Tuesday, November 24, 2015

New Boundary Conditions for Water and Environmental Applications

For numerical modeling of river flows, typically water elevation is required at the upstream boundary. Yet water elevation in natural environmental systems is often unknown and has to be estimated. Improper elevation estimation, however, can generate nonphysical results. In FLOW-3D v11.1, which has just been released, users now have the option of having boundary water elevations dynamically adapt to the conditions inside the domain. This can be achieved through the use of rating curves provided by the user, or in the absence of rating curves; the solver can dynamically adjust the elevation to vary smoothly with the conditions inside the fluid domain. These variations may be further constrained to certain Froude regimes or absolute elevation bounds.
Figure 1. Rating curve for John Creek at Sycamore from USGS

Rating curves

Rating curves define elevation variations at a given location in a river reach according to inflow rates at that location. A relationship between elevation and volume flow rate is established by physical measurements at a particular cross section of the river. Rating curves for rivers in the United States are available from the USGS (U. S. Geological Survey). A typical rating curve will have volume flow rate on the X-axis and elevation on the Y-axis (Figure 1).

Natural inlets

In a case where inflow rate is known but a rating curve is unavailable, a natural boundary condition can be selected in the FLOW-3D model setup interface. At a given cross-section, for a certain specific energy, there can be two possible depths. This arises from the quadratic relationship between specific energy and the depth (see the equation below). The two mathematical depths manifest into supercritical and subcritical depths in reality. In the case of a perfect unique solution to the quadratic equation, the flow is critical. 

Here, E is the specific energy, q is the unit discharge, g is acceleration due to gravity and y is the height of fluid. Graphically, the specific energy and depth relationship can be seen in Figures 2-4. 

Figure 2. Changes to E-y curve, changing q

Figure 3. Possibility of two flow depths (supercritical and subcritical) for the same value of specific energy

Figure 4. Flow depth can be critical (yc) for a unique value of depth and specific energy. In this case, flow is neither subcritical nor supercritical.

Applying new boundary conditions

A rating curve can only be defined for volume flow rate and pressure boundary conditions in FLOW-3D v11.1. For volume flow rate type boundary conditions, instantaneous elevations are calculated using the rating curve to find the elevation corresponding to the flow rate. For a pressure type boundary condition, the volume flow rate is calculated by the solver and elevation is calculated using the rating curve. Rating curves can be applied at both upstream and downstream boundaries. It is important to note that an incorrect rating curve can result in nonphysical flow fluctuations.

Natural boundary conditions can only be defined at the inlet. Flow categories can be defined from one of the following:
  1. Supercritical flow (y<yc)
  2. Subcritical flow (y>yc)
  3. Critical flow (y=yc)
  4. Automatic flow regime (calculated by the solver)

The user can define maximum and minimum limits of elevation for any of these flows. If the depth for a particular flow regime violates the maximum and minimum limits of elevation, the latter will take precedence.

Sample simulation results

Simulation 1 shows the river reach with a natural inlet under volume flow rate boundary condition at the left boundary and a rating curve for the outlet is defined as a pressure boundary condition at the right boundary.  The evolution of water elevation is shown for both upstream and downstream boundaries simultaneously. The simulation shows smooth variation of elevations at the boundaries without any fluctuations or nonphysical behavior. Therefore, this new development in FLOW-3D v11.1 allows for more natural variations of the water level for environmental applications.

Simulation 1. Evolution of water elevation in a river reach with natural boundary condition at the inlet and a rating curve at the outlet.

Tuesday, November 3, 2015

Raster Data Interface and Subcomponent Specific Surface Roughness

FLOW-3D allows users to import solids in STL (StereoLithography) format to represent complex geometries, regardless of the application – micro fluids, metal casting, water and environmental, aerospace, etc. While for many industries, the STL format is a very natural and common way of representing and sharing 3D objects, in the water and environmental industries there is a preference towards surface-driven representations of the environment. After all, the earth’s terrain does look like a surface for most practical purposes.

