[Hossein1]

I want to do an axisymmetric simulation of a collision between a droplet and a 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). In fact, unlike the nodes in the middle of the domain, the nodes on the 'axis' are not removed/added appropriately as particle moves.

[KevinZ09]

I'm not a big dynamic mesh expert, but will give some input:

1: A, B and C should be axis boundary conditions, not walls. In the tutorial they are axis boundary conditions too I believe. They might not be upon reading the files, but you've got to change them to axis boundaries.

2: I don't think you should mesh the particle. I can't come up with a reason why you should.

3: If the mesh gets too stretched, try having a finer initial mesh. Especially near the symmetric axis around the particle.

4: What do you specify as minimum and maximum length scales in remeshing (I can't really read your input values in the picture). And did you set your length scale to mm or m?

[Hossein1]

The first two points was applied.
Regarding #4, based on 'Mesh Scale Info', min and max length scales are 0.0006 and 0.25 mm (I don't know where this 0.0006 comes from as I can't really see a cell with such a small edge in the mesh). However, in the 'Remeshing' window, I input 0.01 and 0.25 mm as min and max length scales.
After the dynamic mesh fails and simulation stops running, min and max length scales are 8e-5 and 0.37 (i.e. the min value is reduced and the max value is increased, while I assume that these are reference values and should remain constant). So, I think something in dynamic mesh does not work properly, otherwise, we don't need to apply point#3 as the nodes must be updated as soon as a cell is stretched up to the max. value that I've defined. Is that right?
(I've attached the picture)

[KevinZ09]

Originally Posted by Hossein1

After the dynamic mesh fails and simulation stops running, min and max length scales are 8e-5 and 0.37 (i.e. the min value is reduced and the max value is increased, while I assume that these are reference values and should remain constant). So, I think something in dynamic mesh does not work properly, otherwise, we don't need to apply point#3 as the nodes must be updated as soon as a cell is stretched up to the max. value that I've defined. Is that right?
(I've attached the picture)

This is not entirely correct. What remeshing actually does it will mark the cells/faces that don't satisfy your criteria, e.g., when the length of one of the cells exceeds the maximum length value. If that's the case it will mark this cell for meshing, and it will TRY to remesh the cell. If it's successfull, it will replace the cell. If not, it will keep the old mesh. This automatically implies that, if remeshing is unsuccesfull, the maximum length of your mesh could be larger than your desired maximum length. That's why it's important you specify realistic values.

Also, I see you're using Diffusion-based smoothing. It's good, and better than Spring-based smoothing in many cases, especially for rotational motions, though I tend to use Spring-based smoothing more when you're using a triangle-mesh and only have translational motion (it's cheaper to resolve). But either one should work for your case. I'd strongly suggest though to play a bit with the parameters you can use there. You said in one of your other posts that the cells near the boundary got too stretched, so obviously you're smoothing isn't correct (remeshing can only do so much). As a start, set the Diffusion Parameter to 0, so you get more of a uniform mesh.

In short, have reasonable remeshing parameters, keep them fixed for a bit, and change your Diffusion Parameter (don't exceed 2) or use the Spring-based smoothing (keep the parameter between 0 and 1). Try it and let me know what the outcome is.

[Hossein1]

I played with different methods of meshing and I think the problem is not the parameters that I'm using in diffusion method or for remeshing. The major problem is that Fluent does not move any of the nodes located on 'axis'. If you watch this short clip, you'll see that only two nodes on the particle move and all other nodes remain fixed and that's the main dilemma (while the other nodes in the middle of the domain are changed according to the particle movement).
I'm not sure whether Fluent always doesn't move any node on the boundaries. In that case I could probably create a horizontal line very close to my axis and put the nodes on it (instead of on axis). Although, I think that might have a bad effect on the droplet approaching the particle from the opposite direction.
Please let me know if you have any idea for updating nodes in an axisymmetric problem.

[KevinZ09]

Originally Posted by Hossein1

I'm not sure whether Fluent always doesn't move any node on the boundaries.

When you use smoothing, what I believe Fluent does is move the boundary nodes according to the specifications (UDF or moving boundary), and then move the interior nodes to smoothen the mesh. This could perhaps imply that nodes not on a moving boundary don't move with smoothing, but only the interior ones. Have you tried turning off smoothing and just using remeshing? Because it does look a bit weird the boundary nodes don't move. So try that perhaps.

Otherwise don't make it axisymmetric. I think that's a better option than adding the "artificial" layer you mentioned. Though the problem should be solvable with a 2D axisymmetric mesh.

[Hossein1]

After trying various scenarios that I thought might work, here is how the issue 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' on 1 and 'local cells' was only checked in Remeshing. Maximum cell skewness was set on 0.5. With this configuration, the nodes on 'axis' are added/removed from the domain as particle moves which maintains the mesh quality.

[classified]

Hi ..
I am working on a problem which involves a half filled tank and which is under rolling motion. I had set a VOF model for 2 phases ( Water and air).
For applying rolling motion I wrote a udf as follows:
************************************************** ***************
#include "udf.h"
#include "dynamesh_tools.h"
DEFINE_ZONE_MOTION (oscillation, omega, axis, origin, velocity, time, dtime)
{
*omega=(0.3323*cos(3.81*time)); //here 3.81 is frequency of rotation
return;
}
************************************************** **************
After that this i interpreted this udf in ansys fluent
Then I choosed for cell zone condition on fluent window and surface body under zone selection box. then to this "surface body" zone i ticked on mesh motion and hooked the above udf.
but the results are not satisfactory...
PLEASE TELL ME WHETHER MY APPROACH IS RIGHT?
OR IF WRONG THEN HOW CAN I GIVE ROLLING MOTION TO TANK..
I AM A NEW USER SO HAVING A BIT OF KNOWLEDGE.


Thanks in advance