direct coupled-field analysis of a bimetallic beam under a thermal load

digital

1. Problem Description

A bimetallic beam consists of two materials with different coefficients for thermal expansion, α1 and α2, and is initially at a reference temperature of 0° F. The beam is simply supported and a uniform temperature is applied to both surfaces. The beam is expected to undergo a large lateral deflection. Determine the midspan deflection after heating and verify the temperature T at the material interface.

digital

2. Problem Specifications

Material properties:

for each strip:
k1 = k2 = 5 BTU/hr-in-°F
for material 1:
E1 = 10e6 psi
α1 = 14.5e-6 in/in°F
for material 2:
E2 = 10e6 psi
α1 = 2.5e-6 in/in°F

Geometric properties for this problem are:

L = 10 in
t = 0.1 in

Loading for this problem is:

Ttop = 400.0°F
Tbot = 400.0°F

Since the problem is symmetric, only one-half of the beam is modeled. The AZ degree of freedom is not required in the analysis and is excluded from the matrix formulation by not specifying any magnetic material properties. A convergence criteria force is specified with a tight tolerance to converge the large deflection behavior.

digital

3. Problem Sketch

digital

4. Procedure

digital

Step 1: Specify the Title and Set Preferences

1. Choose menu path Utility Menu> File> Change Title.

2. Enter the text "Bimetallic beam under thermal load."

3. Click on OK.

digital

Step 2: Define Element Types

1. Choose menu path Main Menu> Preprocessor> Element Type> Add/Edit/Delete. The Element Types dialog box appears.

2. Click on Add. The Library of Element Types dialog box appears.

3. In the left scroll box, scroll to Coupled Field and select it.

4. In the right scroll box, click once on Vector Quad 13.

5. Click on OK.

6. Click on Options. The PLANE13 element type options dialog box appears.

7. In the scroll box for Element degrees of freedom, scroll to UX UY TEMP AZ and select it.

8. In the scroll box for Element behavior, scroll to Plane stress and select it.

9. Click on OK, then click on Close.

digital

Step 3: Define Material Properties

1.Choose menu path Main Menu> Preprocessor> Material Props> Material Models. The Define Material Model Behavior dialog box appears.

2. In the Material Models Available window, double-click on the following options: Structural, Linear, Elastic, Isotropic. A dialog box appears.

3. Enter 10e6 for EX (Elastic modulus). Click on OK. Material Model Number 1 appears in the Material Models Defined window.

4. In the Material Models Available window, double-click on the following options: Thermal Expansion Coef, Isotropic. A dialog box appears.

5. Enter 14.5e-6 for ALPX (Thermal expansion coefficient). Click on OK.

6. In the Material Models Available window, double-click on the following options: Thermal, Conductivity, Isotropic. A dialog box appears.

7. Enter 5 for KXX (Thermal conductivity). Click on OK.

8. Choose menu path Edit>Copy. Click on OK to copy Material Model Number 1 to Material Model Number 2. Material Model Number 2 appears in the Material Models Defined window on the left.

9. In the Material Models Defined window, double-click on Material Model Number 2, and on Thermal Expansion (iso). A completed dialog box appears.

10. In the ALPX field, change the value to 2.5e-6. Click on OK.

11. Click on menu path Material>Exit to remove the Define Material Model Behavior dialog box.

digital

:IStep 4: Create and Glue Rectangles

1. Choose menu path Main Menu> Preprocessor> Modeling> Create> Areas> Rectangle> By Dimensions. The Create Rectangle by Dimensions dialog box appears.

2. Enter 0, 5 and 0,.05 for the X and Y coordinates. Use the TAB key to move between fields.

3. Click on Apply.

4. Enter 0,5 and .05,.10 for the X and Y coordinates and click on OK.

5. Choose menu path Main Menu> Preprocessor> Modeling> Operate> Booleans> Glue> Areas. The Glue Areas picking menu appears.

6. Click on Pick All.

7. Choose menu path Main Menu> Preprocessor> Meshing> Mesh Attributes> Picked Areas.

8. In the graphics window, click on the top rectangle (Area 3 after the glue operation) and click on OK in the picking menu. The Area Attributes dialog box appears.

