Documentation

The Multi-purpose analysis type offers an automated robust meshing strategy producing hexahedral cells suitable for the underlying solver, thereby reducing mesh generation times by huge margins. Because the mesh has a high quality, it requires fewer cells to achieve the same level of accuracy. It offers faster convergence at the cost of a reduced feature set. Some highlights of the mesher are:

- Body fitted Cartesian meshing
- Cells suitable for finite volume discretization
- Robust and quick meshing algorithm

Multi-purpose is a Finite Volume-based CFD solver with segregated pressure-velocity coupling using a proprietary variant of the SIMPLE\(^1\) algorithm. It provides the possibility to simulate both **incompressible** and **compressible** flow, either **laminar** or **turbulent** in a single framework. Turbulence is modeled using the RANS equations with the k-epsilon turbulence model for closure and proprietary wall functions for near wall treatment.

Multi-purpose supports **steady-state** as well as **full transient** analysis. In full transient analysis, the fluid flow is modeled in a time-accurate manner and any rotating component in the domain is solved using the sliding mesh approach.

Within SimScale, one can effortlessly set up a Multi-purpose simulation that involves the following steps:

To create a Multi-purpose analysis, first, select the desired geometry and click on **‘Create Simulation’**:

Next, a window with a list of several analysis types supported in SimScale will be displayed:

Important

*Multi-purpose* is a specialized analysis type restricted to users with a paid plan. For more details please visit our product & pricing page or contact sales.

Choose *Multi-purpose* analysis type and click on **‘Create Simulation’**. This will lead to the SimScale Workbench with the following simulation tree and the respective settings:

To access the global settings, click on **‘Multi-purpose’** in the simulation tree. The following parameters are available to define the fluid flow simulation:

**Compressible:**Toggle on if a compressible flow simulation is desired with heat transfer.**Multicomponent:**Toggle on when simulating the mixing of two or more fluids with different densities and viscosities.**Multiphase:**Multiphase simulations can be performed for multiple fluids with different phases. Works only with transient analyses.**Number of phases:**Specify the number of phases involved in the multiphase simulation.**Cavitation model:**Toggle on to include the cavitation phenomenon using the constant gas mass fraction model.**Turbulence model:**Besides the laminar model the solver supports the k-epsilon turbulence model.**Time dependency:**Both*Transient*(time-dependent) and*Steady-state*options are available.

The *Geometry *section allows you to view and select the CAD model required for the simulation. In general, having a clean CAD model always helps to avoid any meshing or simulation-related errors. However, the mesher is pretty robust and if the CAD is genuinely dirty then a message of mesh failure and further instructions on CAD cleaning or mesh refinement should appear.

Find more details about CAD preparation here.

If the simulation has a rotating component, then rotating zones need to be created for each rotating part. You can find a detailed approach to CAD preparation in the following article:

Under *Model*, gravity can be defined via a vector. The global coordinate system, represented by the orientation cube, applies to the direction of gravity. The vector coordinates \(g_x\), \(g_y\), and \(g_z\) represent the x, y, and z directions.

Surface tension can also be set for multiphase simulations. The default value of the surface tension coefficient is set to zero,

Under *Materials,* the appropriate fluid for the simulation can be chosen from the materials library. The user has the option to change certain fluid properties*. *For compressible simulations, since the temperature is involved the user needs to specify the corresponding thermophysical properties for the fluid in consideration.

Along with perfect gas behavior, it is possible to model real gas behavior also by specifying material properties as a function of pressure and temperature.

Real gas modelling

Fluids operating at very high pressure or low temperatures do not follow ideal gas behavior. For such ‘real’ fluids, more complex relations specifying the physical and thermodynamic properties are required, known as the **real gas model**.

For example, flow of refrigerant in compressors, flow of steam in a steam turbine, flow of gas mixture in a piping system etc.

To simulate real fluids the compressible flow toggle needs to be on under global settings as discused earlier.

For more information, please visit the relevant documentation page for materials.

Initial conditions define the values which the solutions fields will be initialized with. For Multi-purpose analysis, *Initial conditions* can be set up in the simulation tree only when the *multiphase* is toggled on under global settings. The phase fraction can be initialized globally or for a specific region as a *subdomain* for all the phases involved.

