abaqus Workshop

1. Workshop 16
Thermal-Stress Analysis of Intersecting Pipes
Introduction
This workshop involves the thermal-stress analysis of a cylindrical pipe intersection. The
pipes are surrounded by a fluid and are filled with another fluid. The interaction between
the pipes and the surrounding fluids are modeled using surface convection. The internal
pressure due to the inner fluid is modeled with a pressure load. Both the thermal and
mechanical responses are sought. The mechanical behavior of the part is expected to
influence the thermal response weakly. Thus a sequential thermal stress analysis is
performed. The thermal analysis model will be developed first and will form the basis of
the structural analysis model. The structural analysis consists of two steps and will
illustrate the use of the restart capability in ABAQUS. The thermal-stress analysis will
also be performed with ABAQUS/Explicit. Only a quarter of the intersection will be
modeled because of symmetry.
Importing and defeaturing the part
1. Start a new session of ABAQUS/CAE from the workshops/heatTransfer
directory.
2. From the main menu bar, select FileImportPart.
3. In the Import Part dialog box, select the file named pipe_int.sat and click
Continue.
4. In the Create Part from ACIS File dialog box, review the basic information
about the geometry and click OK to proceed.
5. The geometry of the model is shown in Figure W16–1.
Figure W16–1. Initial part geometry

2. 6. A quarter-symmetry model will be used in the analysis. From the main menu bar,
select ShapeCut Extrude to create two extruded cuts. For the first cut,
select the face highlighted in Figure W16–2 as the plane for the extruded cut.
Select the vertical edge highlighted in the figure as the edge that will appear
vertical and to the right of the sketch.
Figure W16–2. First extruded cut
7. Sketch the section for the extruded cut as shown in Figure W16–3. In the
viewport, click mouse button 2 to complete the operation and in the prompt area
click Done to proceed. (Mouse button 2 is the middle mouse button on a 3-button
mouse; on a 2-button mouse, press both mouse buttons simultaneously.) In the
Edit Cut Extrusion dialog box, select the direction of cut as shown in Figure
W16–2 and select the end condition Through All.
W16.2
Select this
face
Direction of cut
Edge that will appear vertical
and to the right of the sketch

3. Figure W16–3. Shape of the first cut
8. Repeat steps 6 and 7 for the second cut, as shown in Figures W16–4 and W16–5.
Figure W16–4. Second extruded cut
W16.3
Select this
face
Direction of cut
Edge that will appear vertical
and to the right of the sketch

4. Figure W16–5. Shape of the second extruded cut
9. From the main menu bar, select ToolsRepair. In the Geometry Repair
Tools dialog box, select the Remove faces tool to remove the fillets shown in
Figure W16–6 (you may use the selection filters to facilitate the face selection).
Select the faces highlighted in the figure. Remember to toggle on Local stitch in
the prompt area before completing the operation.
Figure W16–6. Fillets to be removed
10. The fillets will be removed and the adjacent faces are automatically extended by
ABAQUS/CAE to fill the gaps as shown in Figure W16–7. Rename the model
thermal, and save the ABAQUS/CAE model database as pipe-intersection.
W16.4
Remove these faces

5. Figure W16–7. Final part geometry
Properties and model assembly
The units used in this model are SI (kg, m, s, N, °C). The pipes are made of a typical
commercial purity aluminum alloy. The material is assumed to harden isotropically. The
dependence of the flow stress on the temperature is included.
1. Switch to the Property module.
11. From the main menu bar, select MaterialCreate. Name the material
aluminum, and specify the following thermal properties:
· Temperature dependent conductivity:
204 W/m°C at 0°C
225 W/m°C at 300°C
· Specific heat = 880 J/kg°C
· Inelastic heat fraction = 0.0 (for the ABAQUS/Explicit analysis)
· Density = 2700 kg/m3
12. Add the following mechanical properties. (These properties will be used in the
subsequent stress analysis.)
· Modulus of elasticity = 6.9E10 Pa
· Poisson's ratio = 0.33
· Coefficient of thermal expansion = 8.42E-5
· Temperature-dependent plasticity:
Read the data from an ASCII text file. Toggle on Use temperature-
dependent data, as shown in Figure W16–8, and right-click in the data field
indicated in the figure. From the list of available options, select Read from
File. Read the data from the file plasticProps.inp
W16.5

