Thermal Stresses of Tanks

This page is a continuation of the thermal analysis performed in Examples: Steady State Heat Transfer: Temperature of a Tank. Complete that exercise before starting this one.

Once the temperature distribution is obtained, the expansion induced by the temperatures can be calculated. The general procedure is:

Linear Static Analysis Procedure:

  1. Return to the FEA Editor.
  2. The new design scenario and analysis type can be created in one step: right-click the Analysis Type heading at the top of the tree view and select Set Current Analysis Type Linear Static Stress with Linear Material Models. Click Yes when given the option to create a new design scenario.
  3. Select the new design scenario's name(2<Heat Transfer Analysis>) and click F2 to edit the name. Change it to Static Stress.
  4. Enter the Element Definitions. Since all three parts have the same data, they can be entered simultaneously.
    1. Select the Element Definition for part 1 in the tree view.
    2. Hold the Ctrl key and select the Element Definition for parts 2 and 3.
    3. Right-click one of the entries and select Edit Element Definition.
    4. Type the Thickness of 0.25 inch.
    5. Type the Normal Point (Y) of 33. This will apply the hydrostatic pressure to the inside of the tank. (Any coordinate inside the tank will work. Technically, the normal point only needs to be set for part 2. In this model, there is no problem with setting it for the other parts as well.)
    6. Type the Stress free reference temperature of 70 °F.
    7. Click OK.
  5. Select one of the Material entries in the tree view (or select all three), right-click, and select Edit Materials. The Thermal Coefficient of Expansion has a value, so click Cancel to close the screen.
  6. The boundary conditions will be added in three stages: symmetry boundary conditions, fixed boundary conditions around the bolt hole in the support plates, and vertical boundary conditions on the support plates.
    1. View the model from the top (View Navigate Orientation Top View).
    2. Use point selection (Selection Shape Point or Rectangle) to select the surfaces (Selection Select Surface) along the left edge of the model. The edge of the tank (part 2 surface 6) and support plate (part 1 surface 6) both need to be selected (hold the Ctrl key after selecting the first edge).
    3. Right-click and select Select Subentities Vertices to get just the nodes. (Applying a load to a plate applies the load to the entire element.)
    4. Right-click and select Add Nodal Boundary Conditions. Click the X Symmetry since the X axis is perpendicular to the face. Click OK to apply the boundary conditions.
    5. Repeat for the top edge of the model, selecting the tank (part 2 surface 4) and support plate (part 1 surface 4). Apply Y Symmetry boundary conditions since the Y axis is perpendicular to the face.
    6. Use the surface selection (Selection Select Surface) and select the edge of the bolt hole (part 1, surface 3). Since the bolt holes in both support plates are on the same part/surface, only one needs to be picked to select both. (It may be necessary to zoom in on the support plate to click the edge of the hole.)
    7. Right-click and select Select Subentities Vertices to get just the nodes.
    8. Right-click and select Add Nodal Boundary Conditions. Click No Translation. Click OK to apply the boundary conditions.
    9. Use the surface selection(Selection Select Surface) and select the support plate (part 1, surface 7).
    10. Right-click and select Add Surface Boundary Conditions. Click the Tz box to simulate the contact with the top of the pier. Click OK to apply the boundary conditions.
  7. Apply the hydrostatic load to the tank as follows:
    1. Change to an isometric view: View Navigate Orientation Isometric View.
    2. Use the surface selection (Selection Select Surface) and select the tank anywhere below the water level (part 2, surface 10).
    3. Right-click and select Add Surface Hydrostatic Pressure.
    4. Click the Point Selector to specify the Point on Fluid Surface Pressure on node at the top of surface 10, at the water level. The important coordinate is the Z coordinate. It is 16.63 inch.
    5. The Surface Normal of the Fluid indicates the direction of gravity. Enter a value of -1 for the Z direction.
    6. Enter the Fluid Density of water as 0.0361 lbf/in3.
    7. Click OK to apply the pressure.
  8. The temperatures from the heat transfer model are applied to the stress model under the Analysis Parameters. This is also where the pressure load cases and gravity are specified.
    1. Use the Setup Model Setup Parameters command.
    2. For this analysis, use three load cases to see the effects due to the hydrostatic pressure by itself, temperature by itself, and both loads. (This simulates the cooled condition, the tank immediately after emptying, and the normal operating condition.) Naturally, gravity occurs during all three of these conditions. So, enter the Load Case Multipliers on the Multipliers tab as shown in the following table.
      Index Pressure Accel/Gravity Rotation Angular Accel Boundary Thermal Voltage
      1 1 1 0 0 0 0 0
      2 0 1 0 0 0 1 0
      3 1 1 0 0 0 1 0
    3. Click the Gravity/Acceleration tab to set up the gravity. Click the Set for standard gravity to set the Acceleration due to body force. The direction should be the default of Z multiplier -1.
    4. Click the Thermal/Electrical tab to set up the temperatures. Set the Source of nodal temperatures to Steady-state analysis. Click Browse and browse to the folder containing the model, then to the tank model.ds_data folder, then to the 1 folder where the results from design scenario 1 are stored. Select the file ds.to and click Open.
    5. Click OK to close the Analysis Parameters dialog box. When prompted that a multiplier must be assigned for the thermal effects to be applied to the model, select No. The prompt is referring to the 0 Thermal multiplier for load case 1, and the setup (shown previously) is intentional.
  9. Run the analysis: Analysis Analysis Run Simulation. (Since the analysis is very fast, the Check Model, to check the input before running the analysis, will not be done.)
  10. Once the analysis completes, review the input for accuracy. For this model, the main input to check are:
    1. Pressure in the proper direction: If necessary, activate the loads and constraints from the toolbar. The pressure arrows should increase in length towards the bottom of the tank, and all of the arrows should be pointing outward.
    2. Temperature loaded: Use Results Contours Other Results Applied Loads Temperature to display the temperatures in the stress analysis. The pattern should be identical to the steady-state heat transfer results.
    3. Boundary conditions: The boundary conditions can either be checked individually or as a whole. Since we have the results, it is quicker to check whether the behavior is correct without necessarily checking each one individually.
      1. Deactivate the loads and constraints from the toolbar.
      2. Go to Results Contours Displacement Show Displaced Displaced Options .
      3. Activate the Show Displaced Model option.
      4. Activate the Mesh option to show the undisplaced model.
      5. Move the slider back and forth to exaggerate the displaced shape. If the boundary conditions are correct, then (a) only the tank-end of the support pads will deflect, (b) the nodes on the YZ plane will remain in that plane due to symmetry, and (c) the nodes on the XZ plane will remain on that plane due to symmetry.
  11. When satisfied that the boundary conditions are okay, set the Scale Factor to 5 and close the dialog box.

