As shown in Figure 1, the pipe is fixed on the ground at one end and
the heat flux is applied on the other end.
A linear steady-state heat conduction solution is defined first. Then it is referred
by a structure solution by TEMP to perform the coupled
thermal/structural analysis. The problem is defined in HyperMesh and solved with OptiStruct implicit solver. The heat transfer and structure
results are post processed in HyperView. Figure 1. Model Review
Launch HyperMesh and Set the OptiStruct User Profile
Launch HyperMesh.
The User Profile dialog opens.
Select OptiStruct and click
OK.
This loads the user profile. It includes the appropriate template, macro
menu, and import reader, paring down the functionality of HyperMesh to what is relevant for generating models for
OptiStruct.
Import the Model
Click File > Import > Solver Deck.
An Import tab is added to your tab menu.
For the File type, select OptiStruct.
Select the Files icon .
A Select OptiStruct file browser
opens.
Select the frame.hm file you saved
to your working directory.
Click Open.
Click Import, then click Close to
close the Import tab.
Set Up the Model
Create Coupled Thermal/Structural Material and Property
Create the material and property collectors before creating the component
collectors.
In the Model Browser, right-click and select Create > Material.
A default MAT1 material displays in the Entity Editor.
For Name, enter steel.
Click the box next to MAT4.
The MAT4 card image appears below
MAT1 in the material information area. The
MAT1 card defines the isotropic structural material.
MAT4 card is for the constant thermal material.
MAT4 uses the same material ID as
MAT1.
If a quantity in brackets does not have a value
below it, it is turned OFF.
To add a value, click the quantity in brackets.
An entry field appears below it.
Click the entry field and enter a value.
Enter the following values for the material, steel, in the Entity Editor.
[E] Young's modulus
2.1 x 1011 Pa
[NU] Poisson's ratio
0.3
[RHO] Material density
7.9 x 103 Kg/m3
[A] Thermal expansion coefficient
1 x 10-5/ °C
[K] Thermal conductivity
73W / (m * °C)
A new coupled thermal/structural material, steel, is created. Figure 2. Material Entity Editor
In the Model Browser, right-click and select Create > Property.
A default PSHELL property displays in the Entity Editor.
For Name, enter solid.
For Material, click Unspecified > Material.
In the Select Material dialog, select
steel and click OK.
Figure 3. Assign the Material steel to the Property solid
For Card Image, select PSOLID from the drop-down menu
and click Yes to confirm.
The property of the solid steel pipe has been created as 3D PSOLID.
Material information is linked to this property.
Link Material and Property to Existing Structure
Once the material and property are defined, they need to be linked to the
structure.
In the Model Browser, click on the
pipe component.
The component template displays in the Entity Editor.
For Property, click Unspecified > Property.
In the Select Property dialog, select
solid and click
OK.
Figure 4. Assign the Property solid to the Component
pipe
Apply Thermal Loads and Boundary Conditions to the Model
A structural constraint spc_struct is applied on the RBE2
element to fix the pipe on the ground. Two empty load collectors,
spc_heat and heat_flux have been
pre-created. In this section, the thermal boundary conditions and heat flux are
applied on the model and saved in spc_heat and
heat_flux, respectively.
Create Thermal Constraints
Click the Set Current Load Collector panel located at
the right corner of the footer bar, as shown below.
A list of load collectors appears. Figure 5. Setting the Current Load Collector
Select spc_heat as the current load collector.
From the Analysis page, click constraints.
Go to the create subpanel.
Click the entity selection switch and select nodes from
the pop-up menu.
Click nodes > by sets.
Select the predefined entity set heat and click
select.
The selected nodes on the fixed end should be highlighted.
Uncheck the boxes in front of dof1,
dof2, dof3,
dof4, dof5, and
dof6 and enter 0.0 in the
entry fields.
Click load types = and select SPC
from the pop-up list.
Click create.
This applies these thermal constraints to the selected nodal
set.
Click return to go to the Analysis page.
Create CHBDYE Surface Elements
The heat flux will be applied on the surface of the free end of the pipe. Therefore, the
surface elements CHBDYE for defining heat transfer boundaries must be
created first.
Click BCs > Create > Interfaces.
For Name, enter heat_surf.
For Card Image, select CONDUCTION from the drop-down
menu.
Select an appropriate color from the palette.
For Secondary Entity IDs, click Elements.
The Secondary Entity IDs panel is now displayed below the Graphics
Browser.
Click the switch button for elems and select
faces from the pop-up list.
Click the highlighted solid elems and select
by sets from the pop-up selection menu.
Select element set solid elems and click
select.
Click nodes in the face nodes field.
Select four nodes on one face of a solid element where the heat flux is
applied, as shown in Figure 6.
Figure 6. Nodes on the Surface Element
Click add.
This adds the CHBDYE surface elements on all the solid elements
following the same side convention, as shown in Figure 7. Figure 7. CHBDYE Surface Elements
Click return to return to the Entity Editor.
Click Close.
