I want to do an axisymmetric simulation of a head-on collision between a falling droplet and a spherical particle. However, as you can see in the attached figure, dynamic mesh fails to follow the particle movement (when simulation starts, A=A' and B=B', but after some time steps you can see that how A and B are getting stretched). Do you know how to define the domain for such an axisymmetric problem?
PS.
1) It might be something related to the way that I define the domain. I assign A, B and C as 'axis' Boundary Conditions. However, in the case file of this Ansys tutorial, they are defined as 'wall'. However, when I change A, B and C to 'wall', simulation stops as soon as I run it.
2) I don't need necessarily to mesh inside the particle and I've tried that case as well, but the problem still exists.
Dear Sir,
I recommend using the hybrid mesh instead of auto meshing because hybrid mesh approach will give more control on the creating nodes in the critical regions where different surface parts are joining. Besides, you should also take care of exact tolerance gap between the mating surfaces.
Hi Sayed,
How did you set the remeshing parameters?
Did you give proper Max skewness value and other params?
Hi Dhyan,
The info. was added to the problem Figure.
Thank you!
PS. My feeling is that Fluent does not limit itself to the maximum skewness that I enter, although I don't know what should be modified here so that the dynamic mesh is updated correctly.
Try using only local cell remeshing and copy the same mesh scale info provided by Fluent. Also, for smoothing use spring-based with may like 0.5 for the spring constant.
Thanks Dhyan, It seems that I have a little better mesh now, but as the particle moves, it sweeps the nodes in front.
It seems that I have a little better mesh now, but as the particle moves, it sweeps the nodes in front.
Another thing is that my initial mesh has uniform triangular cells of 0.2 mm edge. However, the 'minimum length scale' that I get in Mesh Scale Info is ~ 0.0001 mm before I start the simulation. I don't know where this small value comes from.
I've attached an illustration for more clarification. Resolution is high enough for reading the numbers, but you may need to download the picture first.
Thanks again
PS.
- The fact that cells are broken down is due to the Gradient Adaption
- The simulation always stops exactly when the particle moves 0.2 mm (distance between two initial nodes)
Hi Sayed,
So did you check the mesh before importing in fluent or within fluent. Did you check the minimum and max volumes or face statistics?
Also, What is the cell skewness and orthogonal quality values of the mesh? Try to have a mesh with max skewness less than 0.8 (if mesh is done in ANSYS Meshing).
Or
As in the relief valve example given, why don't you try to use layering instead which much more stable and of good quality?
What you can try is make small region outside your solid particle and form a quad mesh outside the domain and a tria mesh inside that domain. Then you apply layering for the outer domain only with smoothing for both zones.
Dear Dhyan,
Thanks for comments.
When I imported the mesh into Fluent and before start running the simulation, the min and max length scale was 0.001 and 0.286 mm.
Maximum cell and face skewness are already below 0.8 (set on 0.6) and:
min vol (m3): 3.7e-12
max vol (m3): 5.8e-10
min2d vol (m3): 1.2e-08
max 2d vol (m3): 2.5e-08
For the 2nd part, and due to having a moving particle in the middle of mesh, do you think that zones shown in the attached picture can be used for layering technique (I'm not sure if the default layering parameters are ok)? or I necessarily need to define the narrow area around the particle? (with a trian mesh inside that narrow area, and quad mesh outside it).
Thanks again!
I tried many different scenarios and here is how the dynamic mesh issue in an axisymmetric model was finally resolved:
For 'Dynamic Mesh Zones', I defined particle as a 'rigid wall' and gave velocity to it with UDF, and then I defined the symmetry line as 'deforming' and with the appropriate min. and max. length scale. For this to work, both 'smoothing' and 'remeshing' must be selected (I set 'diffusion parameter' as 1).
Thanks and please let me know if there is room for improvement.
Hi,
Good, it started working. But, using deforming condition for symmetry felt strange for me. Anyways if it works then no issues.
If possible please send the current picture of the mesh after motion and the various parameters which you have used.
Dear Sir,
I recommend using the hybrid mesh instead of auto meshing because hybrid mesh approach will give more control on the creating nodes in the critical regions where different surface parts are joining. Besides, you should also take care of exact tolerance gap between the mating surfaces.
Thank you, Mr. Ghassan,
1) I've attached a picture of the hybrid mesh that I'm using right now. Liquid deformation is very similar to my experiments, however, the lamella is shorter (?).
2) I'm not sure what you mean exactly with "take care of exact tolerance gap between the mating surfaces". I appreciate if you can explain.
Thanks!
- Badges
- Science topic