Raster Data Interface

In the upcoming release of FLOW-3D v11.1, we have adopted an industry norm for terrain import: the file format known as the ESRI ASCII raster format. The details of the format are described here. All GIS software packages are able to export in this format. Such *.asc terrain files will now be able to be imported directly (Figure 1) into the FLOW-3D user interface.

Figure 1. Direct import of terrain in FLOW-3D v11.1 using ESRI ASCII raster terrain format

Subcomponent Specific Surface Roughness

Alongside terrain import, a critical modeling variable in modeling flood wave propagation, flooding area, etc., is surface roughness. In particular, the user needs to model local, spatially-varying surface roughness. In FLOW-3D v11.1, users will be able to import surface roughness coefficients in the same ASCII raster format.

More specifically, the user actually imports a raster file of the land coverage index and provides a simple text file palette conversion table. This table converts the type of land coverage (sand, vegetation, built-urban, etc.) defined in the raster file to surface roughness values that are required by the FLOW-3D solver. This gives the user a very effective way to fine tune the surface roughness coefficients without having to regenerate the entire raster file by simply altering the palette conversion table.  The ASCII raster format was chosen because it remains simple, yet lets the user easily control the surface coefficients that are mapped over the domain following the land coverage types.

Figure 2. Example of overlay of terrain in FLOW-3D v11.1 Model Setup Graphical User Interface

Figure 3. Example of overlay of terrain in FLOW-3D v11.1 Model Setup Graphic User Interface

In the same framework of modeling complex flood events, functionality to overlay actual pictures of the environment, such as river banks, built structures, and developed housing has been added.  FLOW-3D v11.1 allows users to directly texture their terrain with corresponding imagery, typically obtained from satellite imagery.

This operation can be conducted in two stages in FLOW-3D. The first stage is during model setup (Figures 2 and 3), so that the user can see the context of the model he or she is building, making it easier to be sure the simulation is properly set up. The second stage is during post-processing in FlowSight. This is where the overlay of the flooding event and the terrain imagery is used to reveal the extent of the flood zones and the interaction of the flood wave with the environment.

Example Simulations and Conclusion

Figures 4 and 5 show the results from flood routing of the streams in two different terrains. Upstream elevations have been plotted for the example cases. Note that the analysis has been done on a terrain overlaid with surface roughness data. The ability to import raster data and overlay it with surface roughness provides the user a single platform, i.e., FLOW-3D, to conduct the water and environmental studies on the terrain. Typical flood wave propagation through a stream can be seen in Simulation 1.

Figure 4. Flood event analysis of the example in Figure 2 with overlaid surface roughness data

Watch the YouTube video >

Simulation 1. Flood event analysis of a location on earth. Terrain raster data has been overlaid surface roughness data within FLOW-3D.

Tuesday, October 27, 2015

P-Q Squared Analysis

P-Q2 analysis is a standard procedure used to optimally match the target gate velocity to the capabilities of the HPDC (High Performance Die Casting) machine’s plunger hydraulic system. Desired fill time and an optimum gate design can be attained by performing P-Q2 analysis, which in turn, maximizes the efficiency of the HPDC system. 


The theoretical basis of the P-Q2 analysis is the conservation of energy for steady incompressible flow. According to Bernoulli's equation, the metal pressure at the gate is proportional to the flow rate squared:

The assumptions for this analysis are:
  • Constant discharge coefficient
  • Liquid metal has reached the gate
  • No air in metal stream at the gate
  • No solidification during the filling
  • Runner is the main resistance in the flow
As shown in a typical P-Q2 diagram below, the machine performance line shows how the die casting machine capabilities vary depending on the flow rate. A larger flow rate demands a larger pressure from the machine to move the plunger at desired velocity. This means that, the higher the pressure, smaller the plunger, and the higher the flow rate, the larger the plunger. The operational window is defined by the fill time, gate velocity, metal pressure, etc. It is important that both the die and machine operate within the operational window (Figure 1).