Create Heat Flux on Surface Elements
In this step, the uniform heat flux into CHBDYE elements is defined with QBDY1
entries.
Set your current load collector to heat_flux.
From the Analysis page, click flux to enter the Flux
panel.
Go to the create subpanel.
Click elems > by group.
Select heat_surf and click
select.
The surface elements are highlighted.
Click load types= and select
QBDY1.
In the value= field, enter 1.0.
Click create.
The uniform heat flux in the surface elements is defined.
Click return to go back to Analysis page.
Create Heat Transfer Load Step
An OptiStruct steady-state heat conduction loadstep is created,
which references the thermal boundary conditions in the load collector spc_heat and the
heat flux in the load collector heat_flux. The gradient, flux, and temperature output
for the heat transfer analysis are also requested in the load step.
In the Model Browser, right-click and select Create > Load Step.
A default load step displays in the Entity Editor.
For Name, enter heat_transfer.
Click the drop-down menu in the Value field next to
Analysis type in the Entity Editor and select
Heat transfer (steady-state).
For SPC, click Unspecified > Loadcol.
In the Select Loadcol dialog, select
spc_heat and click OK.
Figure 8. Select the Constraints
For LOAD, click Unspecified > Loadcol.
In the Select Loadcol dialog, select heat_flux and click
OK.
Verify that the Analysis type is set to HEAT.
Check the box next to OUTPUT.
Activate the options of FLUX and
THERMAL on the sub-list.
Under each result selection, click the space next to FORMAT and select
H3D format from the drop-down menu. For THERMAL,
click the Table icon and select
H3D from the drop-down menu in the table that
opens.
Click the button under OPTION and select ALL, as shown
in Figure 9.
Flux and Thermal output can also be requested in the Control Cards panel on
the Analysis page. Figure 9. Setting up the Heat Transfer Loadstep
Create a Structure Load Step
To perform a coupled thermal/structural analysis, the heat transfer SUBCASE needs to be
referenced by a structural SUBCASE through TEMP card. Since this is not
directly supported in HyperMesh, a linear static
structural subcase is created and temperature is added using
SUBCASE_UNSUPPORTED or by editing the .fem file after
the model export.
In the Model Browser, right-click and
select Create > Load Step.
A default load step displays in the Entity Editor.
For Name, enter structure_temp.
Click on the drop-down menu in the Value field next to Analysis
type in the Entity Editor and select
Linear Static.
For SPC, click Unspecified > Loadcol.
In the Select Loadcol dialog, select
spc_struct and click
OK.
Check the box next to SUBCASE_UNSUPPORTED.
Click the Table icon to the right of Data: Comments
and enter the following text in the first row of the pop-out
table.
TEMP=1
Note: The TEMP ID used above could be
different from your model. Make sure the ID of the
heat transfer subcase is selected for
TEMP.
Click Close.
Submit the Job
From the Analysis page, click the OptiStruct
panel.
Figure 10. Accessing the OptiStruct Panel
Click save as.
In the Save As dialog, specify location to write the
OptiStruct model file and enter
pipe_complete for filename.
For OptiStruct input decks,
.fem is the recommended extension.
Click Save.
The input file field displays the filename and location specified in the
Save As dialog.
Set the export options toggle to all.
Set the run options toggle to analysis.
Set the memory options toggle to memory default.
Click OptiStruct to launch
the OptiStruct job.
If the job is successful, new results files
should be in the directory where the pipe_complete.fem was written. The pipe_complete.out file is a good place to look for error messages that could help
debug the input deck if any errors are present.
View the Results
View Heat Transfer Analysis Results
From the OptiStruct panel, click HyperView.
HyperView is launched and the results are
loaded. A message window appears to inform of the successful model and result
files loading into HyperView.
Click Close to close the message window, if one
appears.
On the Results toolbar, click to open the
Contour panel.
Select Subcase 1 - heat transfer as the current load
case in the Results tab, as shown below.
Figure 11. Results tab in HyperView
In the Contour panel, select the first pull-down menu below
Result type and select Element Fluxes (V).
Click Apply.
A contoured image representing thermal
fluxes should be visible.
Select the first pull-down menu below Result
type and select Grid Temperatures
(s).
Click Apply.
Both flux and temperature results are
shown below. Figure 12. Results of Heat Transfer Analysis
View the Results for the Coupled Thermal/Structure Analysis
Select the structure analysis subcase as the current load case in the Load Case and Simulation Selection window.
Select the first pull-down menu below Result type and select Element
Stresses [2D & 3D] (t).
Select the second pull-down menu below Result type and select
vonMises.
Click Apply.
A contoured image representing von Mises stresses should be visible.
Each element in the model is assigned a legend color, indicating the von Mises
stress value for that element, resulting from the applied loads and boundary
conditions.
Select the first pull-down menu below Result type and select
Displacement (v).
Select the second pull-down menu below Result type and select
Mag.
Click Apply.
Both stress and displacement contours are shown below. Figure 13. Results of the structural analysis