Boundary layer parameters requirement in quasi-2D CFD-DEM problem
Altair EmployeeHi Support,
I’m doing a CFD-DEM problem with Acusolve and EDEM. The geometry is a thin slot (width/thickness/height: 60/2/150 cm), and the side walls are in non-slip condition. The other boundary conditions and particle positions are shown below:
The particle diameter is 4.5 mm, which means the geometry can accommodate approximately 4 particles in the thickness direction, so I’d like to have 4 layers of elements in the thickness direction (average mesh size: 5 mm).
My questions are as follows:
- Because of the non-slip wall condition and also because there are only 4 layers of elements in the thickness direction, I guess that I should add boundary layer mesh to avoid low flow velocities near walls. Is that correct?
- Assuming that I need boundary layer mesh, however, the flow field in the boundary layer is not my focus. Do I need to carefully calculate the boundary layer parameters, such as first layer thickness and growth rate?
I would be grateful if you could help me in this matter.
Regards,
Gary
Best Answer
-
The boundary layer meshing resolves the near-wall velocity profile better, but does require more mesh to do so.
If your main interest is in the motion of the EDEM particles, the boundary layer meshing (and exact near-wall profile) likely has less impact than with a CFD-only simulation where the pressure drop may be of great importance. So you're likely fine with a thicker first boundary layer element.
As you do mesh sensitivity studies, you may find you need more CFD mesh elements in the bulk flow. The particles appear to be fairly dense, which often requires more CFD mesh.
The typical question - simulation runtime versus accuracy - how do the results of interest change as the mesh is refined? That's something you'll need to determine by running simulations with different meshes.
0
Answers
-
The boundary layer meshing resolves the near-wall velocity profile better, but does require more mesh to do so.
If your main interest is in the motion of the EDEM particles, the boundary layer meshing (and exact near-wall profile) likely has less impact than with a CFD-only simulation where the pressure drop may be of great importance. So you're likely fine with a thicker first boundary layer element.
As you do mesh sensitivity studies, you may find you need more CFD mesh elements in the bulk flow. The particles appear to be fairly dense, which often requires more CFD mesh.
The typical question - simulation runtime versus accuracy - how do the results of interest change as the mesh is refined? That's something you'll need to determine by running simulations with different meshes.
0 -
acupro_21778 said:
The boundary layer meshing resolves the near-wall velocity profile better, but does require more mesh to do so.
If your main interest is in the motion of the EDEM particles, the boundary layer meshing (and exact near-wall profile) likely has less impact than with a CFD-only simulation where the pressure drop may be of great importance. So you're likely fine with a thicker first boundary layer element.
As you do mesh sensitivity studies, you may find you need more CFD mesh elements in the bulk flow. The particles appear to be fairly dense, which often requires more CFD mesh.
The typical question - simulation runtime versus accuracy - how do the results of interest change as the mesh is refined? That's something you'll need to determine by running simulations with different meshes.
Hi Acupro,
Thanks for your detailed explanation. I have some follow-up questions:
1. Just to clarify, "So you're likely fine with a thicker first boundary layer element," does it mean that the first layer or even the total boundary layer thickness has less impact on the CFD-DEM model, so any thickness is acceptable?
2. In most literature on CFD-DEM, the CFD grid should be larger than the DEM particles in the so-called unresolved method, usually about 1.1–1.6 times. If I do the mesh sensitivity study, the CFD mesh is bound to be smaller than my particles. Does Acusolve 2022.3 support the resolved method?
3. The default turbulence model and wall treatment method in Acusolve are the Spalart-Alamars model and wall function. However, SA model is a low Reynolds number model. When using the SA model, does the wall treatment still utilize the wall function?
Regards,
Gary
0 -
Ying-Hsuan Ko said:
Hi Acupro,
Thanks for your detailed explanation. I have some follow-up questions:
1. Just to clarify, "So you're likely fine with a thicker first boundary layer element," does it mean that the first layer or even the total boundary layer thickness has less impact on the CFD-DEM model, so any thickness is acceptable?
2. In most literature on CFD-DEM, the CFD grid should be larger than the DEM particles in the so-called unresolved method, usually about 1.1–1.6 times. If I do the mesh sensitivity study, the CFD mesh is bound to be smaller than my particles. Does Acusolve 2022.3 support the resolved method?
3. The default turbulence model and wall treatment method in Acusolve are the Spalart-Alamars model and wall function. However, SA model is a low Reynolds number model. When using the SA model, does the wall treatment still utilize the wall function?
Regards,
Gary
1 - This really comes down to your particular needs/desires from the results. We often use a coarser boundary layer mesh to save on runtime. However, if the exact near-wall velocity profile has a large impact on the behavior of the EDEM particles, then you'll want to have a more-resolved mesh. The only way to know is to run with different meshing strategies/parameters to see how that affects the results of interest. Then you can judge if the additional cost of running with more mesh is worth the change in the results.
2 - Yes - the communication handles what you refer to as the resolved method. If the fluid velocity is constant across several particles, you may be fine with larger CFD mesh elements. If the velocity varies widely across a single particle, then you'll want five to six mesh elements across the particle length to resolve those gradients. You'll again get better accuracy at the cost of higher simulation time.
3 - The standard wall function in AcuSolve supports the full boundary layer - with a maximum first node Y+ around 300. Lower Y+ will give better accuracy as the flow profile is then resolved more versus assumed by the wall model, again at the cost of higher runtime. The wall function is valid through all portions of the boundary layer - to low first-node Y+ values.
0 -
acupro_21778 said:
1 - This really comes down to your particular needs/desires from the results. We often use a coarser boundary layer mesh to save on runtime. However, if the exact near-wall velocity profile has a large impact on the behavior of the EDEM particles, then you'll want to have a more-resolved mesh. The only way to know is to run with different meshing strategies/parameters to see how that affects the results of interest. Then you can judge if the additional cost of running with more mesh is worth the change in the results.
2 - Yes - the communication handles what you refer to as the resolved method. If the fluid velocity is constant across several particles, you may be fine with larger CFD mesh elements. If the velocity varies widely across a single particle, then you'll want five to six mesh elements across the particle length to resolve those gradients. You'll again get better accuracy at the cost of higher simulation time.
3 - The standard wall function in AcuSolve supports the full boundary layer - with a maximum first node Y+ around 300. Lower Y+ will give better accuracy as the flow profile is then resolved more versus assumed by the wall model, again at the cost of higher runtime. The wall function is valid through all portions of the boundary layer - to low first-node Y+ values.
I see, thank you very much for your detailed explanation.
0