9. Enter 2 for material number and click on OK.

digital

Step 5: Set Element Density and Mesh

1.Choose menu path Main Menu> Preprocessor> Meshing> Size Cntrls> Global> Size. The Global Element Sizes dialog box appears.

2.Enter 1 for No. of element divisions and click on OK.

3. Choose menu path Main Menu> Preprocessor> Meshing> Mesh> Areas> Free. The Mesh Areas picking menu appears.

4. Click on Pick All.

5. Click on SAVE_DB on the ANSYS Toolbar.

digital

:})Step 6: Set Boundary Conditions and Initial Temperatures.

1. Choose menu pathUtility Menu> Select> Entities.

2. In the top scroll box, select Nodes.

3. In the second scroll box, select By Location.

4. Click on X coordinates to select it, and enter 0 for Min, Max.

5. Click on Apply.

6. Click on Y coordinates, then Reselect.

7. Enter .05 for Min, Max, and click on OK.

8. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears.

9. Click on Pick All. The Apply U,ROT on Nodes dialog box appears.

10. Click on UY for DOFs to be constrained and click on OK.

11. Choose menu path Utility Menu> Select> Entities.

12. Click on X coordinates to select it, click on From Full, enter 5 for Min, Max and click on OK.

13.Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> Symmetry B.C.> On Nodes. The Apply SYMM on Nodes dialog box appears.

14.Click on OK to accept the default of Symm surface is normal to X-axis.

15.Choose menu path Utility Menu> Select> Everything.

16. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On Nodes. The Apply U,ROT on Nodes picking menu appears.

17.Click on Pick All. The Apply U,ROT on Nodes dialog box appears.

18.Unselect UY and select Temp.

19.Enter 400 for displacement value and click on OK.

digital

;)Step 7: Set Analysis Type and Large Deformation Option

1.Choose menu path Main Menu> Solution> Analysis Type> New Analysis.

2.Click on OK to accept the default of Static.

3.Choose menu path Main Menu> Solution> Analysis Options. The Static or Steady-State Analysis dialog box appears.

4.Click Large deform effects option on and click on OK.

digital

)Step 8: Set Convergence Based on Force Only

1.Choose menu path Main Menu> Solution> Load Step Opts> Nonlinear> Convergence Crit. The Default Nonlinear Convergence Criteria dialog box appears.

2.Click on F to select it and click on Replace.

3.Enter 0.1 for Minimum reference value and click on OK.

4.Close the warning message box.

5.Click on Close.

digital

B)Step 9: Solve the Model

1.Choose menu path Main Menu> Solution> Solve> Current LS.

2.Review the information in the status window, and click on Close when finished.

3.Click on OK in the Solve Current Load Step dialog box to begin the solution.

4.Close the warning box and choose Yes to the question "Should solve be executed?".

5.Click on Close when the solution is done.

digital

:8)Step 10: Look at the Deformed Shape

1.Choose menu path Utility Menu> PlotCtrols> Style> Displacement Scaling.

2.Click on 1.0 (true scale) for Displacement scale factor and click on OK.

3.Choose menu path Main Menu> General Postproc> Plot Results> Deformed Shape. The Plot Deformed Shape dialog box appears.

4.Click on Def + undeformed, and click on OK. The deformed shape appears on the ANSYS Graphics window.

digital

:!(Step 11: List Nodal Solution

1.Choose menu path Main Menu> General Postproc> List Results> Nodal Solution. The List Nodal Solution dialog box appears.

2.In the right scroll box, click on All U's UCOMP to select it, and click on OK.

3.Review the results in the PRNSOL Command window, and click on Close.

digital

Step 12: Exit ANSYS

1.Choose QUIT from the ANSYS Toolbar.

2.Choose the save option you want and click on OK.

yiby

这是ANSYS help里面的一个例子，楼主辛苦了！
但希望以后“顺便”标明例子的出处，以免让大家混淆！

yzh9909324

这是ANSYS help里面的一个例子，楼主辛苦了