6. Figure W16–8. Reading plastic material properties from a file
13. Create a homogeneous solid section named aluminumSection, and assign it
to the part.
14. Switch to the Assembly module, and create an instance of the part pipe-int.
Analysis procedure and output
To simulate the thermal response of the part, a single heat transfer step will be used.
1. Switch to the Step module.
15. From the main menu bar, select StepCreate. In the Create Step dialog box,
select Heat transfer as the general procedure type and create a transient heat
transfer analysis step using the following parameters:
· Description: Thermal analysis
· Total time period = 200
· Maximum number of increments allowed = 100
· Initial increment size = 1
· End the step when the temperature change rate is less than 0.5
· Maximum allowable temperature change per increment = 10
16. Accept all default ODB output requests. Specify a restart frequency of 5.
Surface film condition
The conditions to model the surface convection will now be applied.
1. Switch to the Interaction module.
17. From the main menu bar, select InteractionCreate. In the Create
Interaction dialog box, select Film condition as the interaction type and click
Continue. Specify a film condition for the outer surface of the pipe shown in
Figure W16–10. Use a film coefficient of 50 W/m2
·s°C and sink temperature of
20°C.
W16.6
Toggle this on
Right click
here

7. Figure W16–10. Surface for outer film condition
18. The fluid temperature on the inner surface is time-dependent. Thus, an amplitude
curve is required to prescribe the temperature history. From the main menu bar,
select ToolsAmplitudeCreate. Accept the default Tabular type, and click
Continue. Enter the film sink temperature amplitude data points (0, 20),
(10, 400), and (200, 400) in the table. Click OK.
19. Create a film condition for the interior surface of the pipe shown in
Figure W16–11. Specify a film coefficient of 1200 W/m2
·s·°C. Enter a value of
1°C for the sink temperature, and use amplitude curve Amp-1 created earlier for
the sink amplitude. The magnitude of the sink temperature will be the product of
the specified value and the amplitude.
W16.7

8. Figure W16–11. Surface for inner film condition
Initial conditions
The pipe is initially at room temperature (20°C).
1. Switch to the Load module.
20. The pipes are initially at a temperature of 20°C. From the main menu bar, select
FieldCreate.
21. In the Create Field dialog box, set the step to Initial, the category to Other, the
type to Temperature, and click Continue.
22. Select the complete model by dragging the mouse across the viewport with the left
mouse button held down. Click Done.
23. In the Edit Field dialog box, enter a value of 20°C for the initial temperature
Magnitude.
Partitioning and meshing the part
You will now generate the finite element mesh. Rather than creating more complicated
partitions for the sake of generating an all-hex mesh, create a series of simple partitions to
subdivide the part instance into hex- and tet-meshable regions. ABAQUS/CAE will
automatically impose the necessary tie constraints between regions of the mesh that are
incompatible.
1. Switch to the Mesh module.
24. From the main menu bar, select ToolsPartition. In the Create Partition
dialog box, select Cell as the partition type and Extend face as the method.
Partition the end region shown in Figure W16–12. Use the face highlighted in the
figure as the face to be extended.
W16.8

9. Figure W16–12. First partition
25. Similarly create a partition for the other end, as shown in Figure W16–13.
Figure W16–13. Second partition
26. Create another partition near the pipe junction using the Define Cutting plane
technique and the Point & Normal method for specifying the partitioning plane.
Select the point highlighted in Figure W16–14 as the point through which the
plane will pass and the highlighted edge as the normal direction.
Extend this face
Extend this face
W16.9

10. Figure W16–14. Third partition
27. Similarly create another partition using the same technique as shown in
Figure W16–15.
Figure W16–15. Fourth (and final) partition
28. From the main menu bar, select MeshControls and assign the Tet element
shape to the region highlighted in Figure W16–16.
Define cutting
plane through
this point
Edge normal to the
cutting plane
Define cutting plane
through this point
Edge normal to the
cutting plane
W16.10