Figure 1. Plot showing the operational window

Setting up P-Q2 analysis

To perform P-Q2 analysis, the Geometry Type of the piston must be defined as Plunger. This can be done when you add the piston to your geometry (Geometry -> Add geometry).

Figure 2. Geometry tab

Enable P-Q2 analysis by selecting the Perform PQ^2 analysis option in the Details tab of the component,  Piston (Figure 2). Enter the machine parameters (Figure 3) to define the machine performance line.

Figure 3. Defining machine parameters

During the design stage, the user specified process parameters may not be optimal, for instance, the resulting pressure is beyond the machine capability. If so, toggle on the Adjust velocity option for the piston velocity to be automatically adjusted to match the machine capability. Now, the flow rate will be adjusted at each time step if the pressure at the piston head is beyond the machine capability. Once the pressure drops below the machine performance line, the piston will then accelerate towards the prescribed velocity. 

Viewing or Post-Processing The P-Q2 diagram

The P-Q2 analysis data such as pq2 pressure, and pq2 flow rate, are written out in the History Data. They can be accessed in FlowSight by pressing the History data button. In the History Data dialog, select Piston: pq2 diagram in the variable list and press the New plot button to create a plot of the P-Q2 diagram:

Figure 4. History data and the P-Q2 diagram

The P-Q2 diagram above indicates that adjustment may be needed to bring the pressure down below the machine performance line. You can either toggle on the Adjust velocity option and retry (see Figure 5), or modify your machine parameters.
Figure 5. Adjusted pq2 diagram


FLOW-3D Cast v4.1 allows you to perform P-Q2 analysis that helps achieve desired fill time and optimum gate design. The analysis data can be viewed and processed in FlowSight, an integrated post-processor that comes with the FLOW-3D Cast installation.

Tuesday, October 6, 2015

Batch Post-Processing and Report Generation

In the upcoming releases of FLOW-3D v11.1, FLOW-3D Cast v4.1, and FLOW-3D/MP v6.1, batch post-processing and report generation have been developed hand-in-hand to save users significant time when it comes to visualizing, analyzing and communicating the results of their simulations.

Batch post-processing allows you to define a set of post-processed results that are created in the background while a simulation is running or after it has been completed. So, when you come back to your workstation, your videos, images, and other output will be ready. This is particularly helpful when simulations are huge and post-processing can take a significant amount of time. Report generation can be run after batch post-processing is complete, which combines the results into an HTML file that can be viewed in a browser and easily shared.


Batch post-processing requests can be defined even if no results are available yet. Context files from other simulations or a previously run simulation can be used. Also, a user-defined template can be applied to a simulation doesn't have results yet. A Context File contains information about layout, views, orientation, variables loaded, etc. Results can be requested ahead of time to be written according to the context file.

Within batch post-processing, animations, scenario files or images can be ordered – any or all. Scenario Files are essentially “interactive animations” that are played in a special viewer that allows the results to be rotated and zoomed in/out providing much more flexibility for analyzing results.

The setup of batch post-processing requests is even more flexible when simulation results exist. Certain plots like isosurface, volume render, 2D-clip, line plot, etc. (Figure 1) can be requested ahead of time and generated automatically.

Figure 1. Batch Mode window showing the available types of plots that can be written

Figure 2. Sample results that are requested through Batch Mode.

An example of the batch post-processing is shown in Figure 2. Column 1 allows the user to select the type of plot. In 3D options, an iso-surface, volume render and 2D clip are requested for hydraulic head. In 2D options, another 2D clip is requested and so on. Column 3 allows the user to select the type of output, animation, scenario and image, respectively. In column 4, timelines can be chosen – Selected or Restart. In conclusion, setting up a batch process is very flexible.

