CFD Online Logo CFD Online URL
Home > Wiki > CONVERGE FAQ


From CFD-Wiki

Jump to: navigation, search

We hope you find the following FAQ helpful. For more information about many of the topics listed here, please review the CONVERGE documentation available on (login required). In particular, the CONVERGE Manual, CONVERGE Studio Manual, Getting Started Guide, and training slides may be especially helpful. In addition, the example cases (each consisting of a surface geometry and input parameters) in CONVERGE Studio can provide a useful starting point for your own cases.



What are the hardware and software requirements for CONVERGE and CONVERGE Studio?

Please refer to the Getting Started Guide for hardware and software requirements, installation instructions, and other related information.

Should I enable hyper-threading for my CONVERGE simulation?

CONVERGE, like other software packages that are designed to run on a large number of cores, does not run as efficiently when hyper-threading is enabled. This is true even when the number of processes in a simulation does not exceed the number of physical cores on the machine. For best performance, disable hyper-threading before running a CONVERGE simulation.

On Linux, what does the File locking failed in ADIOI_Set_lock</code error message mean? On Windows, what does failed MPI_fopen() mean?

On a Linux machine, this error may be the result of MPI interacting with an NFS-mounted file system. To be able to use mpi_write_flag = 1 on an NFS-mounted file system, use NFS version 3.0+ and ensure that the client machine is mounted to the file system with the noac (no attribute caching) option.

I see that CONVERGE offers various MPI implementations (MPICH2, HPMPI, OPEN MPI, PMPI). Which one should I use?

Based on some internal testing of ICE cases, we have found that OpenMPI may be the fastest. However, OpenMPI is not always forward/backward compatible. Different major CONVERGE versions may require different OpenMPI installations. PMPI gives the best compatibility across different versions. Please note that results may vary due to different release versions of each MPI implementation.

Can CONVERGE run on GPUs?

Currently the CONVERGE solver does not run on GPUs. Convergent Science engineers are actively working on porting the SAGE detailed chemistry solver to GPUs.


My therm.dat file contains multiple entries of the same species. Which entry does CONVERGE use?

CONVERGE uses the first entry and ignores any subsequent entries for that species. If you validate your therm.dat file in CONVERGE Studio before running a simulation, CONVERGE Studio will offer several ways to resolve duplicate entries.

Why don’t results from one version of CONVERGE always match results from an older version of CONVERGE?

Each version of CONVERGE contains numerous enhancements and bug fixes, and these changes may affect simulation results. Please see the release notes (available on for specific information about changes to CONVERGE. Convergent Science engineers can explain why results may have changed and suggest ways to more closely match results from previous versions (contact

My RANS simulation shows cycle-to-cycle variation. Is this variation to be expected?

Yes. A well-resolved unsteady RANS simulation does not smear all perturbations and thus can predict cyclic variations. An example of this phenomenon is GDI engines that show high cycle-to-cycle variation in measured cylinder pressure data. The following publications contain details on this topic.

  • Jupudi, R., Finney, C., Primus, R., Wijeyakulasuriya, S., Klingbeil, A.E., Tamma, B., and Stoyanov, M.K., “Application of High Performance Computing for Simulating Cycle-to-Cycle Variation in Dual-Fuel Combustion Engines," SAE Paper 2016-01-0798, 2016. DOI:10.4271/2016-01-0798
  • Richards, K., Pomraning, E., Senecal, P.K., Scarcelli, R., and Wallner, T., “Cyclic Variation in Unsteady RANS Engine Simulations,” International Multidimensional Engine Modeling Users’ Group Meeting at the SAE Congress, Detroit, MI, United States, April 20, 2015.
  • Richards, K., Probst, D., Pomraning, E., Senecal, P.K., and Scarcelli, R., “The Observation of Cyclic Variation in Engine Simulations When Using RANS Turbulence Modeling,” Proceedings of the ASME 2014 Internal Combustion Engine Division Fall Technical Conference, ICEF2014-5605, Columbus, IN, United States, October 19-22, 2014.
  • Scarcelli, R., Matthias, N.S., and Wallner, T., “Numerical and Experimental Analysis of Ignition and Combustion Stability in EGR Dilute GDI Operation,” Proceedings of the ASME 2014 Internal Combustion Engine Division Fall Technical Conference, ICEF2014-5607, Columbus, IN, United States, October 19-22, 2014.
  • Scarcelli, R., Richards, K., Pomraning, E., Senecal, P.K., Wallner, T., and Sevik, J., “Cycle-to-Cycle Variations in Multi-Cycle Engine RANS Simulations," SAE Paper 2016-01-0593, 2016. DOI:10.4271/2016-01-0593.
  • Scarcelli, R., Sevik, J., Wallner, T., Richards, K., Pomraning, E., and Senecal, P.K., “Capturing Cyclic Variability in EGR Dilute SI Combustion Using Multi-cycle RANS,” Proceedings of the ASME 2015 Internal Combustion Engine Division Fall Technical Conference, ICEF2015-1045, Houston, TX, United States, November 9-11, 2015.

