As engineers design subsea piping they must ensure it will survive the harsh conditions found underwater. Therefore, it is important to use simulation software, standards and best practices to assess these designs.
Finite element analysis (FEA) is a simulation tool that can prove that your duplex steel tee junction meets the pressure vessel code.
The assessment of subsea piping is done in accordance with the Submarine Pipeline Systems standards of Det Norske Veritas and Germanischer Lloyd (DNV GL), and the Alternative Rules for Construction of Pressure Vessels by the American Society of Mechanical Engineers (ASME).
Typically, there are four pressure tests you need to worry about when assessing your tee junction:
- Factory acceptance test (FAT).
- Installation test (laydown test).
- Leakage test (offshore test).
- Operation test (in-place test).
For FAT, each component is tested by itself using pressure caps. All the other tests require a systems simulation, so engineers can determine the loads that each part experiences. For simplicity’s sake, this blog will focus on the FAT test.
Design Criteria of an Subsea Tee Junction
ASME notes that there are four typical failure modes for pressure vessel components:
- Failure due to plastic collapse.
- Failure due to local yielding (local failure).
- Failure due to buckling.
- Failure due to cyclic loading.
When performing FAT, our focus will be on plastic collapse and local failure.
ASME defines the load combinations engineers need to use for simulation. For the design to pass the FAT, the detailed stress results must not exceed the allowable stresses/strains governed by the code.
The blog will test plastic collapse using elastic stress analysis and elastic-plastic stress analysis.
As for testing local failure, ASME also provides two alternative analysis methods: elastic analysis and elastic-plastic analysis.
FAT doesn’t require you to perform all possible analysis methods to pass — only two. This means that there are four different analysis combinations an engineer can use to complete a FAT check. These combinations are listed in Table 1.
Table 1. Possible test combinations needed to determine if a part passes a FAT check
|Combinations||Plastic Collapse||Local Failure|
|1||Elastic Stress Analysis||Elastic Analysis|
|2||Elastic Stress Analysis||Elastic-Plastic Analysis|
|3||Elastic-Plastic Stress Analysis||Elastic Analysis|
|4||Elastic-Plastic Stress Analysis||Elastic-Plastic Analysis|
Your design needs to meet the requirements of both tests listed in your chosen combination to pass the FAT.
How to Model and Simulate an Subsea Piping Tee Junction
The simulation of a subsea piping tee junction starts with a good hexahedral mesh. The objective of this mesh is to get stress results that are detailed enough to be linearized.
The ANSYS simulation platform offers a shared topology tool that can simplify the meshing of the part. Using ANSYS Discovery SpaceClaim, engineers can cut the volume into multiple pieces and then regroup them as a multibody part. This can be seen in the video below:
This procedure makes it possible for finite element nodes to be shared between volumes. Discovery SpaceClaim will then treat all the volumes as a single connected part, so it is completely meshed with hexahedral elements.
Engineers complete the preprocessing by setting up a frictionless support and inputting the load defined by ASME. The support will ensure the part is restricted horizontally. Table 2 summarizes the load factors that need to be plugged into ANSYS Mechanical based on the given setup. These loads will determine if the part passes or fails the FAT.
Table 2. Load factor table for different analyses
|Check Type||Analysis Type||Load Factor for Analysis||Load Factor for Evaluation|
|Protection against Plastic Collapse||Elastic||1||1|
|Protection against Local Failure||Elastic||1||1|
After the part is properly meshed and preprocessed, we are ready to perform an elastic stress analysis or an elastic-plastic stress analysis.
Let’s start with the elastic stress analysis.
For this test, ASME states that a stress linearization method must be used. To do this, engineers can create a path in the geometry that extracts their results. This is called constructing a stress classification line (SCL). The constructed paths in this model are shown in Figure 2.
The linearized stress results are listed in Table 3. The table also contains the allowable stress for the design based on calculations from the ASME standard.
For the design to meet FAT requirements, according to ASME, the utilization value in the last column of Table 3 (equal to the simulation results divided by the allowable stress) must be less than one. This design has passed the elastic stress analysis as all the utilization values are less than one.
Table 3: Linearized stress results along the paths
|SCL||Stress Component||Results (MPa)||Allowable Stress
ASME VIII Div2
|Path 1||Membrane stress||349||369||0.95|
|Membrane stress + Bending Stress||641||787||0.81|
|Path 2||Membrane stress||151||369||0.41|
|Membrane stress + Bending Stress||240||787||0.30|
|Path 3||Membrane stress||270||369||0.73|
|Membrane stress + Bending Stress||240||787||0.38|
|Path 4||Membrane stress||137||369||0.37|
|Membrane stress + Bending Stress||261||787||0.33|
|Path 5||Membrane stress||207||369||0.56|
|Membrane stress + Bending Stress||217||787||0.28|
|Path 6||Membrane stress||352||369||0.95|
|Membrane stress + Bending Stress||638||787||0.81|
For the elastic-plastic stress analysis, the load factor applied on the tee are again determined by the ASME code. The part passes or fails based solely on convergence. If it converges then the part is stable — if it does not converge then the part is unstable.
In this current analysis, the tee component results passed the elastic-plastic stress analysis.
This indicates that the structure meets the minimum requirements to prevent plastic collapse.
How Simulation Can Prevent Local Failure of an Subsea Tee Junctions
To complete the FAT, you must still test your tee junction’s ability to survive local failure. The two tests that can be used for this assessment are elastic analysis and elastic-plastic analysis.
For elastic analysis, ASME states that the sum of the local primary membrane stresses (σ1, σ2 and σ3) shall be less than or equal to four times the allowable stress (S) defined by the ASME standard. In this case, the results are:
This means that the design passed the elastic analysis.
The elastic-plastic analysis requires engineers to perform four steps:
Step 1: Extract three principle stresses (maximum normal stresses: σ1, σ2 and σ3) and the equivalent stresses (von Mises stress: σe).
Step 2: Determine the limiting triaxial strain (εL) based on your material (in this case duplex steel). This value is based on the formula offered by ASME:
In this formula, αsl, εLu and m2 are material-dependent parameters defined by the ASME standard.
The next steps determine if the maximum triaxial strain in the part is less than the limiting triaxial strain.
Step 3: Check the forming strain. This is the strain found within the part that was created by the manufacturing process. This value is estimated based on the material and fabrication method in accordance with the table found within the ASME standard.
However, for parts that are heat-treated, the forming strain will become insignificant. In this case, it is assumed the value is equal to zero.
Step 4: Extract the equivalent plastic strain from the simulations and compare it to the limiting triaxial strain based on the strain ration. The component passes if the strain ratio is less than one. The strain ratio is defined by the following formula:
These calculations are not native to the ANSYS simulation platform. However, the software can make customized versions of these calculations by setting up a user-defined result.
The strain ratio in this setup is less than one. As a result, the part passed the elastic-plastic analysis. This indicates that the design meets the requirements for the local failure plastic strain check.
Since the part passed all assessments, it has passed the FAT. This assessment was performed using ANSYS Mechanical Software. To learn other ways that ANSYS can help you design your subsea applications, click here.