Avoid Repetition

Analysis of many similar simulations (e.g., parametric studies) is much easier with batch post-processing as the repetition of requesting the same post-processing graphical results is eliminated. This can be achieved by simply choosing an already available template. Templates can either be process templates like metal casting and hydraulics or a user-created template. If you choose a process template for metal casting, certain default variables and plots relevant to the metal casting industry will be written. But, if you want to use a customized template that you have created, then choose one from the User Templates tab.

More Automation

Avoid the hassle of accessing your workstation at night using Run Batch Process. All you need to do is to choose Run Simulation and Batch Process. This way, the batch processing will start automatically once your simulation has completed. This higher level of automation can be opted for if one or more of the following cases applies:
  • The simulation is large and you don’t have time to interactively post-process results
  • You already know what you want to see from the results and would just like it to be done automatically
  • The results analysis is very complex and would take lots of time to recreate interactively

Report Generation

Once batch post-processing has completed, the user can assemble the myriad of animations, images and text results into an HTML report by right-clicking on the simulation in the Portfolio and selecting Generate Batch Report. The report will be generated in HTML5 format (sample report in Figure 3) and can be easily sent to your manager, associates, colleagues, and clients. Images and videos will be embedded in the report. You will still have control over the formatting of text, captions, and references.

In conclusion, you can now spend less time on post-processing and reporting and instead run more simulations.

Figure 3. HTML report for an energy dissipative tumbler simulation

Tuesday, September 22, 2015

Solid Propellant Combustion Modeling

Solid fuel combustion is a traditional method of extracting energy from solid objects. However, an important relatively new application of solid fuel combustion is in rocket propulsion. The development of the new Combustible objects model in FLOW-3D v11.1 was motivated by solid propellant combustion in rockets. The model describes the conversion of solid rocket propellant to gas with a heat source, mimicking the combustion process in solid-fuel rockets.

The physics behind the model

The burning of the propellant in the combustion chamber results in increased temperature and pressure of the surrounding gas. In addition, as propellant is burned, the flow domain increases. It is of interest to predict these changes in the flow because the dynamics (e.g., trajectory and velocity) of the rocket depends on them. To account for the changes in the size of the flow domain, a variant of the General Moving Object (GMO) model has been developed. In the augmented model, the geometry component representing the solid propellant is designated as a GMO component of a special type: instead of moving, it changes shape and size. Such deformation of a combustible part can be seen in Simulation 1. If the elastic stresses within the solid propellant need to be modeled, the Fluid-Structure Interaction model will work with this new development.

The mass source of the combustion gas is assumed to be of stagnation type, i.e., the initial velocity of the exhaust gas is zero. As a result, no additional source term is present in the momentum equations. The combustion rate is defined by the equation below. dm/dt is the combustion rate or, simply, the rate of change of mass of the solid propellant, P is the pressure of the combusting gas, and a and b are empirical parameters.
How to set up the model

The model requires that the compressible flow model is activated. The solid propellant is defined as a special type of geometry component – combusting and the reaction parameters (a and b) need to be defined. Default values for multiplier and power coefficients are given, but these values can be changed by the user. The default values for multiplier and power coefficients are 1e-05 and 0.5, respectively. These values can be changed by the user.

An example simulation with results

This simulation is of a solid propellant combusting inside a rocket. The design used for the rocket part along with the real part is shown in Figure 1. A cylindrical mesh was used because of the cylindrical geometry of the setup.

Figure 1. The rocket part used for simulation in FLOW-3D v11.1 along with a real part

Results and Discussion

Evolution of gas pressure (evolution with time is shown in Simulation 1), velocity, and combustion gas mass fraction is typically what a user will likely study. Courant number is also shown in the results (Figure 2), which is a ratio of the distance traveled by fluid in one time-step to the mesh cell size.