How do I obtain more repeatable answers from my RANS multi-cycle simulation?

By changing some numerical settings, you can force predictions to be more repeatable. Increasing numerical viscosity in the solution will dampen perturbations. Increasing cell sizes and using lower-order discretization schemes can increase the repeatability of a solution. It is important to note, however, that these changes may reduce accuracy.

How can I see how long CONVERGE spends on different processes (e.g., spray, combustion, and load balancing)?

In CONVERGE Studio, go to Simulation Parameters > Run parameters > Misc and set the Screen print level to verbose or more verbose. You will see output such as the following: Time for ncyc 41 = 3.89 seconds load balance = 0.00 seconds ( 0.00%) solving transport equations = 3.37 seconds (86.50%) move surface and update grid = 0.01 seconds ( 0.16%) combustion = 0.00 seconds ( 0.00%) spray = 0.06 seconds ( 1.60%) writing output files = 0.27 seconds ( 6.89%)

Are closed-cycle simulations sufficient for modeling diesel engines?

It is important to simulate the induction in order to accurately characterize the velocity field. It is possible to run the intake simulation and map that solution at IVC for the closed-cycle simulation rather than assuming constant initial flow conditions.

How do I find Convergent Science’s recommended settings for different types of simulations?

Please refer to the example cases. In CONVERGE Studio, go to File > Load example case. These cases are also available at (login required).

I ran two simulations with identical settings except that one simulation was initialized via mapping. Why are the results from these two simulations not the same?

The mapping data file does not save grid information and thus CONVERGE does not map data into the same cells. Instead, in a simulation with mapping, CONVERGE initializes each cell with data from the nearest point in the mapping data file. This process may result in some data smearing (i.e., several cells in the new simulation may be initialized with data from the same point in the map file). In addition, the AMR resolution from the old grid is not carried over to the new simulation. These differences are the reasons that the results are not identical.

Does Convergent Science recommend running an LES simulation at RANS grid settings?

No. An LES simulation will require smaller cell sizes.

What CONVERGE quantity can be compared against measured mass flow rate data at the intake port?

CONVERGE writes mass flow at the valves to regions_flow.out. CONVERGE writes mass flow rates from the inflow and outflow boundaries to mass_avg_flow.out and area_avg_flow.out.

What are some of the pre-processing requirements and recommendations for a four-stroke engine surface data file?

We recommend moving the piston to BDC (note that the piston must be at BDC if you are using a CONVERGE-calculated piston motion profile). The valves must be in an open position. We recommend aligning the cylinder axis with the z axis. We recommend that the fire deck be at z = 0.0. Ensure sufficient resolution for the surface triangulation.

How can I accelerate my steady-state simulations?

The steady-state solver in CONVERGE 2.4 is a density-based pseudo-time-stepping solver that can be used for solving a wide range of steady flow simulations (internal/external flows, combustion, sprays and films, CHT, MRF, surface chemistry, etc.). The solver allows the use of higher CFL numbers and also automated solver control for certain simulation parameters (CFL numbers, solver tolerances, and grid sizes). Both of these features help reduce the computation cost of your simulation.

Please consult the CONVERGE 2.4 Manual for recommended parameters for steady-state simulations. Remember that these values may require modification for some cases. Some general recommendations are given below.

We recommend initiating your steady simulation with a relatively coarse grid (grid_scale = -1 or -2 in, so as to allow the initial transients to be rapidly flushed out of the domain. Time-based or automated grid scaling should be used, although care should be taken to ensure that the grid always remains adequately refined in regions in which the flow is complex.  The maximum CFL number can be set to approximately 20 to 30 for non-reacting flows and approximately 10 to 15 for reacting flows. If the solver has excessive recoveries, you can reduce the CFL number. If automated control is activated, the solver will perform this action on its own.  Monitoring a few flow variables is useful for determining convergence in a steady simulation and can be used for automatically controlling grid scaling or solver settings. We recommend monitoring variables at OUTFLOW boundaries (temperature, mass flow rate, and species concentration), within the domain (maximum, minimum, and mean pressure and temperature; species concentration; and spray mass), or at monitor points (velocity, pressure, and temperature). The initial velocities and pressures and the corresponding INFLOW boundary conditions should be as consistent as possible. For instance, if the inflow velocity is 1 m/s, then the initial condition should be 1 m/s as well.

