3d dynamic meshing
 

A sample case file is attached for seeing the settings. Also, you need to imporve your mesh.


https://drive.google.com/open?id=1I9..._L7ZMNCz0JiS5B

Dear All

I am a PhD Student in Mechanical Engineering. My thesis is based on "Fluid Structure Interaction at Microscale". Right now, I am trying to simulate transient FSI in a rectangular microchannel. The three walls of the rectangular microchannel, which includes the two side walls and the bottom walls, are rigid (no deformation) and the top wall is soft (deformable). Please see the attached image for geometry.

We are using ANSYS Workbench for this 2 way coupled transient FSI simulation. The CFD is being carried out in Fluent with dynamic mesh option on, while the FEM is carried out in Transient Structural. While I have been able to succesfully carry out the simulation for steady state, the transient simulations are not converging due to "negative volume" problem in Fluent . The settings which I have invoked are:
1. Used both diffusion based smoothing, with diffusion constant ranging from 1 to 3, and spring based smoothing, with spring constant value of 0.5.

2. Used remeshing with minimum length scale and maximum length scale of 0.001 times minimum cell info and 100 times the maximum cell info. I suspect that this is not particularly useful because Remeshing does not get invoked for hex mesh anyhow and my fluid domain is hex mesh.

3. Declared the lower surface of the upper wall, which see the fluid domain, as System Coupling. Declared the entire fluid domain, which is just beneath the top wall as Deforming.

4. The adjacent cell height was taken to be the average height of the mesh (cell) in the fluid domain in the direction perpendicular to top wall .

Apart from these, I also ramped the data transfer pertaining to force and displacement in the System Coupling module and kept the time step to 10^-5.

Even then I have failed to get the simulation going past a few iterations, not even the first time step is converging.

Please advise on the basis of your rich knowledge and experience, how I should proceed.

Flow Setup
 

I am afraid I could not understand the flow setup. There is only one open side for the fluid domain. Are there no inlets and outlets? Is it natural convection in a cavity? Does the flow simulation run without FSI?

Hi All

Perhaps, I was not clear with the way I presented the picture. The picture in the previous message was for a cross-section, i.e. for z = constant. The length wise geometry is shown in the picture attached with this message.

The flow direction is along z. The z =0 is the inlet, while z = L is the outlet. The top cuboid shown in the picture is the top (deformable) wall of the channel. The lower cuboid is the flow domain. The three edges of the lower cuboid form the three edges of the channel, which are rigid, while the fourth edge forms the FSI interface with the top wall.

Deflection
 

This appears to be a simple channel flow. What is the reason for deflection?

Remeshing cannot be used with hex cells. If the deflection is not very high, then use smoothing. If deflection is high, then use remeshing, however, you have to mesh the domain using tetrahedral cells. Remeshing in hex cells is possible only via layering, which may not be applicable in this case. If you enable remeshing, Fluent will invoke remeshing for hex cells as well and fail, leading to error. So, disable it.

For diffusion based smoothing, use a value of diffusion parameter between 1 and 2. Spring based smoothing is not really applicable here but depends on the motion. If the motion is more or less normal to the moving surface, like a piston, then spring based is alright, otherwise, do not use it with hex cells. Cells zones are never supposed to be declared deforming or otherwise, only boundaries require settings or those cells zone that move as rigid bodies.

Hey

Thank you for your reply.

Yes, the flow is indeed a channel flow and the deflection (of top wall) is caused by the flow underneath it.

To ensure that re-mesh works, the hex mesh is to be replaced by the tet mesh. But if we do that, we will also have to insert prism elements to capture the boundary layer effects, is it not so?

So the question then arises, will re-meshing work with prism mesh? Do we need it to work with prism mesh? How do we ensure that?

Thank you for your time and we look forward to hearing from you.

Regards

Hex or Tet
 

You don't need to use tet mesh. All I meant is, in case the deflection is very high and remeshing is required, then you have to use tet. If deflection is not very high, which I do not expect in this case, hex with diffusion will work fine.

I still do not understand why the flow in a channel would cause any deflection at all until and unless the material is sensitive to turbulence.

Thanks for the reply.

There is no turbulence. The deflection is there because
a: The top wall is made of soft material, PDMS, (which has elastic modulus of order of 1 MPa, compared to GPa for steel).
b: Due to lubrication approximation, nature of geometry, the hydrodynamic pressure is very high. To put in other words, you need a large amount of pressure to push the fluid through a long, narrow channel.

You can see the below papers by our group , where I have carried out the same simulation, but in steady state.

So according to you:
1. We should continue to use hex mesh, but switch off remeshing
2. If we want to use re-meshing, then we should use tet mesh, but then the question comes about using prism layers to capture BL effects.

Please advise. And thank you again for your time.

[1] Hydrodynamic Bulge Testing: Materials Characterization Without Measuring Deformation: https://asmedigitalcollection.asme.o...051012/1074424

[2] Non-Newtonian fluid–structure interactions: Static response of a microchannel due to internal flow of a power-law fluid. https://www.sciencedirect.com/scienc...77025718303343

Deformation
 

If the deformation is only due to high pressure, then you would not expect much variation in transient simulation as compared to your steady-state. The frequency of oscillation in a laminar flow is rather low. So, in my view, hex with smoothing will do the job for you. If you need tet, then you should use boundary layer mesh near the solid boundary. And Fluent gives you option to ensure that remeshing is done only away from the boundary layer mesh. That way, the quality of flow-field near the solid object is maintained and remeshing is also successful.