Courant Number

Higher values of Courant number indicate that the time-step size may be too big to accurately capture the local flow parameters. In Figure 4, the Courant number stays low inside the ignition chamber but increases as the flow transitions from the chamber to the nozzle. Since the main purpose of studying this case was to simulate the behavior of combustible object, as far as the ignition chamber goes, the Courant number there is low, ensuring an accurate solution. This may not be the case in the nozzle, but the user can reduce the time step to run the simulation at a lower Courant number, if required.

Figure 2. Planar plots of important variables in FLOW-3D v11.1

Explicit vs. Implicit

By now you might have thought about the numerical complexities involved in this simulation. The overall time-step size is limited by the advection velocity in the nozzle, which may lead to large computation times. An implicit advection scheme could be used to speed up the calculations. However, the time step-size must be carefully controlled to minimize the errors associated with the implicit scheme.

Pathlines and Circulation

Pathlines are excellent mathematical functions and visualization tools to understand the history of a fluid particle in the computational domain. A strong visualization tool like FlowSight calculates the pathlines depending on user’s requirements in terms of length, number, etc. Figure 3 shows the combustible part from the bottom (longitudinal direction) in the top-left viewport. The pathlines are calculated and visualized in the main viewport (the figure in the center). At one glance, it can be seen that a significant amount of local circulation is happening, along with a global circulation at the periphery. Such physics may be important to understand while programming the trajectory of a rocket. 

Figure 3. Pathlines of the fluid in the combustible part visualized using FlowSight


Simulation 1. Deformation of the combustible component and the evolution of pressure over time.

Wednesday, September 9, 2015

Thermal Die Cycling Model

Thermal die cycling is a standard process die casting facilities use to get their die up to temperature for full production. Think about showing up to work in the morning, mid-winter: your machines are cold! Typically someone will fire the die to get the machines warmed up and then go through a series of “dry shots” where the parts are considered sub-par quality or have a high potential for defects. After a handful of cycles (around 10), the die is hot and has a consistent temperature distribution throughout, ensuring consistent results. The series of dry shots informs you about your cooling channels’ performance and whether you need to re-locate or up the flow rates, before building any tooling. This process can be effectively simulated in FLOW-3D Cast v4.1, saving valuable time and decreasing costs even more.

The physics behind the model

The Thermal Die Cycling model in FLOW-3D Cast v4.1 provides accurate calculations for the following physics:
  • Assessing thermal distribution of die/tooling
  • Heat removal rate of the cooling channels and their locations
  • Thermal analysis of the entire casting process for tooling design to assess large volume (or small volume for prototyping) thermal development and a steady operating state
  • Parting line cooling during the die spraying and cleaning stages
  • Cooling of the cover and ejector at different rates during a period of high thermal gradients during the ejection stage

Apart from the physics there are stages in a thermal die cycling process that can affect the results of the simulation, e. g., leaving the part in the die during the ejection stage changes the nature of the heat transfer for all components involved. Similarly, along with the cooling lines the parting lines should also be modeled. The Thermal Die Cycling model considers all such scenarios to accurately predict the actual process.

How do I access the model?

The Thermal Die Cycling model can be accessed in the Casting Models tab of the Models window. On clicking Thermal Die Cycling (Figure 1), a Thermal Die Cycling window will pop up (Figure 2).

Figure 1. Accessing thermal die cycling in FLOW-3D Cast v.4.1

Figure 2. The Thermal Die Cycling model window in FLOW-3D Cast v4.1.

How do I use the model?

The Thermal Die Cycling model is easy and intuitive to use, however, there are certain requirements for various design stages to ensure that the model gives accurate results that I will talk about in the following paragraphs.

Requirements for different stages
You can define each step of your own process but the first step must always be “Solidification.” We give you options to define different cooling heat transfer coefficients at all stages during each cycle. The ejection stage allows you to define different values for both the cover and ejector for accurately simulating the differential cooling rates of the cover and the ejector. The difference in cooling rate arises because while the part remains in one side of the die (typically the cover), there will be a different thermal profile between the ejector/cover sides.