My case crashed due to a problem with sealing. What should I do?

Check the following items. The moving part and the seal-to part should not intersect during the entire process. The moving part and the seal-to part should be aligned in the moving direction and in the azimuthal direction. The gap between the moving part and the seal-to part should be smaller than the sealing tolerance by about one order of magnitude. The sealing tolerance should not be too large. (Typical sealing tolerances are 0.01 to 0.1 mm for an engine case.) CONVERGE contains a sealing test utility (converge –l) that allows you to quickly identify errors in the sealing setup. For more information about this tool, please consult the CONVERGE Manual.

When do you recommend using the real gas equation of state?

We recommend the real gas equation of state for all simulations.

Can I use multiple boundary embeddings for the same boundary at different times?

CONVERGE does not allow multiple boundary embeddings for a single boundary. You can, however, accomplish the same effect by adding a box or cylinder embedding.

Can I set up monitor points that moving with the piston or other moving boundary in my simulation?

Yes. CONVERGE 2.4+ contains a monitor points option in which points placed on a moving boundary will move with that boundary. To set up this feature in CONVERGE Studio, go to Output/Post-Processing > Monitor points.

How do I obtain the desired compression ratio?

CONVERGE Studio 2.4+ contains a compression ratio calculator (go to Applications > IC engine > Compression Ratio). You can also use this tool to move the piston to a location that yields the desired compression ratio. If you are using CONVERGE Studio 2.3 or earlier, please consult Chapter 19 of the CONVERGE 2.3 Manual for directions on calculating the compression ratio and moving the piston to the desired location.


My simulation runs slowly. How can I identify the cause?

There can be many reasons that may cause a simulation to run more slowly than expected. First, look at the log file (or at time.out, for CONVERGE 2.3+) to see what is limiting the time-step. If screen_print_level = 3 in, CONVERGE records in the log file and in time.out the time spent on each major routine (combustion, spray, load balancing, moving grids, etc.). These data can shed some light on the slowdown. Some of the major contributors to a slow simulation are too many parcels in a spray simulation, a large chemical mechanism in a combustion simulation, and poor load balancing. You can also review metis_map.out and cell_count_ranks.out to understand and determine how to improve the load balancing.

The time-step in my simulation is limited by dt_cfl. How can I accelerate my simulation?

When the variable time-stepping algorithm is used, CONVERGE controls the time-step by the user-specified CFL numbers (among other limiting criteria). When the convective CFL number limits the time-step, it may be due to smaller cell sizes or high flow velocities. You can use a region- and temporal-based CFL number to increase the time-step when important events are not occurring. For example, set dt_cfl = 1 during combustion and increase it to 4 during the exhaust phase. Refer to the SI8_engine_PFI_SAGE example case (in CONVERGE Studio, go to File > Load example case) to see a demonstration of this technique. Turning off embedding during less important times of the simulation (or in less important parts of the domain) may also help alleviate this restriction.

How can I speed up my multiple-cycle engine simulations?

CONVERGE features such as skip species, region- and temporal-based convective CFL number, and region- and temporal-based AMR can speed up multi-cycle engine simulations. The SI8 engine CHT example case includes these features.

My simulation slows down significantly when spray starts. What should I do?

A slowdown when the spray starts is expected, but there are some steps to take if you are concerned. First, try reducing the number of parcels. Note that the specified number of parcels in is for a single nozzle, while the injected mass is for the entire injector. If you dramatically reduce the number of parcels, you should check how sensitive the predictions are relative to the injected number of parcels. If collision is turned on, verify that multiple nozzles do not reside in a single cell.

My turbomachinery simulation time-step is limited by dt_move. How can I make this simulation run faster?

A time-step limited by dt_move is a typical bottleneck in high speed turbo-machinery simulations. This time-step limit was put in place primarily for stability reasons. There are two options to try to get around this bottleneck and speed up your simulation: increase the cell sizes at the moving boundaries or relax the dt_move constraint. Note that either of these workarounds can affect the solution accuracy and stability.

The swept cell volume of any moving boundary is limited to a portion of cell in a single time-step. The default value in CONVERGE is 0.5 (i.e., in a single time-step, the moving boundary cannot sweep more that 50% of the smallest cut-cell volume). You can use values greater than 1.0, although higher values might affect solution stability or accuracy. To change this value in CONVERGE Studio 2.4+, go to Simulation Parameters > Simulation time parameters > Moving boundary time-step multiple.