Boundary conditions help to add closure to the problem at hand by defining how a system interacts with the environment. In an incompressible simulation, the computational domain will be solved for two fields: pressure \((P)\), velocity \((U)\), while for a compressible simulation the temperature \((T)\) field is also involved. Additional turbulent transport quantities may be included based on the turbulence model selected.

The following boundary conditions are available for a Multi-purpose simulation:

- Velocity inlet
- Velocity outlet
- Pressure inlet
- Pressure outlet
- Wall (including wall roughness)
- Symmetry

Important

Parametric Studies

Multi-purpose analysis type allows parametric studies with the velocity boundary condition. When you select *Flow rate* as the velocity type while assigning velocity to an inlet or outlet face then you can input multiple flowrates at once either directly or by uploading a file.

This will initiate multiple runs with different flow rates assigned at once in parallel giving the user a huge time advantage.

Results become available for individual flow rates as separate runs (*Run 1, Run 2,……*) and also for the complete parametric study where the whole parametric curve is plotted. Figure 11 shows the pressure difference curve for all 8 flow rates assigned under the simulation run named *Test run* by the user.

Under *Advanced concepts*, you will find additional setup options for rotating zones and porous media.

*Rotating zones*can be used to model rotating systems such as turbines, fans, ventilators, and similar systems. Currently, the MRF (Multiple Reference Frame) type is supported.*Porous media*concept allows users to define regions with porosity characteristics within the computational domain.

The *Simulation control* settings define the general controls over the simulation. There are differences in the setup parameters, depending on the *Time dependency* of the analysis. Find below the differences between transient and steady-state analyses:

In the simulation control settings, there are only two parameters exclusive to the Multi-purpose analysis type:

*Number of iterations*:**Steady state:**It represents the number of iterations beyond which the simulation terminates, i.e., no more iterations will be performed.

*Convergence criteria*: The relative residual is the ratio of the current iteration residual to the running maximum residual -the maximum residual until that iteration.**Steady-state:**A relative residual is computed by dividing the residual at each iteration to the running maximum value. Once the relative residuals fall below the convergence criteria for all equations, the simulation is assumed to be converged and will stop. Lower values like 0.001 are recommended for convergence.**Transient:**For a transient simulation, a relative residual is defined by dividing the residual of each sub-iteration (iteration per timestep) by the running maximum. The simulation progresses to the next timestep if this relative residual falls below the convergence criteria or the number of maximum sub-iterations per timestep is reached. Currently, the default maximum limit to the number of iterations per time step is 25. In case of no convergence, the relative residual for the last sub-iteration for that time step is recorded and we move forward to the next time step. The recommended value for convergence criteria is 0.1.

For a complete overview of the other simulation control parameters and their meaning, please check out this page.

The* Result Control* section allows users to define additional simulation result outputs. It controls how the results will be written meaning the write frequency, location, statistics of the output data, etc. The following control items are supported:

**Forces and moments**: Calculates the forces and moments on a specific surface or set of surfaces. This is useful, for example, when one wants to find pressure and viscous forces on turbine blades in a hydrodynamic analysis.**Surface data**: Calculates average or an integral sum of the simulation results on a specified surface area.

For the Multi-purpose analysis type, the mesh generated is a Cartesian mesh which means that each cell represents a cube with edges parallel to the XYZ Cartesian axes making the mesh highly orthogonal.

The meshing algorithm is automated and follows a top-down approach which works by creating a binary tree structure. The bounding box (an imaginary box encompassing the dimensions of the flow domain) is refined anisotropically by cutting cells in the first layer (x-direction), in the second layer (y-direction), and the third layer (z-direction).