For the rest of the stages, and in between these stages, you can rearrange and re-order as you need. For example, if you were to air dry before and after your lubrication stage, you may in fact remove too much heat so you might test different arrangements of your process. Another problem might be that you are not removing enough heat during the spraying/cleaning stages. This aspect of the analysis is extremely easy to change and can be done in columns 3 thru 5 (Figure 2). Depending on how long you are spraying the die, or what you are spraying with, your heat removal can change. Take room temperature oil for 10 seconds versus cooled water for 1 second, both will react very differently with your die surface temperatures and thus the total heat removed will also differ. We allow you to quickly assess these differences before you have to manufacture any tooling, a huge cost savings and improvement of your bottom line. Now, if these practices do not succeed in maintaining your thermal profile, you know that you will need to re-assess the locations of your cooling channels in order to get your desired outcomes and once again, this is a huge cost savings for your company. Manufacturing a set of die tooling only to find that your cooling lines are inadequately placed is a setback that can be easily avoided using this model and can get your parts to market as fast as possible.

Finally, this model essentially “turns off” all fluid dynamics calculations and the physics involved are strictly heat transfer based (conduction only). This allows for extremely fast simulation results and can be easily worked into a facility’s workflow. The fully-developed heat distribution throughout your die as your initial condition for your consequent filling and solidification simulations will allow for an accurate assessment of your temperature-related defects. It also helps to identify early solidification issues before you send the designs off to be manufactured, avoiding potentially catastrophic flaws.

Sample simulations

Two sample simulations of a heat exchanger for a consumer product are shown below. Simulation 1 models the die spray stage and evolution of the temperature profile on the 'surfaces' of the two die components, the ejector and the cover. The surfaces where the die components come together during a shot are referred to as the ‘parting lines,’ where a majority of the heat removal will take place. This stage also acts as a cleaning stage in reality, but since we do not model leftover residues, we do not take this into account.


Simulation 1. Cycle 10, Die Spray (Cleaning and Cooling) surface temperature: Notice the heat transfer occurs on all surfaces simultaneously; individual spray jets are not considered at this time.

Simulation 2 is a cross-sectional view of the die components during the entire tenth, and final, cycle. For this analysis there were 6 stages in each cycle: 1. Solidification, 2. Ejection, 3. Open, 4. Blow Air, 5. Spray lubricant, 6. Closed, and we ran 10 total cycles. On the shop floor this would translate to 10 "shots" in order to develop this temperature profile. Notice the cooling profile at the parting lines, which are the horizontal contours, and how they change with time.

Tuesday, September 1, 2015

Mooring Lines Model and Wave Absorbing Layer

While the Mooring Lines model and the Wave Absorbing layer are two separate developments in FLOW-3D v11.1, I am going to talk about both in this post because users will often use them together in simulations. The development of the Wave Absorbing layer in FLOW-3D v11.1 was prompted by the need to minimize wave reflection at open boundaries of the simulation domain; while extensive use of mooring lines in ocean engineering led to the development of the Mooring Lines model. Although these developments can be used hand in hand, completely independent use of each is also possible.

Mooring Lines model

Mooring systems are common in offshore structures, ship mooring and renewable energy harvesters. A mooring line can extend to thousands of meters, so the effects of mass and fluid drag cannot be neglected. FLOW-3D v11.1’s new model accounts for these effects to calculate the dynamic behavior of the system. Combined with FLOW-3D’s General Moving Object model and free-surface flow capability, FLOW-3D provides a highly-accurate computational solution to cases involving dynamic movement of objects such as a US patrol boat (simulation 1) or a semi-submersible offshore platform (simulation 2), tethered to mooring lines in a body of water.

Simulation 1. Movement of US patrol boat (digital model only) tied to four mooring lines in presence of the waves.