How can I check the status of my simulation?

Look at the time.out file, which is available in CONVERGE 2.3.10+. You will find the wall time per time-step, which tells you how much time is being spent at each time-step or cycle. This quantity can give you an idea if your simulation is slowing down. You can also see if there are any recoveries in the simulation and what is causing the recoveries. The time.out file also contains the time-step size, what is limiting the time-step, and the values of the CFL numbers at each time-step.

Will the triangle count in my CAD file affect my simulation’s runtime?

Yes, especially for cases with moving boundaries. CONVERGE generates the grid at each time-step, and there is a computational cost in trimming Cartesian fluid cells. If a geometry contains an unnecessarily high triangulation, we recommend coarsening the surface to reduce the number of triangles while retaining the surface features. CONVERGE Studio contains a coarsening tool.

Think of it this way: a rectangle can be defined by two triangles. Alternatively, a poor CAD algorithm can define a rectangle of the same area by 1 million small triangles. This huge triangle addition can slow down simulations. For typical engine geometries, keep the triangle count around 0.3 to 0.5 million.

By looking at cell_count_ranks.out, it is clear that the load balancing of my simulation is not optimal. How can I improve the load balancing?

CONVERGE distributes blocks of cells rather than individual cells. A value of parallel_scale = -1 in yields the highest number of blocks for domain decomposition. Try increasing parallel_scale (e.g., from -2 to -1). Also, larger embed scales in fixed embedding and AMR can also make load balancing difficult, and thus reducing the embed scale and the base mesh size can allow you to achieve better load balancing while maintaining the same smallest cell size. Even though this approach will increase the total number of cells, the case may run faster due to better load balancing. Chapter 11 in the CONVERGE Manual gives a great example of how reducing the base mesh size can reduce the cell count on the highest-loaded rank.

What is the non-transport passive CHEM_STIFF?

CONVERGE allows the use of stiffness-based load balancing for simulations that use the SAGE detailed chemistry solver (stiffness-based load balancing is required for SAGE simulations without adaptive zoning and optional for SAGE simulations with adaptive zoning). Any simulation that uses stiffness-based load balancing must contain the non-transport passive CHEM_STIFF in the file.

My simulation spends quite a bit of time on load balancing. Why?

If a significant amount of time is spent on load balancing, it is likely due to a large number of parallel blocks (see metis_map.out). Reduce parallel_scale (e.g., from -1 to -2) and rerun the simulation. Check that the new load balance at the reduced parallel_scale is still adequate.

What is the optimum number of cells/processor for a typical ICE simulation?

Having at least 50,000 cells/core has been observed to give good parallel speedup.

How often does CONVERGE do load balancing?

The load_cyc parameter in controls the frequency of load balancing. In addition, CONVERGE load balances each time a fixed embedding changes (either refined or released) and at the start of a simulation (new simulation, mapping, or restart) a load balancing event is done.

I see that CONVERGE offers various MPI implementations (MPICH2, HPMPI, OPEN MPI, PMPI). Which one should I use?

Based on some internal testing of ICE cases, we have found that OpenMPI may be the fastest. However, OpenMPI is not always forward/backward compatible. Different major CONVERGE versions may require different OpenMPI installations. PMPI gives the best compatibility across different versions. Please note that results may vary due to different release versions of each MPI implementation.

Can CONVERGE run on GPUs?

Currently the CONVERGE solver does not run on GPUs. Convergent Science engineers are actively working on porting the SAGE detailed chemistry solver to GPUs. 


There is burning in the intake port in my G-Equation simulation. Why?

The G-Equation combustion model is active when the G_EQN passive is set to zero, and thus the entire simulation domain and the INFLOW and OUTFLOW masses must be set to a negative G value to avoid initializing flames from unintended locations. Refer to the SI8_engine_premix_GEQN example case (in CONVERGE Studio, go to File > Load example case) for example settings.

Note that, in CONVERGE 2.3 and earlier, combustion is either on or off for the entire simulation. For 2.4+, however, combustion has user-specified start and end times (combust_start_time and combust_end_time in

There is burning in the intake port during the second cycle of my G-Equation simulation. The first cycle did not have this problem. Why is there burning in the second cycle?

Before the fresh unburned mixture enters the cylinder at the start of the second cycle, the entire simulation domain should be reinitialized with a negative value of G. To set up this option in CONVERGE Studio, go to Physical Models > Combustion modeling > G-Equation > Additional… > Initial G-value and select the Use file option. Refer to the SI8_engine_premix_GEQN example case (in CONVERGE Studio, go to File > Load example case).

