DOC

w-2a-creating-parts-1-solids

By Laurie Elliott,2014-01-06 19:19
13 views 0
w-2a-creating-parts-1-solids

    Workshop 2a

    Creating Solid and Rigid PartsHinge Model

    Goals

    ; Create and modify a base feature for a deformable solid part

    ; Add solid extrusion and cut features to a part

    ; Use datum geometry to position a sketch

    ; Create a rigid part of revolution

    Introduction

    In this workshop you will create three parts using Abaqus/CAE. The components are part of the hinge assembly shown in Figure W2a1 and will be used in subsequent workshops

    to build a complete model and perform an analysis. It is important that you use the dimensions stated and not deviate from the workshop; otherwise, you may find it difficult to assemble the model and complete subsequent workshops. The structure consists of two deformable hinge components (one with a lubrication hole, one without) and a rigid pin.

    Figure W2a1. Hinge assembly (left) and discretized finite element model (right)

    In the first part of the workshop you will create the hinge component with the lubrication hole. Next, you will create the hinge component without the lubrication hole by copying and modifying the hinge component with the hole. In the third part of the workshop you will create the rigid pin.

    ? Dassault Systèmes, 2008 Introduction to Abaqus/CAE

    W2a.2 Creating the hinge component with the lubrication hole

    Figure W2a2 shows the hinge component with the lubrication hole as a shaded plot. You will create this component first.

    Figure W2a2. Hinge component with lubrication hole

    Creating the base feature

    First you will create the base feature to which the flange will be attached.

    1. Start a new session of Abaqus/CAE from the ../CAE/Workshops/hinge

    directory by entering the following command at the prompt:

    abaqus cae

    2. Select Create Model Database from the Start Session dialog box.

    3. Abaqus/CAE enters the Part module and displays the Model Tree in the left side

    of the main window.

    4. Create the base block of the hinge component. In the Model Tree, double-click

    the Parts container to create a new part. The text in the prompt area asks you to

    fill out the Create Part dialog box, shown in Figure W2a3.

    Figure W2a3. Create Part prompt

    Abaqus/CAE always displays prompts in the prompt area to guide you through a procedure.

    5. Name the part Hinge-hole; and ensure that the selections for Modeling Space,

    Type, and Base Feature are as shown in Figure W2a4.

    ? Dassault Systèmes, 2008 Introduction to Abaqus/CAE

    W2a.3

    Figure W2a4. Create Part dialog box

    6. Enter 0.2 as the Approximate size of the model, as shown in Figure W2a4.

    The units used for the parts are meters. Abaqus/CAE does not have any built-in

    units. It is the user's responsibility to choose a consistent set of units. The

    approximate size chosen should be sufficient so that any aspect of the part can be

    modeled.

    7. Click Continue.

    Abaqus/CAE initializes the Sketcher and displays a grid.

    8. Click the Sketcher Options tool in the Sketcher toolbox to change the

    sketcher options. Enter a value of 0.01 in the Grid spacing entry field, and make

    sure that there are no other digits to the right of the digits you entered. Take a

    minute to review the available options before clicking OK.

    9. From the Sketcher toolbox, select the rectangle tool .

    10. Sketch an arbitrary rectangle, and click mouse button 2 in the viewport to exit the

    rectangle tool.

    11. Dimension the top and left edges so that each is 0.04 m long.

    12. Click mouse button 2 to exit the Sketcher.

    ? Dassault Systèmes, 2008 Introduction to Abaqus/CAE

    W2a.4 13. In the Edit Base Extrusion dialog box, enter an extrusion depth of 0.05 and

    click OK.

    14. Abaqus/CAE exits the Sketcher and displays the extruded part as a shaded plot in

    the viewport. Drag the Render Model toolbar over the

    viewport and use the tools to change the render style. Modifying the base feature

    You will now modify the base feature to change the shape into a cube. 1. In the Model Tree, expand the Hinge-hole item underneath the Parts container.

    Then expand the Features container that appears. In the list of features that

    appears, double-click Solid extrude-1.

