For simulating a droplet collision onto a moving particle, I use a semi-circle as my particle in an axisymmetric solution. However, I don't have just one line as the 'axis' of domain and particle breaks it up into 3 connected lines as shown in the attached picture. However, when I run the simulation, it stops after a few time steps due to having an inappropriate mesh. It should be noted that when the simulation starts, A=A’ and B=B’ and you can see how particle motion changes the quality of mesh mainly around the impact area. Could you please let me know what to do to prevent this error?
I think the problem is the breaking points on the axis that causes the dynamic mesh not to be able to adjust itself while particle is moving.
PS. I’ve meshed inside the particle and I’ve defined particle as a ‘solid zone’. Therefore, the fluent recognizes a ‘particle-shadow’ as well which is like a virtual interface on the particle surface that I’ve defined it as a ‘wall’ in Boundary Conditions.
Dear
see the following may be help you
http://archimer.ifremer.fr/doc/00006/11757/8497.pdf
Thanks Razi, I looked into the paper, but I think my problem arises from disconnectivity of the 'axis' that I have (which is due to having a particle there). Therefore, when particle moves, dynamic mesh fails to update the mesh properly. I need to figure out how to resolve this issue. (maybe in meshing software)
Dynamic mesh simulations with a deforming mesh are always tricky - I had several problematic cases with this, too. The mesh itself and the mesh settings are looking ok, so I don't think you can solve this issue inside the meshing software: it's a Fluent problem. Did you try to decrease the time step size in order to reduce absolute change in position of the droplet? Also, I'd consider to reduce the limits for the cell and face skewness as well as the maximum length scale allowed (0.25 mm in your case). The length d that is marked in your sketch seems to be smaller than this and the adjacent cell is stretched already. Just out of curiosity: why do you need the axis at all?
Regards,
Stephan
I use a 'variable time step' based on Courant number=0.2 so that Fluent can change it based on the droplet velocity. It's usually around 1e-7.
I need to have an 'axisymmetric solution' and for defining that, I think we need to define the axis first (on the x direction). Regarding length 'd' that you mentioned, in fact the adjacent cells still have the initial length by which mesh was created (0.2 mm) and 'd' is stretched after particle movement (therefore, d>0.2 mm)
Don't you think that spring or layering method might be more suitable for this problem? I've tried spring with coef. 1 but I've not tried the layering yet. Do you have any idea of the suitable parameters for layering method?
Bests,
Sayed
Hello Sayed,
I set up two simple test cases similar to yours (see zip file enclosed, UDF for CG motion is included too). The first case has the symmetry axis, but this is not included in the second case. Since I don't know all your boundary conditions, I did only the preview of the dynamic mesh motion, but no simulation. However, I could reproduce your issue that the calculation stops due to negative cell volumes. When using the full domain case (without symmetry plane), the calculation runs through without any problems (see also the two figures below). You can check all the settings in the Fluent case: I used the layering and smoothing with the default settings. I also recommend to use the option 'size function' in the remeshing tab - this was very helpful to maintain a certain mesh quality.
The final result of my quick test cases: after playing around with all settings for the remeshing, layering and smoothing, I think that Fluent is not able to update nodes at the outer edges of the domain (Fluent doesn't do that in the full domain case either, only nodes within the bulk region were updated - at least in all the cases I ran through, which were at least 30 different combinations...). I found that a negative volume occurs, whenever the droplet moves over a distance that is longer than the length of the first adjacent cell next the droplet near the symmetry axis (in the corner where the two axes inside and outside the droplet hit each other).
Since the case without the symmetry axis works, you may want to use this for your simulations. Of course, you can also contact ANSYS support for further help...
Regards,
Stephan
Hi Stephan,
Thanks for detailed information. What you mentioned that Fluent does not update the nodes on the boundary is really interesting and the exact dilemma that I'm facing right now.
Regarding the 2D simulation, I've already set up a case for particle-droplet collision. It still needs some fine tunings, but I think generally works well. I've attached a snapshot of my results. The reason that I'm trying to use axisymmetric method is that the nature of my problem is not 2D as the interfacial forces applies on a cylinder is different than a sphere.
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.
- Badges
- Science topic