Should I use temperature AMR in a G-Equation combustion simulation?

In simulations with the SAGE detailed chemistry solver, temperature AMR is used to resolve the flame front so that the flame propagation speeds (and thus the fuel burn rates) are correct. However, in the G-Equation model, the flame speeds are determined from a flamespeed correlation and so we recommend NOT activating temperature AMR. This will reduce the total cell count and allow the simulation to run faster. Note that CONVERGE does not prohibit the use of temperature AMR in a G-Equation simulation.

What laminar and turbulent flamespeeds are used in SAGE?

Unlike many simplified combustion models, the SAGE detailed chemistry solver does not calculate laminar and turbulent flamespeeds directly. When using SAGE for calculating premixed combustion, the turbulent flamespeed is the result of the chemical reaction rates (from the mechanism file, e.g., mech.dat) and the enhanced mixing from the turbulence model.

How can I have CONVERGE write out laminar and turbulent flamespeeds in my SAGE simulation?

You can use the flamespeed correlations in the G-Equation combustion model. When you set up your simulation in CONVERGE Studio, go to Output/Post-Processing > Post variable selection > Cells and select Laminar Flame Speed and Turbulent Flame Speed. You must also select the desired correlations in Physical Models > Combustion modeling. Note that these calculated flamespeeds are not used in the SAGE calculations and give only an approximation of the flamespeeds that result from the SAGE solver.

My high-EGR case does not burn well with the same chemical kinetics mechanism that gave me good predictions for no- or low-EGR cases. What should I do?

This is a limitation of the mechanism. It is likely that the mechanism was not validated against ignition delay and laminar flamespeed data under high-EGR conditions. If such data are available, CONVERGE 2.4+ contains a mechanism tuning tool (that sets up input files for genetic algorithm optimization) that can change the reaction rate coefficients to match the high-EGR data. See the CONVERGE 2.4 Manual for more details about this feature.

What parameters are available to increase or decrease the burn rates in a SAGE simulation?

We recommend reviewing the grid and boundary condition settings for accuracy before trying to tune the reaction rates. The Reaction multiplier option can be used to increase or decrease fuel burn rates (in CONVERGE Studio, go to Physical Models > Combustion modeling > Models (SAGE) > SAGE Parameters). The turbulent Schmidt number can be reduced to enhance mixing and thereby increase burn rates (go to Materials > Global transport parameters).

The NOx emissions in emissions.out and species_mass.out are not identical. What is the difference between these quantities?

The NOx emissions in emissions.out are from the extended Zel’dovich mechanism, which is hard-coded in CONVERGE. The calculated NO mass is multiplied by a factor of 1.533 to output NOx mass. This output is available even if you are not solving detailed chemistry. If you are using the SAGE detailed chemistry solver and if the chemical mechanism includes NOx species and reactions, then those species masses are recorded in species_mass.out. The NOx mass calculated using SAGE might not match exactly with that calculated using the extended Zel’dovich mechanism. In the passive NOx model, radicals [O] and [OH] can be assumed to be at equilibrium, while species NOx does not make such an assumption. This assumption in the passive NOx model is valid only at high temperatures (T > 2200 K). Quantities solved outside of this requirement might be responsible for the different NOx emissions data.

The lower heating value (LHV) of the fuel used in the experiments is different from the fuel surrogate used in the simulation. How can I correct this?

In CONVERGE 2.4+, you can specify LHVs for individual species. The data in the thermodynamic data file (e.g., therm.dat) will be adjusted to recover the user-specified LHV. To set up this option in CONVERGE Studio, go to Materials > Gas simulation and check Lower heating value. Open the accompanying dialog box to specify the species-specific LHVs.

How can I calibrate the ignition delay in the Shell ignition model?

In CONVERGE Studio, go to Physical Models > Combustion modeling > Models (CTC/Shell) and adjust the Ignition delay constant (af04). Increasing this value will reduce the ignition delay.

Can the RIF model be used to simulate premixed combustion in CONVERGE?

No. CONVERGE’s RIF model can be used only for non-premixed combustion.

Does the RIF model require an auto-ignition model in order to simulate diesel combustion?

No. CONVERGE’s RIF model uses the provided chemical kinetics mechanism to capture ignition delay.

Does CONVERGE use pre-compiled flamelet libraries (lookup tables) or does CONVERGE solve the kinetics in the mixture fraction space on the fly?

For the FGM model, CONVERGE uses pre-compiled flamelet libraries. For the RIF model, CONVERGE solves the kinetics in the mixture fraction space on the fly.

Does the RIF model in CONVERGE support unsteady and multiple flamelets?