    Figure W2a5. Expanded Model Tree

    2. The Edit Feature dialog box appears. Enter 0.04 as the Depth, as shown in

    Figure W2a6.

    Figure W2a6. Edit Feature dialog box

    3. Click OK.

    The feature will be regenerated, and the viewport displays the cubical base feature

    of the first hinge component.

    ? Dassault Systèmes, 2008 Introduction to Abaqus/CAE

    W2a.5

    Adding the flange to the base feature

    You will now add the flange, which includes the main bore, to the base feature. The

    lubrication hole will be added later.

    1. In the toolbox, click (or select Shape?Solid?Extrude from the main

    menu bar).

    2. Select the face at the front of the cube by moving the mouse pointer over the

    desired face. Click mouse button 1. Note that the selection options can be used to

    select faces if required.

    3. Select the edge indicated in Figure W2a7 as the edge that will appear vertical

    and on the right side of the sketch.

    Select this edge

    Figure W2a7. Face and edge selection

    4. As before, the approximate shape of the new feature will be sketched first. From

    the Sketcher toolbox, select the connected lines tool .

    5. Sketch the rectangular portion of the flange by drawing three lines as follows.

    a. Starting at any point to the right of the cube, connect the line to the top-

    right corner of the cube.

    b. Continue the next line to the bottom-right corner of the cube. This line is

    automatically assigned a vertical constraint.

    c. The final line extends from the bottom-right corner of the cube to any

    point to the right of the cube.

    6. Click mouse button 2 in the viewport to exit the connected lines tool. 7. Refine the sketch by defining the following constraints and dimension.

    a. Use the constraints tool to constrain the top and bottom lines of the

    sketch so that each is horizontal.

    ? Dassault Systèmes, 2008 Introduction to Abaqus/CAE

    W2a.6 b. Assign an equal length constraint to these two lines (use [Shift]+Click to

    select both lines).

    c. Dimension either line so that it is 0.02 m long.

    d. The sketch appears as shown in Figure W2a8.

    Figure W2a8. Rectangular portion of the flange

    8. Close the profile by adding a semicircular arc using the 3-points circle tool .

    a. Select the two vertices at the open end of the rectangle as the endpoints of

    the arc, starting with the top one. Select any point to the right of the sketch

    as a point that lies on the arc.

    b. Define tangent constraints between the ends of the arc and the horizontal

    lines to refine the sketch

    9. Click mouse button 2 in the viewport to exit the 3-points circle tool.

    The resulting arc is shown in Figure W2a9.

    Figure W2a9. Curved portion of the flange

    ? Dassault Systèmes, 2008 Introduction to Abaqus/CAE

    W2a.7

    10. From the Sketcher toolbox, select the center-perimeter circle tool to sketch

    the flange hole.

    a. Place the center of the circle to approximately coincide with the center of

    the arc created previously. The perimeter point should be placed to the

    right of the center point. Apply a concentric constraint between the two

    circular regions.

    b. Use the dimension tool to change the value of the radius to 0.01 m.

    c. Dimension the vertical distance between the center of the circle and the

    perimeter point. Edit this dimension so that the distance is 0. (If the

    distance is already 0, you cannot add a vertical dimension.) This will

    adjust the location of the perimeter point so that it is on the same

    horizontal plane as the center point.

    Note: When you mesh a part, Abaqus/CAE places nodes wherever

    vertices appear along an edge; therefore, the location of the vertex on the

    circumference of the circle influences the final mesh. Placing it on the

    same horizontal plane as the center point results in a high-quality mesh.

    The final sketch is shown in Figure W2a10.

    Figure W2a10. Final sketch

    11. Click mouse button 2 in the viewport to exit the sketcher. In the Edit Extrusion

    dialog box, select Blind as the end condition type, and enter 0.02 as the extrusion

    depth. Abaqus/CAE displays an arrow indicating the extrusion direction. By default, this arrow points in the direction of the outward normal of the selected face. Click Flip in the dialog box, and then click OK.