For the mesh in Multi-purpose analysis, the settings can be set to automatic or manual. The parameters under each mode are described below:

The user gets to define the following parameters:

*Fineness*: It automatically controls the fineness levels for the mesh cells varying from*Coarse (1)*to*Fine (10)*.*Merge CAD surfaces*: It combines (merges) the faces of each CAD volume, making it easier to mesh. Any CAD faces with boundary conditions or result controls are left untouched. This feature does not repair faults in the CAD geometry or add/subtract surfaces. It is intended to optimize the arrangement of CAD surfaces for improved mesh generation. This feature makes the mesh generation process more robust with:- Improved meshing of small surfaces
- Better handling of complicated, multi-part geometries
- Better mesh distribution, saving simulation time and core hours

The user gets to define the following parameters:

*Cell size specification*: It controls if the following parameters are entered as**Absolute**values, in corresponding length units, or they are rather**Relative to CAD**, in which case the parameters represent a fraction of the representative length of the model.*Minimum cell size*: This parameter specifies the minimum size for all cells of the resulting mesh.*Maximum cell size*: It specifies the maximum size for all cells of the resulting mesh.*Cell size on surfaces*: This parameter specifies the size for all cells on and close to the surfaces.*Specify growth rate*: It specifies the cell size ratio between the adjacent cells. It needs to be a whole number greater than 1 such that the cell size increases towards the interior of the mesh domain. For example, a value of 2 would mean that the inner cell is twice as big as its adjacent cell closer to the surface.*Merge CAD surfaces*: Same as discussed above for the automatic mesher.

For additional mesh refinements on specific volume regions within the simulation domain, the choice of region refinement is available.

These volume regions or refinement zones can be created using geometry primitives.

**Target cell size:*** *This parameter specifies the length scale of all the cartesian cells lying within the defined refinement zone. The resulting cell size might be smaller than the target specified to accommodate for the binary-tree mesh algorithm.

Smaller cell sizes mean larger mesh size and consequently longer simulation runtimes.

Note

The meshing log and the mesh are only visible once the simulation is finished. However, the time per iteration and the time to convergence are a lot lower compared to other solvers.

Your core hours will be consumed only after a successful
simulation run.

Once all the settings are defined, click on **‘Simulation Runs’** to begin the simulation.

After the simulation is finished the SimScale’s integrated post-processor can be used to visualize the mesh as well as the simulation results.

As explained under Simulation control > Convergence criteria, convergence plots are available for post-processing during and after the simulation run. The following images show convergence plots for residuals for a steady-state and a transient simulation of an Ercoftac pump respectively.

In Figure 16 the residual on the y-axis is a relative residual, the ratio between the residual at that iteration to the running maximum residual.

In Figure 17 the residual on the y-axis is a relative residual, the ratio between the residual at the last sub-iteration of that particular timestep to the running maximum residual.

For a Multi-purpose simulation, the mesh quality parameters can be viewed within the SimScale’s integrated processor. This allows the user to inspect mesh criteria and use this information to improve the mesh. The following mesh parameters are available.

- Volume Ratio
- Cell Volume
- Minimum Edge Length
- Non-Orthogonality
- Edge Ratio

Mesh criteria can be displayed using various filters. Figure 18 shows an example of the non-orthogonality displayed on a cutting plane through a centrifugal pump. Please find more information on mesh quality parameters and the suggested mesh quality values here.

An additional Field Output only available in a Multi-purpose simulation is the *Relative Velocity*. This field function is used to evaluate the velocity of the fluid relative to the rotational velocity of the rotating region. It is applicable only within the rotating zone and every other region is greyed out. The relative velocity is calculated as in equation 1.

$$ Relative \ Velocity = Local\ Velocity\ – Rotational\ Speed \times Local\ Radius \tag{1} $$

The *Local Velocity* is the velocity at the centroid of a cell within the rotating zone and the *Local Radius* is the distance of the centroid of the cell to the origin of the rotating zone. By multiplying the *Rotational Speed* of the rotating region with the *Local Radius* the *Local Rotational Velocity* is calculated. Thus the *Relative Velocity* is calculated by subtracting the *Local Rotational Velocity* from the *Local Velocity*.

Figure 19 shows an example of the *Local Velocity* in comparison to the *Relative Velocity*.

Did you know?

An advantage of using Multi-purpose analysis involving rotating flows is that power about the axis of rotation is directly output.

Last updated: October 22nd, 2024

We appreciate and value your feedback.

Sign up for SimScale

and start simulating now