Can I use the same mechanism for the SAGE detailed chemistry solver and the RIF model?

Yes, but note that you cannot run both SAGE and RIF in a single simulation.

What advantage do the simplified combustion models have compared to the SAGE detailed chemistry solver?

The simplified combustion models are generally faster than SAGE.

Do the phenomenological, PM, and PSM soot models work with the RIF combustion model?


Which species and reactions are considered in the CTC model?

The CTC models considers CO, H2, CO2, O2, H2O, N2, and the fuel. Chapter 13 of the CONVERGE Manual describes the reactions in the CTC model.

Which parameters should I change to calibrate the CTC model?

Increasing the Turbulence time-scale constant will decrease the rate of combustion. You can also adjust the Chemical time-scale constant. To change these parameters in CONVERGE Studio, go to Physical Models > Combustion modeling > Models (CTC/Shell).

How can I avoid having my soot values oscillate close to EVO?

You can tighten the passive tolerance. More generally, however, we recommend ending combustion before EVO.

Can I predict engine knock using the G-Equation model?

Yes, you can predict engine knock via G-Equation as long as you are using a version of the G-Equation model that includes the SAGE detailed chemistry solver outside of the flame front (the G = 0 surface). In CONVERGE Studio, go to Physical Models > Combustion modeling > Models (G-Equation) > Models and select one of the options that includes SAGE outside of the flame front.

When using ECFM3Z, how can I generate my own TKI tables?

Generating your own TKI tables is an advanced option. Please contact the CSI Applications Team ( for more information.

Can I set up ECFM+TKI for knock simulations?

Yes, ECFM+TKI is available in CONVERGE 2.3+.

Should I use ECFM or ECFM3Z for GDI/PFI engines?

For GDI/PFI engine simulations, you should use ECFM. Be sure to run your simulation on CONVERGE 2.3.20+.

How can I convert a map.out file from a SAGE simulation for use with an ECFM simulation?

Please contact the Applications Team ( to obtain a script for this conversion.

How do I account for the fuel’s cetane number?

When using the SAGE detailed chemistry solver, you can use a fuel blend that has the same cetane number as the fuel used in the experiments. It is important to ensure that all of the surrogate fuel species are available in your chemical kinetics mechanism. When using the CTC/Shell model for diesel combustion, one of the reaction rates in the shell model can be made a function of the cetane number via a user-defined function. For details, please see the following paper: Ayoub, N. and Reitz, R., "Multidimensional Modeling of Fuel Composition Effects on Combustion and Cold-Starting in Diesel Engines," SAE Technical Paper 952425, 1995, doi:10.4271/952425

How do I account for a fuel’s Research Octane Number (RON)?

When using the SAGE detailed chemistry solver, you can use a fuel blend that has the same RON as the fuel used in the experiments. It is important to verify that all of the surrogate fuel species are available in your chemical mechanism.

Typically nC7H16 and iC8H18 are blended to achieve the desired RON, and Convergent Science can provide mechanisms that include these two species. Contact

Can CONVERGE tune kinetic mechanisms to match ignition delay and laminar flamespeed data?

Yes. CONVERGE 2.4’s mechanism tuning tool can be used to optimize mechanisms to match ignition delay and laminar flamespeed data for multiple operating points. Please see the CONVERGE 2.4 Manual for more details.


Although my multi-hole injector is symmetric, the spray penetration patterns from each nozzle are not identical. The spray plumes aligned with the grid seems to penetrate more than the non-aligned plumes. Why?

This phenomenon is caused by numerical viscosity associated with large computational cell sizes. A spray injected along the diagonal of a cubic cell is subjected to more numerical viscosity than a spray aligned with the edges of the cells. This effect diminishes as the cells are refined. For more information, please refer to the Convergent Science white paper on numerical viscosity (available for download at

Must I increase the number of spray parcels when I refine the grid?

Yes. If the cell size is reduced and the number of parcels stays constant, then the amount of liquid in a cell increases, which tends to artificially increase gas velocities. You can use 1.5e-10 kg/parcel as a guideline for 0.35 mm cell size (i.e., the grid settings that are given in our diesel engine sector example cases [in CONVERGE Studio, to go File > Load example case]). Each time the cell is refined one level (e.g., embed_scale changes from 2 to 3), you should increase the number of parcels injected by at least a factor of 4. Please consult the following publication for more details: Senecal, P.K., Pomraning, E., Richards, K.J., and Som, S., “Grid-Convergent Spray Models for Internal Combustion Engine CFD Simulations,” Proceedings of the ASME 2012 Internal Combustion Engine Division Fall Technical Conference, ICEF2012-92043, Vancouver, BC, Canada, September 23-26, 2012. DOI:10.1115/ICEF2012-92043

Which pressure should be used to calculate parcel velocities in the spray rate calculator?