Review the von Mises results (Results Contours Stress von Mises)and displacement results (Results Contours Displacement Displacement Magnitude ) of all three load cases (Results Contours Load Case Options Next). The maximum results are summarized in the table below.

Load Case Condition Maximum von Mises Stress Maximum Displacement Magnitude
1 Pressure and gravity 5600 psi 0.0249 inch
2 Temperature and gravity 21400 psi 0.0330 inch
3 Pressure, temperature, and gravity 19600 psi 0.0334 inch

Other Ideas:

Transient Heat Transfer and Linear Static Stress:

If a transient heat transfer analysis had been performed instead of a steady state heat transfer, the steps to perform the linear static stress would be the same as outlined above except for the step when choosing the Source of nodal temperatures. Naturally, this would be set to Transient analysis. Then, since linear stress uses just one temperature profile from the transient heat transfer analysis for all load cases in the stress analysis, use the Time step drop-down menus to indicate which time step to use.

Steady-State heat Transfer and Mechanical Event Simulation (MES):

The steps to perform a thermal stress analysis with the nonlinear/MES analysis instead of linear static stress are very similar. The differences are as follows:

  1. In the Element Definition, select a Material model that includes thermal effects, such as Thermoelastic. Otherwise, the parts experience no thermal expansion (as would be noticed by viewing the material properties: there would be no coefficient of expansion).
  2. In the Analysis Parameters, the Thermal/Electrical tab is used to specify the source of temperatures, just like the linear analysis. The difference with nonlinear/MES is that the temperatures from a steady-state heat transfer analysis can be adjusted over the duration of the analysis by the assigned load curve. All temperatures T from the steady-state heat transfer analysis are multiplied by the value entered for the load curve multiplier LCM. Second, the expansion is based on the difference between these temperatures (TxLCM) and the entered stress free reference temperature. So it is usually impractical to use a load curve to ramp the temperatures from the stress-free condition to the operating condition. Assigning the temperatures to a load curve that is set to a constant value of 1 applies the entire thermal load at the start of the analysis and may cause convergence difficulties. Of course, it may be possible to use a load curve multiplier for the beginning of the analysis that starts all of the temperatures closer to the stress free reference temperature, and thereby reduces the convergences difficulties that would result from applying the full load.

If the stress results are dependent on the loading path, it may be better to use a transient heat transfer analysis instead of a steady-state heat transfer analysis.

Transient Heat Transfer and Mechanical Event Simulation (MES):

Using the results from a transient heat transfer analysis in a nonlinear/MES stress analysis is similar to the procedure for a steady state heat transfer analysis as described above. The only difference is related to the load curve. As explained above, the temperatures from the steady-state analysis are multiplied by the load curve multiplier, which then defines how the temperatures change over time. Since transient heat transfer already has results over time, the temperatures from the transient heat transfer analysis are not assigned to a load curve. Instead, nonlinear/MES matches the time of each transient heat transfer result to the time-steps of the stress analysis. If a time-step in the stress analysis does not have a corresponding time in the heat transfer analysis, the temperature results are interpolated.

Parent topic: Linear and Dynamic Stress