Thanks again for your reply. I appreciate yours taking time to help and guide me.

I have re-started the run with hex-meshing but re-meshing option switched off.

However, I would like to understand in a little more detail your suggestion regarding tet mesh+ Boundary layer treatment in FSI. How can we tell the Fluent to re-mesh only tet elements, while leaving the Prism elements (boundary layers) as it is? What are the options in FLUENT to switch on and switch off in order to achieve that?

Please advise.

Also, our ultimate aim to simulate the transient FSI in a microchannel made of viscoelastic material. To that end, we are first simulating transient FSI in a linearly elastic channel.

Thank you

Edit: The hex-mesh run, with re-meshing switched off, has been completed but again it did not converge with the same errors as "negative" volumes.

Hi all

Thank you for your help and guidance so far.

To my utter dismay, the run did not go on and failed with negative volume error, again.

I had converted the whole domain to tet mesh (no hex/prism). Spring smoothing was on with 0.5 spring constant. Remeshing was also on with Local cell option. The time step of FSI was 10^-5.

Please help me solve this problem.

If you wish I could send the full workbench files to you.

Thank you

Deformation Shape
 

What kind of shape is expected due to the deformation?

The deformation is primarily normal to the flow. The flow is in +z direction, and the deformation is in +y direction.

Before the FLUENT solver fails, it encounters reverse flow, initially at the pressure outlet, but then at the pressure inlet as well.

I have run simulations like these several times before, at more extreme conditions (with higher pressure/flow rate). But they were all steady state cases. This is the first transient FSI I am running. Also, the earlier FSI simulations were flow rate controlled, this is pressure drop controlled.

Thanks

Vishal

Suggestions
 

With remeshing, at least, I would expect it to work well. The time-step is also small enough. Does it fail in the very beginning? If that is the case, you can initialize with high pressure inside the system so as to avoid any flow reversal. However, if it fails after some iterations due to flow reversal, then you may have to do something with pressure outlet condition. I suppose in new version, there is option to ensure that there is no flow reversal; this creates a wall in place of flow reversal.

To debug the case, you should try Fluent alone by giving the boundary some random motion in the expected direction, such as, by using UDF for sine wave motion. UDF for this is certainly available within UDF manual. Once the mesh and dynamic settings are good enough for it to work with sine wave motion, it most likely will work with FSI as well. UDF for deformation of a cantilever is available at

https://www.afs.enea.it/project/nept...udf/node85.htm

You can modify the equation to sine wave with expected amplitude.

Dynamic Mesh Failed. Negative cell volume detected
 

Hi

I am new to Ansys Fluent and i have been struggling with 3D simulation on a body during free fall. I read lots of posts talking about the error "Dynamic Mesh Failed. Negative cell volume detected". I tried every possible solution described in the posts (decreasing the time step, decreasing the maximum length scale in re-meshing, decreasing the spring stiffness) but nothing made it to work.
Can someone help me in figuring out this issue? I am discussing my entire problem setup below. Any help would be really be appreciated.

- I have an elliptical body (about 6") that I am testing it for free fall in a fluid medium with 6DOF. I have a large cylinder surrounding the body which is assumed as a fluid domain.

- I subtracted the elliptical body from the fluid domain and meshed it using adaptive mesh in Fluent mesh. I am using Ansys 2019R2.

- I had three named selections 1) inlet 2) outlet 3) ellipbody (this is the body i want to analyze for free fall)

- Now i am in the fluent setup and i am using transient condition with pressure-based solver. I had the fluid, material setup and verified cell zone ad boundary conditions.

- In the dynamic mesh, I selected re-meshing and smoothing. For re-meshing I used Local cell, Local face with values of min/max length scale similar to mesh scale info. For smoothing i used spring constant of 0.001 with 100 maximum interactions.

- I also selected for 6DOF, and created a 6 DOF property (with inputs for mass of the body and moment of Inertia values). I came to know that if you are doing a free fall study, there is no need to write a UDF in Ansys 2019R2. Just create a 6DOF property.

- Later i created dynamic mesh zones for ellipbody (rigid body, In Motion Attributes tab, selected the 6DOF property created in previous step).

- Then i initialized and ran the calculation for a timestep size of 0.003 sec for 1000 time steps.

- I have the solution run but throws me this error- "Dynamic Mesh Failed. Negative cell volume detected" just after it started.

Any help in understanding the problem will be a lot helpful.

Mesh and Smoothing
 

First of all, you need to ensure that the mesh is tetrahedral and not hex or hex dominant. Secondly, it should be of good quality, i.e., low skewness and high orthogonal quality. Secondly, do not use 0.001 as spring constant. Keep it default, rather 0.2 might improve the results. You may also prefer using diffusion based method instead of spring analogy based.

I am also facing same problem can you please help me

please I am also having same error in my simulation ( negative cell volume) please help me to solve the problem