    12. Use the Fit View tool to resize the display to fit in the viewport.

    ? Dassault Systèmes, 2008 Introduction to Abaqus/CAE

    W2a.8

    Modifying the main bore

    Previously you modified the base feature by changing the extrusion depth (which is a feature attribute). Now you will modify a feature by editing the sketch.

    1. In the Model Tree, expand the Hinge-hole item underneath the Parts container.

    Then expand the Features container that appears. In the list of features, expand

    the contents of Solid extrude-2 (the flange).

    2. Double-click Section Sketch underneath Solid extrude-2.

    3. From the edit tools in the Sketcher toolbox, select the edit dimension value tool

    .

    4. Select the radial dimension of the circle (0.01). In the Edit Dimension dialog box,

    type a new radius of 0.012 and click OK.

    5. Click mouse button 2 in the viewport to exit the Edit Dimension Value tool.

    6. Click mouse button 2 in the viewport to exit the Sketcher toolset, and click OK in

    the Edit Feature dialog box to confirm the change.

    7. From the main menu bar, select Feature?Regenerate.

    Abaqus/CAE regenerates the feature and displays the updated geometry in the

    viewport.

    Creating a stand-alone sketch of the lubrication hole You will now create a stand-alone sketch, which will be used to extrude the lubrication hole. It is advantageous to use a stand-alone sketch when a feature of similar size and shape is used for several parts of an assembly.

    1. In the Model Tree, double-click Sketches.

    2. Name the sketch Hole, and use an Approximate size of 0.2. Click Continue.

    3. Use the Create Circle: Center and Perimeter tool , and create a circle with a

    radius of 0.01 centered at the origin. Enter the coordinates of the center point 0.0,

    0.0 and a perimeter point 0.01, 0 in the text box in the prompt area.

    4. Dimension the radius of the circle to 0.003.

    5. Click Done in the prompt area to complete the sketch.

    Creating a sketch plane

    As can be seen in Figure W2a2, the lubrication hole is drilled through the flange at an angle to the main axis of the part. To model this feature, you will create a sketch plane from which the lubrication hole will be extruded.

    1. Double-click Hinge-hole in the Model Tree to make the part current in the

    viewport.

    ? Dassault Systèmes, 2008 Introduction to Abaqus/CAE

    W2a.9

    Figure W2a11. Part Hinge-hole selected

    2. From the main menu bar, select Tools?Datum.

    The Create Datum dialog box appears.

    3. Choose Point as the datum Type and select Enter parameter from the list, as

    shown in Figure W2a12.

    Figure W2a12. Create Datum dialog box

    4. Select the curved edge of the flange, as shown in Figure W2a13.

    Figure W2a13. Edge selection for datum plane creation 5. The arrow indicates the direction along which the edge parameter increases. The

    parameter ranges in value from 0.0 to 1.0. If the sense of the arrow is as shown in

    ? Dassault Systèmes, 2008 Introduction to Abaqus/CAE

    W2a.10 Figure W2a12, enter a value of 0.25; otherwise, enter 0.75, and press [Enter].

    Abaqus/CAE creates a point at 1/4 the length of the edge, which in this case is a

    point located at 45º from the horizontal axis of the main bore in the flange. 6. Create a datum axis to define the normal to the datum plane. Select the Axis

    datum type from the Create Datum dialog box. Then select the 2 points option

    from the Method list. Select the center of the main bore and the datum point you

    created previously. Abaqus/CAE will create the datum axis, as shown in Figure

    W2a14.

    Figure W2a14. Hinge component with datum axis

    7. From the Create Datum dialog box, select Plane and choose the method Point

    and normal. Select the datum point previously created and the datum axis.

    Abaqus/CAE will construct the datum plane through this point and normal to the

    datum axis. Your model should now look similar to the one shown in Figure

    W2a15.

    Figure W2a15. Model with datum plane

8. Close the Create Datum dialog box.

    ? Dassault Systèmes, 2008 Introduction to Abaqus/CAE

Report this document

For any questions or suggestions please email
cust-service@docsford.com