11. Figure W16–16. Region assigned tet elements
29. From the main menu bar, select MeshElement Type and then select the
whole model as the region to be assigned an element type. In the Element Type
dialog box, choose Standard as the element library and Heat Transfer as the
element family. Accept the default element type (DC3D8 elements for hex-
meshable regions and DC3D4 for tet-meshable regions).
30. From the main menu bar, select SeedInstance and assign a global seed size
of 0.05 to the part instance.
31. From the main menu bar, select MeshInstance to generate the part instance
mesh. The message shown in Figure W16–17 appears to indicate that tie
constraints will be automatically generated at the interface between the tet and hex
element regions. Click Continue.
Figure W16–17. Warning message regarding tie constraints
W16.11

12. The meshed part is shown in Figure W16–18.
Figure W16–18. Finite element mesh
Thermal analysis
1. Switch to the Job module.
32. From the main menu bar, select JobCreate, create a job named pipe-
thermal, and click Continue. Accept the default job parameters, and click OK.
33. The nodal temperatures must be written to the results file for them to be read by
the subsequent stress analysis. Currently there is no direct way of requesting this
output using the ABAQUS/CAE menus. The output must be requested using the
Keywords Editor. From the main menu bar, select ModelEdit
Keywordsthermal to open the Keywords Editor. Select the last text block
available (before the *End step option), and click Add After. Enter the
following two lines in the new text block:
*node file
nt,
34. Click OK to close the Keywords Editor.
35. Save the model database.
W16.12

13. 36. Open the Job Manager, and submit the job for analysis.
Postprocessing
1. Once the analysis completes, click Results in the Job Manager.
37. Plot the contours of nodal temperature by selecting the variable NT11 from the
Field Output dialog box. The contour plot is shown in Figure W16–19.
Figure W16–19. Temperature distribution in the pipes
Stress analysis
The stress analysis consists of two steps. In the first step, a pressure load is applied. In the
second step, the thermal load is applied. The complete structural analysis will be
performed using two jobs to illustrate the use of the restart analysis capability.
The thermal analysis model and properties will form the basis of the stress analysis
model. From the main menu bar, select ModelCopy Model and copy the model
named thermal to a new model named stress. From the Model pull down list,
select stress. Make the following changes to this model.
1. Enter the Step module. Delete the Heat Transfer step, and create a Static,
General step with a time period of 10 and an initial time increment size of 1.
38. Create a set named n-hist consisting of the two vertices on the outer and inner
surface of the pipe as shown in Figure W16–20. Request displacement history
output for this set.
W16.13

14. Figure W16–20. Vertices belonging to set n-hist
39. Enter the Load module. Apply a pressure with magnitude 3.50E6 Pa to the
internal surfaces of the pipe.
40. In the Initial step, define symmetry boundary conditions to each symmetry plane
and a pinned condition to the top face as shown in Figure W16–21,
Figure W16–22, and Figure W16–23.
Tip: Set the selection filter type to Face to facilitate the selections.
Figure W16–21. XSYMM faces
Select these two
vertices
W16.14
Select these
faces

15. Figure W16–22. ZSYMM faces
W16.15
Select
these
faces
Boundary condition on this face
represents attachment to a larger
structure.

16. Figure W16–23. PINNED face
41. Enter the Mesh module. Change the element type assigned to the part instance
regions to C3D4 and C3D8I by choosing the 3D Stress element family.
42. From the main menu bar, select ModelEdit Keywordsstress and click
Discard All Edits to delete the two keyword lines added for the temperature file
output in the thermal analysis.
43. Enter the Job module. Create a job named pipe-stress, and run the analysis job.
44. Save the model database.
45. Once the job completes, enter the Visualization module and plot the contours of
stress and displacement. The displacement magnitude contour plot is shown in
Figure W16–24. In this figure the displacement magnification has been set to
1.0.
W16.16
Select this
face