In order to calculate the parcel velocities that come out of the nozzle hole, we recommend using the difference between the injector sack pressure and the back pressure (cylinder pressure).

When using Lagrangian spray parcels (and not modeling the injector internal flow), how do I incorporate the incoming turbulence from the fuel injector into the domain?

This is an active area of research, and CONVERGE 2.3+ includes a VOF-spray one-way coupling feature. In VOF-spray one-way coupling, you first run a VOF simulation (without Lagrangian spray modeling), after which CONVERGE writes a file that contains velocity, turbulence, temperature, and other data from the nozzle exit. Next you run a Lagrangian spray simulation in which CONVERGE initializes the spray parcels with the data from the VOF simulation. The turbulence at the nozzle exit (from the VOF simulation) is mapped to the gas and parcel phrases in the Lagrangian spray simulation. CONVERGE 2.4+ contains the Eulerian-Lagrangian Spray Atomization (ELSA) model, which is a spray injection model that combines Eulerian multi-phase modeling and Lagrangian particle tracking methods. For more information about VOF-spray one-way coupling and the ELSA model, see the CONVERGE 2.4 Manual.

In the Kelvin-Helmholtz model, is the Shed mass constant (in CONVERGE Studio, Physical Models > Spray modeling > Injectors > Models) applied only to blobs or is it applied to any droplets subjected to a breakup event?

This parameter is applied to all droplets in the domain that are undergoing KH breakup.

Does the Kelvin-Helmholtz model act only on blobs or does it also act on the first generation of child droplets (i.e., the droplets derived from the primary breakup)?

The KH model acts on all drops.

Is it correct to apply the Kelvin-Helmholtz model to the breakup of child droplets (i.e., not blobs), when the KH theory refers only to the disintegration of liquid jets (i.e., blobs)?

The KH model assumes that the fastest growing surface wave is much smaller in magnitude than the surface on which it grows, and thus it does not matter if it grows on a liquid sheet, a ligament, or a spherical drop.

How are primary and secondary breakup simulated in the modified KH-RT model?

Primary breakup is simulated via the KH model. For secondary breakup, the KH and RT models compete against one another.

In the KH-RT model, which parameters can be adjusted to change the drop size?

You can adjust several KH and RT parameters. In CONVERGE Studio, go to Physical Models > Spray modeling > Injectors. Click Edit to open the [Injector #] configuration dialog box. All of the parameters below are in that dialog box. RT model size constant (rt_const3): Increase this value to increase both the drop size and the penetration. RT model time constant (rt_const2b): Increase this value to increase the drop size. KH shed mass constant (kh_shed_factor): Reduce this value to increase the drop size. KH model breakup time constant (kh_const2): Reduce this value to make drop breakup happen more quickly. KH model size constant (kh_balpha): Increase this value to increase the drop size.

How are the blobs initialized when the Injection drop distribution is based only on nozzle size and the discharge coefficient model uses a varying nozzle velocity coefficient?

CONVERGE dynamically calculates the velocity coefficient based on the injection pressure at that time. CONVERGE then calculates the contraction coefficient (Ca) from the following relationship.


In the equations above, d_0 and d_eff are the nominal and effective nozzle diameters.

(To set up these options in CONVERGE Studio, go to Physical Models > Spray modeling > Injectors > Time/Temp/TKE/EPS/Mass/Size > Main and set Injection drop distribution to None and go to Injectors > Models and set Discharge coefficient model to Use correlation for Cv.)

When should I use a spray-wall interaction model?

You should use a spray-wall interaction model whenever the spray impinges on a wall.

Are there any guidelines on the meshing requirements for spray-wall interaction models?

CONVERGE has no special meshing requirements for the spray-wall interaction models. You can use the typical grid recommendations.

Are there any guidelines on the number of parcels relative to the injected mass?

There are no strict guidelines, although 1.5e-10 kg/parcel is a general recommendation that is appropriate when cell sizes on the order of 0.35 mm. Note that this value is an estimate and should not be taken as a strict rule. Refer to the following paper for more details:

  • Senecal, P.K., Pomraning, E., Richards, K.J., and Som, S., “Grid-Convergent Spray Models for Internal Combustion Engine CFD Simulations,” Proceedings of the ASME 2012 Internal Combustion Engine Division Fall Technical Conference, ICEF2012-92043, Vancouver, BC, Canada, September 23-26, 2012. DOI:10.1115/ICEF2012-92043

Can a single liquid parcel species evaporate into multiple gas-phase species?

