MET 425 - FEA Applications II
Prof. Dave Johnson, psuprofdj@psu.edu
Penn State - Erie, The Behrend College
HW-6: prep for final
project
Concepts:
- 2D approximation of a portion of a much more
complex structure
|
|
|
|
The figures above from http://www.nrc.gov/reactors/operating/ops-experience/vessel-head-degradation/images.html
show a typical nuclear reactor. The control rods are raised and lowered
through many nozzle-shaped ports on the reactor head. Although there are
many of these nozzles on the reactor head, it is common to analyze one in a
two-dimensional, axisymmetric analysis.
Background: Davis Besse is a
reactor in northern Ohio on the southwest shore of Lake Erie. A
corrosion problem was detected in 2002 at the nozzle-reactor head
fillet. This fillet location is also a location of high stress and a
weakening of the head in this location might have leaked/flooded the
containment building with coolant from the reactor. Repairs required two
years.
A typical nozzle-reactor head joint is
the focus of this analysis project. We can develop a 2D model of the
region of interest. You may click here to access the ParaSolid
File [Use a Right-click on this link, then "Save Target
As...", then "Save as type: All Files", and use a file name
like: "fea2_pwr_Geom2D.x_t" ]
|
Dimensions:
- A7 = 7.5o
- Nozzle Outside Radius,
H4 = 2 in.
- Nozzle Wall Thickness,
H8 = 0.625 in.
- Head Inside Radius,
R5 = 77.53 in.
- Head Outside Radius,
R6 = 83.53 in.
- Nozzle Length,
V10 = 12 in.
Weld Dimensions:
- Width of Weld Notch,
H13 = 0.47 in.
- V9 = 1 in.
- V11 = 0.47 in
- V12 = 0.235 in
- V14 = 0.94 in.
|
Edit the Geometry with
DesignModeler and "Form New Part" from the TWO bodies representing
the nozzle and the weld.
The spherical head material is SA-508, Grade 3 and the nozzle and
weld are SA-813 Type 304
The ASME Code
(Section II, Part D) give material properties vs. temperature (density is
constant for both materials).
For this
assignment, enter only the structural material data (not the thermal
properties) and enter only the 100 F data set for each material.
For thermal-stress analysis, the Reference
Temperature is 100 F.
The simulation specification for this analysis
requires that the connection between the nozzle and the head be
"detached." In order to achieve this requirement, suppress the
automatic contact region that is created between these bodies.
Run a static structural analysis to validate the model. Use Uniform
Temperature of 100 F, Reference Temperature of 100F, and the highest internal
pressure load 2572 psi (applied to five inside edges) and highest blow-off load of 15277 lbf (applied to the top edge of the nozzle). Use a small deflection, linear analysis for
validation to hand calcs.
Confirm the model with hand calcs (before you waste time solving the long
transient simulation on an incorrect model).
Determine an appropriate mesh to achieve
acceptable mesh error in a model which may run for many loadsteps and substeps.
Turn in:
- A plot showing the mesh - document the
no. of nodes and elements and the element type used.
[Hint: this model will be used later
for an analysis with many load steps. Keeping the mesh small, but
accurate is important. Try to keep no. of nodes < 10,000]
- An
environment plot that shows ALL applied boundary conditions
- a plot showing the total
deformation of the assembly
- a plot showing the highest equiv. stress on the part
- any
other plot(s) needed to justify
the mesh error like SERR, deformed shape with SEPC, etc. [SEPC <
5% IN EACH BODY]
- appropriate normal stress plots, scoped to specific
bodies (or edges) - use a "Probe" placed far from known stress
concentrations, to compare to hand calc results:
- hand calcs of the hoop stress in the spherical pressure
vessel (thick-walled or thin-walled ?) compared to the proper FEA
results plot
- hand calcs of the hoop stress in the nozzle
(thick-walled or thin-walled ?) compared to the proper FEA
results plot
- hand calcs of the axial stress in the nozzle
(thick-walled or thin-walled ?) compared to the proper FEA
results plot