abaqus Workshop

1. Workshop 7
Step Definition and Loads: Pipe Creep Model
Defining steps and specifying output requests
You will now define the analysis steps. For this simulation you will define two static,
general steps. In the first step a pressure load is applied; in the second step a transient
analysis is carried out to determine the creep of the pressurized vessel.
In addition, you will specify output requests for your analysis. Moreover, since
interactions, loads, and boundary conditions can be step dependent, analysis steps must be
defined before these can be specified.
To begin this workshop, start a new session of ABAQUS/CAE from the
workshops/pipeCreep directory. Open the database containing the pipe creep
model.
To define a step:
1. From the Module list located under the toolbar, select Step to enter the Step
module.
2. From the main menu bar, select StepCreate to create an analysis step. In the
Create Step dialog box that appears, name the step Pressure and accept the
General procedure type. From the list of available procedure options, accept
Static, General. Click Continue.
3. In the Edit Step dialog box that appears, enter the following step description:
Apply internal pressure. Accept the default settings, and click OK.
4. From the main menu bar, select StepCreate to create another analysis step.
Insert the new step after the one created earlier. In the Create Step dialog box
that appears, name the step Creep and accept the General procedure type. From
the list of available procedure options, select Visco. Click Continue.
5. In the Edit Step dialog box that appears, enter the following step description:
Transient creep. Set the time period for the step to 4.38E5 hours
(approximately 50 years). Use initial and minimum time increments of 1.0 hour
and a maximum time increment of 4.38E5 hours. Set the tolerance for the
maximum difference in the creep strain increment (CETOL) to 1.0E5 and the
maximum number of increments to 1000.
Since you will use ABAQUS/Viewer to postprocess the results, you must specify the
output data you wish to have written to the output database (.odb) file. Default
history and field output requests are selected automatically by ABAQUS/CAE for
each procedure type. This output is sufficient for the first step (Pressure). For the
second step (Creep), however, we require only the following output:
· The displacements, stresses, and creep strains (written as field data to the output
database file every 2 increments).

2. · The displacements for the point shown in Figure W7–1 (written as history data every
two increments).
Figure W7–1. Region for restricted output
The history output request requires a set to be defined. Follow the steps outlined
below to define a set and request output.
To define a set:
1. From the main menu bar, select ToolsSetCreate. In the Create Set dialog
box, name the set Out and click Continue.
6. Select the point indicated in Figure W7–1.
7. Click Done in the prompt area when the appropriate region is highlighted in the
viewport.
To specify output requests to the output database file:
1. From the main menu bar, select OutputField Output Requests
Manager. In the Field Output Requests Manager, select the cell labeled
Propagated in the column labeled Creep. The information at the bottom of the
dialog box indicates that preselected default field output requests have been made
for this step.
W7.2
set Out

3. 8. On the right side of the dialog box, click Edit to change the field output requests.
In the Edit Field Output Request dialog box that appears:
A. Click the arrow next to Stresses to show the list of available stress output.
Accept the default selection of stress components and invariants.
B. Click the arrow next to Strains to show the list of available strain output.
Toggle off PE, PEEQ, and PEMAG.
C. Toggle off Forces/Reactions and Contact.
D. Accept the default Displacement/Velocity/Acceleration output.
E. Save the output every 2 increments.
F. Click OK.
G. Click Dismiss to close the Field Output Requests Manager.
9. Modify the history output by selecting OutputHistory Output
RequestsManager. In the History Output Requests Manager, select
the cell labeled Created in the column labeled Pressure if it is not already
selected. On the right side of the dialog box, click Edit.
A. Toggle on Set name as the domain and, from the list of available sets,
choose Out.
H. Toggle off Energy in the Output Variables region.
I. Select the displacement components (U under Displacement/Velocity/
Acceleration).
J. Save the output every 2 increments.
K. Click OK.
L. Click Dismiss to close the History Output Requests Manager.
Prescribing boundary conditions and applied loads
Symmetry conditions must be applied to the two symmetry planes in the model. In
addition, a single point must be restrained in the vertical direction to prevent rigid body
motion.
Both the pipe and the pressure vessel are assumed to be operating under an internal
pressure of 1.4E7 Pa. In addition, the pipe and pressure vessel are subject to end cap load
conditions. This implies that for any cut through the model, the equivalent load due to the
pressure on the cap can be applied as traction loads on the cut section. Hand calculations
provide that the equivalent traction loads are: 8.281E6 Pa for the pressure vessel and
7.682E6 Pa for the pipe. Furthermore, depending on the proximity of the cuts to the
critical stress region, the boundary conditions could include multipoint constraints that
would require that plane cut sections remain plane. For this exercise we will assume that
the cuts are made a sufficient distance from the area of interest, and this last requirement
will be ignored.
The pipe is at a uniform initial temperature of 540º
C.
To prescribe boundary conditions:
1. From the Module list located under the toolbar, select Load to enter the Load
module.
W7.3

