MET 425 - FEA Applications II

Prof. Dave Johnson, psuprofdj@psu.edu
Penn State - Erie, The Behrend College

Final Project:  ASME Code and FEA Analysis

Concepts: Transient Thermal Analysis Thermal-Stress Analysis Nonlinear material behavior Linearized Stress Results Exposure to ASME Code checks

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 a nozzle-shaped port 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.  Stresses need to be evaluated through specific locations in the nozzle wall using a linearized-stress method.

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 closure 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 thermal-stress analysis, the Reference Temperature is 120 F.

Load Data:

For the thermal transient analysis, all inside surfaces (shown with the 2573 pressure load, above) are exposed to a convection load.  The film coefficient is constant, H = 500 BTU/(hr-ft²-^oF), and the Fluid Temperature is given in the load table.

For BOTH the thermal transient analysis and the static structural analysis, the Initial Temperature is 120 F.

Transient Thermal Load STEP Data for Time Integration and Output Controls:

Since ANSYS ONLY reads in temperature data for each LOAD STEP (it does NOT interpolate temperature data from the thermal analysis for intermediate SUBSTEPS), we will set up 32 load steps to attempt to capture critical time points during the static structural analysis.  Each load step will require only one substep since we are using linear material properties for this simulation.

Static Structural Load STEP Data and Output Controls:

(NOTE: Red times/loads are interpolated from the given load history)  This data is provided in a a tab-delimited text file: fea2_pwr-static_struct_load_steps.txt

Once the load steps have been set up, make sure the "Imported Body Temperature" table shows the correct "Source Time" for each static structural analysis load step.  It should look like this:

The ASME Code gives design stress intensity information for the material used for this analysis:

The simulation specification for this analysis requires the boundary between the nozzle and head be connected for the transient thermal analysis, but for the thermal stress model, this boundary condition is to be detached. In WB 12, we are not permitted to change contact behavior between linked analyses.  So, a command object can be placed BEFORE Solution to "kill" a specific pair of bonded contacts.  NOTE: this operation assumes the contact/target pairs between the nozzle and head are identified as element types 4 and 5.  CONFIRM that this works for your model.

ESEL,S,TYPE,,4,5 ! Select the contact-target elem btw. nozzle and head
EKILL,ALL        ! Kill those elements (structural analysis, only)
ESEL,ALL         ! Select all elements

First (done in HW-6): Run a static structural analysis to validate the model.  Use Uniform Temperature of 120 F, Reference Temperature of 120F, and the highest internal pressure load 2572 psi and highest blow-off load of 15277 lbf.  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.
Add an evaluation of linearized stress intensity* through the nozzle wall at the top of the weld.

Run the thermal transient & static structural (thermal stress) analyses.  
Start with the HW-6 Project Schematic.  Create a “thermal transient” object linked to the HW-6 Geometry.  Then, create a “static structural” object linked to the thermal transient “Results”.  Save As …. (Use a new name for the final project).  Create the same mesh for the new models that was used in HW-6.
Evaluate the stress intensity through the nozzle wall at the top of the weld using linearized stress calculations.  Evaluate the results with respect to the ASME code.

Turn in an engineering analysis report:

• (10%) Cover page with executive summary (analysis objective and summary of findings)
• (10%) Introduction (FEA model assumptions and decisions [modeling approach, material behavior, etc.], procedure, etc.)
• (50%) Results presented, including 
  • first run: model, mesh, loads and constraints, and linearized stress intensity graph and table; 
  • thermal transient: loads and constraints, and temperature histories (max and min temperatures); 
  • static structural: loads and constraints, stress intensity history, linearized stress intensity graph and table at the appropriate time during the transient
• (20%) Conclusions, evaluation with respect to appropriate sections of ASME code (incl. references)
  • report: 
    • average section (path) temperature at times of highest total stress intensity, 
    • values for Sm (Sm depends on the material and temperature), 
    • per ASME Code Section III, NB 3221 evaluate P_membrane [from first static analysis],
    • per ASME Code Section III, NB 3221 evaluate P_{membrane + bending} [from first static analysis],
    • per ASME Code Section III, NB 3222 / NB-3223 evaluate (P + Q)_total RANGE @ highest total stress times. [Assume minimum SINT = 0.  So, Range of SINT = maximum Total SINT]
• (10%) Appendices for 
  • given data summary (material data, geometry, loading, loat steps, etc.), 
  • hand calcs of validation model (appropriate normal stress plots, mesh error, comparison to hand calcs), 
  • hand calcs to support integration time step for thermal transient analysis (compare to given ITS),
  • etc.

*Note: To evaluate the linearized stress intensity:

At the top of the “Model Tree,” Add “Construction Geometry” and insert a “Path”
Define the start and end of the path (seems best to use x, y coordinates to position the path through the wall at the elevation of the top of the weld.
Under “Solution,” insert a “Linearized Stress” Intensity object, change the scope to reference the path you created and set the 2D Behavior as “Axisymmetric, straight”
For the thermal-tress analysis, we would also set the appropriate value of “Time” to represent the condition when the highest value of stress intensity is observed.