What is special about the Mooring Lines model?

The Mooring Lines model considers gravitational and buoyant forces, elastic tension, and normal and tangential drag forces. A mooring line is divided into discrete segments for numerical integration of the dynamics equations. Additionally, mooring lines can exist below the computational domain, reducing the requirement of extending the computational mesh all the way to the depth of the water body. For this a Deep Water Velocity (Figure 3) feature is available to capture flow effects on the portion of lines outside the computational domain. A feature called Confined Space (Figure 3) allows the mooring lines to lie on the ground after a certain defined depth inside the computational domain. Figure 1 shows the mooring lines that partially lie on ground.

Figure 1. The original line length is 100 m but after 70 meter depth it lays flat on ground.

Wave Absorbing layer

A wave damping algorithm has been added to help minimize surface wave reflection from open mesh boundaries and their interference with the solution. Simulation 1 and Simulation 2 have Wave Absorbing layers at the outflow boundaries (where waves are leaving the computational domain).

Where can I find the new developments?

Mooring lines can be added through the Springs and Ropes window in the Meshing and Geometry tab as shown below. The original Springs and Ropes Model is still available for users.

Figure 2. Accessing Springs and Ropes model in Meshing and Geometry tab.

Figure 3. Mooring Lines model (appears after clicking on Springs and Ropes model in Figure 2)

In the same way that users define a component type as a solid, lost foam, etc., they can now define the component as a Wave Absorbing type (Figure 4).

Figure 4. Wave Absorbing component

Wait, how do the Springs and Ropes and the Mooring Lines model differ?

The Springs and Ropes model assumes that the ropes are weightless and always straight when stretched; rope tension is uniform; and rope dynamics is ignored. The Mooring Lines model calculations do not use these assumptions. Having said that, a user may still find the Springs and Ropes model useful if the conditions fall within the assumptions of the model.

Physics and simulation setup

To demonstrate the power of the model, a simulation of a semi-submersible offshore platform tethered to the sea bottom was set up. This platform is tethered by twelve high modulus polyethylene (HPME), SK78 EA mooring lines rated at 630 tons minimum breaking load rope. A severe sea state with 10 meter high non-linear propagating waves is defined. Remember that we have used a Wave Absorbing layer at the outflow to nullify the reflecting effect of these non-linear waves at the boundary.

In this simulation, the mooring lines are tethered to the sea bottom. Other than the mooring lines dynamics, relevant physics activated in this simulation are:
  • Offshore platform and fluid are fully coupled in dynamics
  •  Mooring lines to constrain the offshore platform
  • Non-linear wave generation using the Fourier series method
  • Wave absorbing boundary to minimize wave reflection at the outflow boundary
Mooring lines details and setup

The mooring lines created for this simulation are high modulus polyethylene ropes rated at 630 tons minimum breaking load with a linear density of 5.1 kg/m and diameter of 105 mm. A total of 12 mooring lines are used in the simulation and are coupled in groups of 3 (red, green and blue). There are 4 such groups in the simulation. These groups are referred as quadrants in the simulation. If groups are in order from left to right in the simulation view, then quadrant 1 refers to the leftmost group (group 1) in simulation view, quadrant 3 corresponds to group 2, quadrant 2 corresponds to group 3 and quadrant 4 corresponds to the rightmost group (group 4).

Simulation and observations

Shown in the animation are the moored platform and the maximum tensile force on one mooring line from each quadrant. The tensile force on all 12 mooring lines could have been plotted but in order to keep the plot visually readable, only one line from each quadrant is plotted. An interesting observation is that the maximum tensile force is reached in the line listed in quadrant 1. As one would expect, the mooring lines start drifting in the direction of the waves, causing an increase in tension (tautness) of the lines.

Simulation 2. Dynamics of a semi-submersible moored offshore platform and the maximum tensile force on one line in each quadrant.