4. 10. From the main menu bar, select BCCreate to prescribe boundary conditions
on the model. In the Create Boundary Condition dialog box that appears,
name the boundary condition X-SYMM and select Initial as the step in which it
will be applied. Accept Mechanical as the category and Symmetry/
Antisymmetry/Encastre as the type. Click Continue.
You may need to rotate the view to facilitate your selection in the following steps.
11. Select ViewRotate from the main menu bar (or use the tool from the
toolbar), and drag the cursor over the virtual trackball in the viewport. The view
rotates interactively; try dragging the cursor inside and outside the virtual
trackball to see the difference in behavior.
12. Select the regions of the model indicated in Figure W7–2 using [Shift]+Click.
Click Done in the prompt area when the appropriate regions are highlighted in
the viewport, and toggle on XSYMM in the Edit Boundary Condition dialog
box that appears. Click OK to apply the boundary condition.
Figure W7–2. XSYMM boundary condition region
Arrows appear on the face indicating the constrained degrees of freedom. The
XSYMM boundary condition constrains the degrees of freedom necessary to
impose symmetry about a plane X = constant; after the part is meshed and the job
is created, this constraint will be applied to all the nodes that occupy the region.
W7.4
XSYMM regions

5. 13. Repeat steps 2 through 4 to apply a ZSYMM boundary condition to the region
shown in Figure W7–3. Name the boundary condition Z-SYMM.
Figure W7–3. ZSYMM boundary condition region
To satisfy the end cap condition on the intersecting pipe, apply a displacement constraint
normal to the entire face of the free end of the pipe. This action will constrain the model
against rigid body motion, and the equivalent traction loads will be generated as reaction
forces.
14. From the main menu bar, select BCCreate. In the Create Boundary
Condition dialog box that appears, name the boundary condition EndCap, and
select Initial as the step in which it will be applied. Accept Mechanical as the
category and select Displacement/Rotation as the type. Click Continue.
15. Select the region of the model indicated in Figure W7–4 using the cursor. Click
Done in the prompt area when the appropriate region is highlighted in the
viewport, and toggle on U2 in the Edit Boundary Condition dialog box that
appears. Click OK to apply the boundary condition.
W7.5
ZSYMM region

6. Figure W7–4. U2 boundary condition region
To apply a pressure load:
1. From the main menu bar, select LoadCreate to prescribe the internal pressure
load. In the Create Load dialog box that appears, name the load Internal
Pressure and select Pressure as the step in which it will be applied. Accept
Mechanical as the category, and select Pressure as the type. Click Continue.
16. Select the surfaces associated with the interior of the pipe and pressure vessel
using the cursor; the region is highlighted in Figure W7–5. When the appropriate
surfaces are selected, click Done in the prompt area.
W7.6
Fix U2 at top of pipe

7. Figure W7–5. Surface to which internal pressure will be applied
17. Specify a uniform pressure of 1.4E7 in the Edit Load dialog box, and click OK
to apply the load.
Arrows appear on the model faces indicating the applied load.
Next, apply a pressure load to impose the end cap condition on the pressure
vessel.
18. Repeat steps 1 through 3 above to apply a pressure of 8.281E6 Pa to the region
highlighted in Figure W7–6. Name the load Vessel End Cap.
W7.7
inner surface

8. Figure W7–6. Surface to which end cap pressure will be applied
To apply an initial temperature:
1. From the main menu bar, select FieldCreate to prescribe the initial
temperature. In the Create Field dialog box that appears, name the field
InitialTemp and select Initial as the step in which it will be applied. Select
Other as the category and Temperature as the type. Click Continue.
19. Select the entire model as the region to which the field will be applied.
20. Click Done in the prompt area when the appropriate region is highlighted in the
viewport.
21. Specify a uniform temperature of 540º
C in the Edit Field dialog box, and click
OK to apply the field.
22. Save your model database, and exit your ABAQUS/CAE session.
W7.8
Apply end cap pressure to
this surface