Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

How to know a CFD Analysis solution get converged or not?

Hi ,

I have been conducting a CFD analysis of the air blower model using Simlab and the Acusolve solver. To estimate the first layer height of the boundary layer, I utilized the HM CFD Y+ calculator. Using this first layer height, I generated volume meshes with 5, 8, and 12 boundary layers, employing maximum mesh sizes of 2mm and 3mm, respectively. This resulted in six different meshed files.

For the solution, I used the Spalart-Allmaras turbulence model and selected steady-state as the solution type.

Initially, I performed the analysis using the 3mm mesh with three different boundary layers, the solution solved for 100 time steps (which is the default for steady-state problems). Subsequently, I analyzed the 2mm mesh model with 5 and 8 boundary layers, with the 12 boundary layer model currently running. Notably, the 2mm mesh with 5 boundary layers solved with 50 time steps, while the 8 boundary layer model reached 100 time steps.

The primary output of interest in this analysis is the volume flow rate. I observed that the volume flow rate varied significantly across the different mesh sizes and boundary layer configurations. How can I determine the final, most accurate output based on this analysis?

Additionally, how can I verify whether the solution has converged?

In general, what does "convergence" mean in the CFD simulations?

For reference, I have attached images of the residuals plot and the mass flux plot. Is it correct to assume the solution has converged if the residuals are within 1e-4, or is there another method to assess solution convergence?

Thanks & Regards,
Sivaprakash V.

Find more posts tagged with

AcuSolve

HyperMesh CFD

SimLab

Accepted answers

Jagan

Hi Sivaprakash,

Convergence and accuracy are two different aspects of a CFD solution. A converged solution can be obtained with a coarser mesh, but it may not accurately represent the real physics due to higher discretization errors. Refining the mesh helps minimize these errors and improves accuracy, which I believe is what you are doing.

To determine whether your CFD solution for a given mesh has converged, please refer to this https://help.altair.com/hwcfdsolvers/acusolve/topics/acusolve/training_manual/acusolve_convergence_criteria_r.htm and check if your residuals and solution ratios are within acceptable limits.

You can further reduce the convergence tolerance (e.g. set it to 0.0001) if your interested variables (flow rate, pressure) are not stabilizing as expected after a given number of iterations. However make sure to keep the convergence tolerance same for all the 6 mesh cases.

I believe you have attached the convergence data for only one case, is that correct?

acupro

Here is another discussion similar to that from the Help system Jagan posted earlier.

https://community.altair.com/discussion/41587/how-does-one-judge-the-convergence-of-an-acusolve-cfd-solution?utm_source=community-search&utm_medium=organic-search&utm_term=converge+acusolve

All comments

Jagan

If you're simulating the tutorial model, the SA turbulence model with standard wall functions should provide a sufficient solution without the need to resolve the boundary layer down to a Y+ value of 1. That said, refining the boundary layer further can improve accuracy, especially if your focus is on wall shear stress at the impeller.

As you perform grid refinement study, does the percentage change in the variable (volume flow rate, in your case) progressively decrease?

For example - if you make a mesh change and the solution of interest changes by 15% - maybe the previous mesh wasn't refined enough. Further if you refine the mesh and the variable of interest changes by 10% or lesser then you are going in the right direction.

Sivaprakash_V

Hi jagan,

I am mainly focused on volume flow rate of the air blower.

So performed the mesh independence study.

Then based on the above mentioned residuals and mass flow at inlet & outlet, how to determine the solution is converged or not?

I attached the values for your reference.

Based on the above results how I conclude my final output?
Thanks & Regards,
Sivaprakash V.

Jagan

Hi Sivaprakash,

I believe you have attached the convergence data for only one case, is that correct?

Sivaprakash_V

Yes, I attached the convergence data for one of the cases.

Are you review the table which I shared. It contains mesh size, BL and value of volume flow rate.

Sure, I will go through the convergence criteria.

Now based on the tables, can I confirm the final volume flow rate as 2.8 or 2.95.?

Thanks & Regards,

Siva prakash V.

Jagan

Have the residual and solution ratios of both solutions, where the flow rates are 2.8 and 2.93 m³/min, converged below the same limits (i.e. 1e-4)?

And is the flow rate value constant at 2.8 or 2.93 as the iteration progresses in both cases?

Sivaprakash_V

Yes, for both cases the residual and solution ratio with 1e-4.

Actuall, 2.8,2.8 and 2.93 are the volume flow rate values at 5,8 and 12 BL at two different Mesh sizes.

At the size of 2 and 3 mm, the value of volume flow is 2.8meter cube per minute for 5 and 8 layers respectively.

But for 12 BL, the values of volume flow rate got increased which reached 2.93 and 2.94 respectively.

Thanks & Regards,

Sivaprakash.

Jagan

Are the Y+ values, first layer height, and growth rate the same for the 5-8 BL and 12 BL cases?

Also is it possible for you to share a picture of the respective residual and solution ratios?

Sivaprakash_V

Hi Jagan,

Yes, the Y+ values, first layer height, and growth rate the same for the 5-8 BL and 12 BL cases.

I will share the screenshots of the residuals and solution graph for the cases which I performed.

Thanks & Regards,
sivaprakash V.

acupro

Sivaprakash_V

Hi Jagan,

This PDF contains the residual, solution & Mass flux Plot for my analysis.

PLOTS.pdf

Thanks & Regards,
Sivaprakash V.

Ovando_RBB

The convergence of a CFD model depends on the truncation error, which reflects how closely the numerical solution approximates the exact mathematical equations. When running a simulation, the solver iteratively refines the solution until the change between successive iterations falls below a user-defined numerical tolerance—this is where the truncation error acts as a threshold.

While it's possible to set an extremely tight truncation error (e.g., 1E-10), doing so doesn't automatically guarantee that your simulation results are accurate or physically meaningful. A simulation can converge mathematically but still fail to reflect real-world behavior, especially if the model setup or mesh resolution is inadequate.

To evaluate the accuracy of your CFD model, a more reliable approach is to perform a mesh sensitivity analysis. This involves running the same simulation with different mesh resolutions (typically labeled as coarse, fine, and very fine) while keeping all other parameters constant.

If your output variables (e.g., temperature, flow velocity, voltage) show minimal change across increasingly finer meshes, then your model is likely well-resolved. However, if the results differ significantly, especially between the fine and very fine meshes, it suggests that your current mesh is still too coarse to accurately capture the physical phenomena under study. In that case, refining the mesh further or adjusting the model setup may be necessary.

Sivaprakash_V

Hi,

During the mesh refinement study, We have two parameters 1) Mesh Size 2) Boundary layers.
If I change the mesh size, the boundary layer will affect and If I change the boundary layer the mesh will affect.

How to properly do these mesh refinement study in CFD Cases?

Ovando_RBB

Do you have a screenshot of the problem that you would like to analyze? that will give me more insight on to tell what you could possible do; understanding the physics of your application is the first step towards a successful FEA setup

Sivaprakash_V

Hi,

I’m interested in performing a CFD analysis of an air blower.
The design is similar to the one used in the Altair tutorial.

Thanks & Regards,

Sivaprakash.

Ovando_RBB

Are you solving the steady or transient formulation?

Sivaprakash_V

I am trying to solving Steady state analysis.