[freeze]

HI!

I simulate a piston,recently

I build a cylinder and think it is fluid

I use udf let moving wall to compress the fluid

when I preview mesh motion, it always show Negative cell volume detected

I don't know why remeshing this function have not effect

anyone know how to resolve this problem

attachment is my model and dynamic mesh setup

Thanks

[RaiderDoctor]

Try enabling Local Face, and Region Face in the Remeshing tab of the Dynamic Meshing. Also, you may want to consider switching your Smoothing methods from Spring/Laplace/Boundary Layer to Diffusion. Ansys seems to recommend the latter as being much more robust. The Diffusion Function can be left as boundary-distance, and the Diffusion Parameter can be set to 2 (according to the manual, a value of 0 will cause the cells close to the moving boundary to absorb more of the motion, while a value of 2 will cause the inner cells to absorb more of the motion).



If that doesn't work, your next step would be to examine the area that keeps failing. To do so, go to Postprocessing, Surface, Create, Iso-Surface. In the new menu that pops up, directly underneath Surface of Constant, select Mesh, and then in the drop-down menu below that, select Cell Volume. At the bottom of the menu, click Compute. There should be values populating the Min, Max and Iso-Values region of the menu now. If the Min value is showing a negative number, then you have a negative cell volume. If not, then your mesh is skewed to the point where Fluent thinks you have a negative volume. To show this negative volume (if you have it), click the right arrow on the slide bar. This will generate a volume that is slightly larger than the absolute minimum, which is completely fine. Then, click Create at the bottom. Close out of this menu.


Go to Setting Up Domain, Display, and display your newly created iso-surface. You may need to uncheck the walls to appropriately see it.



Hopefully this helps!

[freeze]

Thanks for your recommend

i am really sorry for the late reply, because last week i have an important exam

i change my method from Spring/Laplace/Boundary Layer to Diffusion and resolve this problem

thank you for explain some fluent dynamic mesh setup

[mohkh]

Dear All @ Raide Doctor
The aim of this study is to simulate the blood flow an elastic blood vessel. Assumption of rigid blood vessel wall decreases and expanding according to the results especially when the vessel undergoes quite large deformations. During the cardiac cycle, the fluid flow induces forces from the time-varying blood pressure.
Pulsatile flow profile was implemented via User Defined Function (UDF) to mimic the cardio-ac cycle.
V(t) = amplitude +sin(ωt)
ω=2πF,F=1/T
Pressure profile was implemented via User Defined Function (UDF) to mimic the cardio-ac cycle.
R(t) = amplitude +sin(ωt+θ)

My set up:
D=300µm
T=0.8 s
Geometry attached file.
I am suffering from NCV even when I start with preview zone motion
Many thancks

[vivjk94]

Originally Posted by mohkh

Dear All @ Raide Doctor
The aim of this study is to simulate the blood flow an elastic blood vessel. Assumption of rigid blood vessel wall decreases and expanding according to the results especially when the vessel undergoes quite large deformations. During the cardiac cycle, the fluid flow induces forces from the time-varying blood pressure.
Pulsatile flow profile was implemented via User Defined Function (UDF) to mimic the cardio-ac cycle.
V(t) = amplitude +sin(ωt)
ω=2πF,F=1/T
Pressure profile was implemented via User Defined Function (UDF) to mimic the cardio-ac cycle.
R(t) = amplitude +sin(ωt+θ)

My set up:
D=300µm
T=0.8 s
Geometry attached file.
I am suffering from NCV even when I start with preview zone motion
Many thancks

did you solve this? if you did please tell us what you did. thanks

[mohkh]

Not yet, I am trying to solve it thanks

[RaiderDoctor]

Hey Mohkh,


Sorry, I didn't see this message previously.



Okay, so there's a lot going on with your setup, but I'm not sure you need all of it. First off, your walls are not rigid body; they are compliant. Rigid means they don't move, compliant means they do (even if you impose the motion).



Next issue is the prescription of motion. I'm not sure where you got it from, but it reminds me of peristaltic motion. To my knowledge, this isn't a good model for cardiac blood vessels. It might be better to try and run a 2-way fluid-structure interaction simulation.


Now, on to why you have negative cell volumes. I'm afraid I'm not sure. It could be due to a number of issues that all require different solutions. But it'll be hard to narrow down which solution is best with the given info. I can suggest you try diffusion smoothing, with remeshing enabled. Use local face, region, zone, etc. Make sure you specify the min and max length scales to be approximately 0.4 and 1.4 of your min and mix mesh scales (find this by clicking on mesh info in the remeshing tab of dynamic meshing). If this doesn't work, check out your time step size. Is it small enough to allow your mesh to absorb the motion? Beyond that, I'm not sure what else I can offer without more info.


Good luck!
RD

[mohkh]

Originally Posted by RaiderDoctor

Hey Mohkh,


Sorry, I didn't see this message previously.



Okay, so there's a lot going on with your setup, but I'm not sure you need all of it. First off, your walls are not rigid body; they are compliant. Rigid means they don't move, compliant means they do (even if you impose the motion).



Next issue is the prescription of motion. I'm not sure where you got it from, but it reminds me of peristaltic motion. To my knowledge, this isn't a good model for cardiac blood vessels. It might be better to try and run a 2-way fluid-structure interaction simulation.


Now, on to why you have negative cell volumes. I'm afraid I'm not sure. It could be due to a number of issues that all require different solutions. But it'll be hard to narrow down which solution is best with the given info. I can suggest you try diffusion smoothing, with remeshing enabled. Use local face, region, zone, etc. Make sure you specify the min and max length scales to be approximately 0.4 and 1.4 of your min and mix mesh scales (find this by clicking on mesh info in the remeshing tab of dynamic meshing). If this doesn't work, check out your time step size. Is it small enough to allow your mesh to absorb the motion? Beyond that, I'm not sure what else I can offer without more info.


Good luck!
RD

Thank you very much for your response and your Time. I will try everything and let you know.