Mesh convergenge study
 

Hi,
I am doing a mesh convergence study of my transient COMSOL CFD model of the blood flow within the left ventricle of the heart. I have solved the simulation for 7 different mesh sizes (pre-defined in COMSOL).
I choose the velocity magnitude as my metric, and integrate it over the whole domain for each time instance. When I am plotting the result, do I see a tendency; finer mesh, higher velocity. And this tendency does not seems to converge.... The same tendency is seen for pressure and shear rate as metric. If I choose parameters as volume or area, do I not see the tendency. Hence I am pretty sure, it is something flow-related.
I am trying to find out whether i need an even finer mesh, or why it does not converge.

I will attach the numbers of degrees of freedom and the plot showing the tendency.



Any suggestion to the behaviour?

Kind regards,
Pernille

1) I would not use such integral to assess a mesh sensitivity
2) How do you compute such integral?
3) The plot in time seems quite acceptable.


Increasing the number of nodes increases the resolution over the walls so that the velocity profile is better described

Hi FMDenaro


Thank you so much for the fast reply.



1) I would not use such integral to assess a mesh sensitivity
- Okay. Do you have an idea to a better metric?



2) How do you compute such integral?
- I do not know if you know COMSOL, but under DERIVED VALUES, do I calculate an volume integral over the parameter spf.U, for the whole domain.


3) The plot in time seems quite acceptable.
- But would you not suppose that graph should become close an closer?


Again, thank you for taking time to help me.


Kind regards, Pernille.

If I see correctly the colours, "fine" and "finer" solutions seems tending towards a convergence

There isn't enough of a significant difference between your grids to suggest convergence is occurring.

Take a look at the Procedure for Estimation and Reporting of Uncertainty Due to Discretization in CFD Applications

http://fluidsengineering.asmedigital...icleid=1434171

Specifically check out the discussion around equations 1 and 2, and the step 2 discussion.

I have a experience to simulate COMSOL about 3 months.
COMSOL CFD is really different comparing other major software..(FLUENT, STAR-CCM+, CFD-ACE+...)

I also experienced too serious convergence problem to solve turbulent flow.
I'm not sure that was my immature skill for COMSOL, it was very hard to get convergenced solution.

FMDenaro: I see what you mean, but I would also say, that it depends a lot of the time instance. And I do not find a reason for that. If I sum up the values for each graph and plot them as point, is the tendency not that clear (see attached image).

Thank you for your help!


lcarasik: Thank you for the article. That is interessting! COMSOL defines h as the longest edge in the element. The refinement factor between the 7 mesh-size is then: 0.9 0.8 0.8 0.8 0.7 0.7. e.g. not higher than 1.3 as suggested. But still; if I compare Extremely coarse with Coarser, Coarser with Normal, and lastly Normal with Finer, then is the refinement factors higher than 1.3. So the significant these meshes should be high enough to convergence "should" occur for them.. (?)



steve lee: Thanks for your reply. I do not have problems with convergence when solving my simulation (any longer ;) ) . It is the sensisitivy study of different mesh sizes I am dealing with know. COMSOL is my first simulation software. I am yousing the laminar flow physics.

In order to have a quantitative measure that can be meaningful of the trend I suggest that you create a succession of grids, each one refined of a factor of 2 in such a way that the nodes of the coarser grid are projected on the finest. Then check using only these nodes.

The COMSOL predefined profiles are really great for getting a decent solution, but they have some arbitrarily lengths in them that makes them not so good for a systematic study. Consider defining your own profiles to have more control over the mesh characteristics.

Your solution in time looks not bad. And it doesn't show mesh independence, but there is some mesh sensitivity that is not terrible.

The problem with the volume integrated velocity magnitude is that this quantity doesn't really represent anything characteristic. The only way for the volume integrated velocity magnitude to converge would be if you were truly mesh independent, which is unrealistic even though it is the desire. I generally pick some sought-after-parameter, a quantity you're actually interested in for your analysis and do the grid dependence check based on this. Reason being, you don't actually care that the solution is grid independent everywhere all the time, you should only care that your particular needed quantity is insensitive to the mesh.

Also, laminar flows can be sensitive to gradients and mesh quality (even more so than turbulent flows) because its dominated by the diffusion term. Getting mesh independent laminar solutions everywhere all the time can be quite tricky because you need to carefully refine the grid in many places.

I don't see anything wrong with your results but if it's not mesh independent, then it's not.