top plane and choose Sketch

    Choose S on the keyboard. A context sensitive toolbar appears with a variety of sketch tools. Note: The toolbar appears where the cursor

    was last clicked.

    Similar commands are grouped into consolidated flyout buttons on the toolbar. These buttons appear with an arrow next to them eg. Rectangle.

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Click the Centre Rectangle tool from the shortcut toolbar. The Rectangle

    PropertyManager is displayed. The Centre Rectangle tool is displayed on the mouse icon.

Place the centre of the rectangle on the origin

    and drag the rectangle as shown.

Left click in the graphics area to position the

    rectangle.

    Press Esc on the keyboard to exit the command

Zoom to fit.

    Press the f key on the keyboard to return to the full Graphics area. Note: The horizontal and coincident geometrical relations are automatically added.

Smart Dimension

    Choose S to activate the shortcut toolbar and choose Smart Dimension .

Add the dimensions shown across.

    The sketch turns black and is fully defined

Exiting the sketch.

    Three options exist to exit the sketch. As in SolidWorks 2006 you may exit the sketch by choosing

    Exit Sketch from the confirmation corner or choose Exit Sketch from the CommandManager

The third option, new to SW 2008, is to double left click on a blank space in the graphics area

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Accessing a sketch to edit it.

    If you wish to edit an existing sketch left click on the sketch in the feature manager

    and choose Edit Sketch

Renaming features on creation

    To enable this feature Choose Tools, Options, FeatureManager Name feature on creation

Extruding the Lego Brick.

    The extrude tool may be accessed in two ways. 1. Click the Features tab from the CommandManager. The Features toolbar is displayed. Select the Extruded Boss/Base tool. The Extrude PropertyManager is displayed

    or

    2. Choose S on the keyboard. The context sensitive toolbar appears with

    appropriate feature tools available. Choose Extruded Boss/Base

Set the End Condition and Depth.

    Select Blind for End Condition in Direction 1. Enter a Depth of 10mm.

    You can use the up and down arrow buttons next to the Depth box to change

    the value by 10mms (default in system options) at a time.

    Click OK from the Extrude PropertyManager. The Extrude1 feature is created.

    Tip: Instant3D provides the ability to click and drag geometry and dimension

    manipulator points to resize or create

    features directly from the Graphics

    area. Use the on-screen ruler to

    measure your modifications.

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Using Instant3D

    Double click on the top surface of the model. An arrow will appear pointing upwards. Click and hold the tip of the arrow with the left hand mouse button. Drag the cursor, a ruler will appear. Move

    the cursor over the ruler and drag the cursor to change the Depth of the extrude in realtime. Press Esc to exit

    Instant3D and record the changes.

    Note: Ensure Instant 3D is enabled on the Features toolbar.

     Enabled Disabled

    Note: Return the Depth of Extrude1 to 10mm to continue with the exercise.

Saving Your Work

    Save the part document as Lego Brick.sldprt.

    You can save your files as often as you wish. However, there are really only two situations that require you to save your work:

    ; After you have done something you want to keep.

    ; Before you try something that you are not sure will work.

    Note: A file saved in a later version of SolidWorks cannot be opened in an earlier version i.e. A

    SolidWorks model created in SW2008 cannot be opened in SW2006.

Shell feature

    To create a wall thickness of 1mm we use the shell command. The shell command may be chosen from the commandmanager by selecting the features tab or by using the S key on the keyboard

Note: When the S key is chosen the pop-up toolbar does not contain the shell command. However, the button

    may be added by right clicking on the toolbar and choose customise.

Choose the features category and drag the shell command

    to the toolbar.

The shell command will appear on the pop-up toolbar

    each time it is activated from then on.

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Insert 1mm as thickness value for the walls

    of the Brick.

    Choose the underneath of the Brick as Faces to remove.

Choose OK.

Choose Isometric from the Heads-up View toolbar

Creating the cylindrical boss.

    Right-click the top face of the Lego Brick. The top face is the Sketch plane and is highlighted in the Graphics area.

    Click the Sketch tool from the Context toolbar.

Choose Normal to from the heads up toolbar

Choose Hidden Lines Visible from the heads up toolbar.

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Sketch a circle.

    Click the Circle tool from the pop-up toolbar.

    Circle PropertyManager is displayed.

Add the sketch as shown.

    Add the tangent relations between the circle and the hidden detail edges as shown.

    Smart dimension the circle to fully define the sketch.

    Choose Shaded with Edges and Isometric from the heads up toolbar. Exit the sketch

    Using Instant3D to create the Extruded Boss/Base Click on the sketch in the graphics area, an arrow appears as shown.

    Click and drag the arrow, as described earlier, to a Depth of 1.6mm.

Press Esc to exit Instant3D. Extrude 2 is created

    in the FeatureManager.

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Tesselation

    The display of geometry on your system may appear somewhat different from the illustrations. The lines may appear rougher. This is called tessellation. Tesselation or line display is related to the performance of the computer. Higher quality graphics or higher system settings will improve model appearance. Choose Tools, Options, Document Properties. Image Quality…

Inserting a Fillet Feature

    The Fillet feature rounds sharp edges and faces. We will use the Fillet feature to round the sharp edges of the

    Lego Brick. The Fillet feature requires an edge or face with a specified radius. In general, it is best to follow these few rules when inserting a fillet:

    1. Add larger fillets before smaller ones. When several fillets converge at a vertex, create the larger fillets first.

    2. Add drafts before fillets. If you are creating a molded or cast part with many filleted edges and drafted surfaces, in most cases you should add the draft features before the fillets.

    3. Save cosmetic fillets for last. Try to add cosmetic fillets after most other geometry is in place. If you add them earlier, it will take longer to rebuild the part.

    Choose Fillet from the Pop-up toolbar

Two PropertyManager tabs are available:

    1. Manual. Use this tab to maintain control at the feature level similar to the

    use of fillet command in SW2006.

    2. FilletXpert. Use this tab when you want the SolidWorks software to manage

    the structure of the underlying features for a constant radius fillet.

Fillet / FilletXpert PropertyManager

    The FilletXpert PropertyManager is displayed when you click the FilletXpert tab in the Fillet PropertyManager. The FilletXpert manages, organises, and reorders constant radius fillets. Use the Add tab to create new constant radius fillets.

    Use the Change tab to modify existing fillets. Use the Corner tab to create and

    manage fillet corner features where exactly three filleted edges meet at a single vertex.

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Choose the FilletXpert tab. Choose the Add tab.

    Choose the edge at the base of the cylinder as shown. A context sensitive toolbar appears.

    Moving the cursor over the buttons will select various other edges to add the fillet to. Choose the middle one. This will include the top edge of the cylinder in the selection.

Choose a Radius of 0.25mm.

    Choose Full preview

    Choose Apply

Choose the edges shown

    Choose a Radius of 0.1mm.

    Choose Apply

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