17. Figure W16–24. Contour of displacement magnitude
Restart analysis
The remainder of the stress analysis will now be performed using the restart analysis
capability. Copy the model stress to stress-restart. For the stress-restart, do the
following:
1. Enter the Step module. Create an additional static step for the restart analysis. Set
the step time period to 200 and the initial time increment to 0.2.
46. Modify the history output request for the node set n-hist. In the second analysis
step, add an output request for nodal temperatures.
47. Enter the Load module. Open the Field Manager. For the second analysis step,
edit Field-1 (the initial temperature) so that its status is set to Reset to initial.
This effectively deactivates the field in this step.
48. Create a new field to apply the temperatures obtained in the thermal analysis. In
the Edit Field dialog box, specify the values shown in Figure W16–25.
W16.17

18. Figure W16–25. Reading temperatures from the .fil file
49. From the main menu bar, select ModelEdit Attributesstress-restart to
edit the model attributes for the restart analysis model. Use the parameters shown
in Figure W16–26. Please note that text input to ABAQUS/CAE is case sensitive.
Figure W16–26. Restart analysis model attributes
50. Enter the Job module. Create a job named pipe-stress-restart. Set the
job type to Restart in the Edit Job dialog box.
51. Save the model database, and submit the analysis job.
W16.18

19. 52. When the job completes, plot the Mises stress contours. The plot is shown in
Figure W16–27.
Figure W16–27. Mises stress distribution at the end of the analysis
Coupled thermal-stress analysis with ABAQUS/Explicit
You will now perform the full thermal stress analysis using the explicit dynamics solver.
Even though a fully coupled procedure is used, the thermal response has been uncoupled
from the mechanical response since the inelastic heat fraction has been set to zero. Thus,
in effect a sequential analysis is performed. The steps required to complete this analysis
are described next.
1. Copy the model named stress to a new model named stress-explicit.
53. Enter the Step module. Delete the Static, General step, and create two
Dynamic, Temp-disp, Explicit steps. For the first step use a time period of
10 seconds, while for the second step use a time period of 200 seconds.
54. For each step, apply Semi-automatic mass scaling using a scale factor of
1.0e8.
55. Enter the Interaction module. Create the following surface film conditions in
Step-2:
· For the outer surfaces of the pipes, use a film coefficient of
50 W/m2
·s°C and sink temperature of 20°C.
· For the inner surfaces of the pipes, use a film coefficient of 1200
W/m2
·s·°C. Enter a value of 1 °C for the sink temperature and use
amplitude curve Amp-1 for the sink amplitude.
56. Enter the Load module. Recall that in dynamic analysis procedures, loads are
applied instantaneously. However, in this problem, a quasi-static response is
W16.19

20. sought. In order to promote a quasi-static response, loads must be applied
gradually. For this purpose create a smooth-step amplitude curve. Name the curve
Amp-2; use the points (0,0), (10,1) to define the curve.
57. Apply a pressure load of 3.50E6 Pa in Step-1.Use the amplitude Amp-2 for
the load application.
58. Enter the Mesh module. Change the element library to Explicit, the element
family to Thermally Coupled, and the element type to C3D8RT and C3D4T.
59. Enter the Job module. Create a job named pipe-stress-explicit and submit it
for analysis.
Postprocessing (continued)
1. Plot the contours for Mises stress and PEEQ on the deformed shape for both the
implicit and explicit analyses. The PEEQ contours for both analyses are shown in
Figure W16–28. The results predicted by ABAQUS/Standard and
ABAQUS/Explicit are nearly identical.
Figure W16–28. PEEQ contours at the end of the analysis
(explicit, left; implicit, right)
60. From the main menu bar, select ToolsPathCreate. Choose the Node list
type, and Continue. Click Select, and select the nodes along the edge shown in
Figure W16–29.
W16.20

21. Figure W16–29. Node path
61. From the main menu bar, select ToolXY DataCreate. Select Path from the
Create XY Data dialog box, and click Continue. Examine the various options
in the XY Data from Path dialog box. Click Plot to display the variation of
PEEQ along the path as shown in Figure W16–30.
Figure W16–30. Path plot of PEEQ (explicit analysis)
W16.21
The path starts
here
Select the nodes
on this edge to
define the path