Yes, this can be done using composites, which are composed of multiple base species. To set up composites in CONVERGE Studio, go to Materials > Composite species.


For 1DCHT cases, how can I view the surface temperature in a post-processor?

bound_temp in gives the surface temperature. 

Can CONVERGE seal surfaces on an INTERFACE?

At this time, CONVERGE does not allow sealing on an INTERFACE. 

What interpolation method does CONVERGE use for spatial boundary condition profiles?

CONVERGE does not interpolate for spatial boundary condition profiles. Instead, CONVERGE obtains information from the nearest data point.

How can I obtain surface-averaged data on individual boundaries? 

In CONVERGE Studio, go to Case Setup > Output/Post-Processing > Output files > Output generation and select Generate WALL boundary-averaged output. This option will generate a series of files named bound*-wall.out.

What is the difference between monitor points and super-cycle monitor points? 

Monitor points are locations in the domain at which CONVERGE collects data during the simulation. The general monitor point option ( or Case Setup > Output/Post-Processing > Monitor points) allows you to place points throughout the domain and to select from a variety of variables to be monitored at those locations. CONVERGE writes monitor point data at each time-step.

Super-cycle monitor points ( or Case Setup > Physical Models > Super-cycle modeling) provide temperature data from specific locations within the solid domain. CONVERGE writes super-cycle monitor point data at each super-cycle.

When I run a CHT case, I see the following warning message: Problem with the number of regions in rank #. Is this a problem? 

This message is commonly seen in CHT simulations and does not indicate a problem. This message should not cause a crash or impact simulation results or runtime.

When I run a CHT case, my case crashes and I see the following error: The surface has a non-interface triangle that is only connected to a single interface triangle. What is the problem? 

This error is often related to an incorrect INTERFACE assignment. An edge can be shared by two triangles only if both triangles are non-interface or if both triangles are interface. CONVERGE does not allow an edge to be shared by one interface triangle and one non-interface triangle.

When I run a CHT case, my case crashes and I see the following error: Neighboring triangles are associated with different streams. What is the problem?

This error is often associated with an INTERFACE boundary. For an INTERFACE boundary, the surface normal of all triangles in that boundary must point toward the same region and that region must be consistent with the information in the boundary definition file (in CONVERGE Studio, go to Boundary Conditions > Boundary to set up this region). You may see the error specified above if a single surface normal points in the wrong direction.

How can I output the prescribed heat transfer coefficient to the post*.out files?

This option is not available in CONVERGE 2.3. In CONVERGE 2.4+, include bound_htc in (Case Setup > Output/Post-Processing > Post variable selection).

I am comparing heat transfer coefficients (HTCs) from CONVERGE with HTCs from other codes and they do not match. Why?

In CONVERGE, the HTC is a local value based on the near-wall cell temperature, not a free-stream temperature. This HTC differs from an HTC that is based on a user-specified reference temperature, and it also differs from an HTC that could be estimated from a Nusselt number correlation. Because HTC definitions vary from code to code and because CONVERGE uses local HTC values that depend on the near-wall mesh, we recommend instead comparing flux.

Can we perform an all-in-one coolant/combustion/solid simulation?

Currently CONVERGE does not allow three phases in the same simulation and thus the coolant/combustion/solid combination is not allowed. This combination needs to be separated into two simulations (for example, a gas/solid CHT simulation and a liquid simulation).

Can I use super-cycling on a non-engine case? If so, how do I set supercycle_stage_num and supercycle_stage_interval?

CONVERGE allows super-cycling on non-engine cases. As long as the temperature of the solid part can be approximated as steady state, you can use super cycling to get steady state solid temperature distribution faster than a normal transient simulation. For example, if you have a nozzle in a tunnel that spraying water into the air flow for 1 minute in every 10 minutes. You can set supercycle_stage_num as 1 and supercycle_stage_interval to 10 minutes to get a steady state temperature distribution in the solid tube wall through super-cycle. If the simulation has temporally periodic variation in its behavior (for example, as in an engine), supercycle_stage_num*supercycle_state_interval must equal the cyclic period.

What is the convection temperature boundary condition?

In CONVERGE, you can set a convection boundary condition for either a solid or a fluid WALL boundary. In either case, the convection boundary condition prescribes the convection between the wall and the environment (note that the environment is not included in the computations). Note that there is an additional piece of information that you must specify for this type of boundary condition when used for a fluid WALL: you must declare the temperature wall treatment used inside the domain (i.e., Law-of-the-wall, Dirichlet, or Neumann).

My wiki