Error: Negative volume and Creating empty surface
 

Hello everyone,

I have two interface walls defined as dynamic mesh, that move as a rigid body according to an udf in a flow domain. The problem is in transient time.
When I try to compute the solution, the simulation stops with this error:

"Warning: no positive-volume exist.
Error: update-dynamic-mesh failed. Negative cell volume detected
Note: zone-surface: cannot create surface from sliding interface zone.
Creating empty surface."

If I see the mesh surrounding dynamic mesh zones (interface walls) it's deformed a lot. But, I don't know how to fix it and I can't understand the "Note".

Could anyone help me?

Thank you in advance.

It is producing negative volume due to dynamic mesh setup. Either check the mesh settings (use tetra ) or dynamic mesh settings.

I'm already using tetra mesh...
I tried with declaration of fluid zone surrounding the particle as deforming zone...but it doesn't work... :(

i've got your problem either.
it seems that problem is within using interface walls in remeshing method
:(

At the end I did't use interface walls , but a mesh around the moving body that connects the wall of moving body and the mesh of external fluid domain.

at last i found the answer (:
actually i was modelling a simple 3d model of falling sphere in water.
i 've successfully done it with interface walls.
my problem was that i didn't take buoyancy into account; sphere had much less density than water so it went up in about 0.01 sec. (density of sphere is calculated by fluent which is mass divided by volume )
don't forget to choose both interfaces as "rigid body" and "passive" in dynamic mesh options.

How did you take buoyancy into account?

Hello All,

I want to do analysis of heat transfer from water flowing through pipes submerged inside concrete. I am modelling in GAMBIT and wish to analyse it on Ansys FLUENT.

Can anybody help me out, how to model and simulate?

Does any tutorials exist?

hi mate,
actually with 6DOF option in dynamic mesh, fluent automatically considers buoyancy force between solid(ie. box) and fluid(water).
my problem was that i considered rather little mass for box (in the main problem it was sphere) so that it went up!
in this example(2d version), i made a structred grid around box and let it move with the same speed as box.(as you can see in picture).
and used remeshing method for unstructured grid.
i use fluent v14.0 64 bit, if you want, post me your email so i send you case & data and udf.
Attachment 16128

hi mate,
modelling "water through pipe which is surrounded by concrete", it appears to be a rather simple task.
how much are you familiar with gambit & fluent?
you wanna model it 2d or 3d?

Sadjad,

I am a beginner of GAMBIT & FLUENT. My aim is to analyse the heat transfer and to analyse the temperature distribution among the concrete. I think 2D would suffice me, can you help me out?

your analysis seems easy if you set all problem's specifications correct.
but you need first to learn meshing with Gambit.
by doing these tutorials at this site(Cornell University), you'll have a rather sufficient view of Gambit&Fluent.
https://confluence.cornell.edu/displ...arning+Modules
Then you can start simulating what you want.

But, I didn't find any tutorial that is nearer to my work.

you are right but if you are a beginner, you need to learn these two softwares from base.
by doing those tutorials you will get familiar with meshing via Gambit and some basic CFD modellings with Fluent.

Thank you sadjad!

Hi Sadiad,

I had the same experience of the solid sphere bouncing off the liquid surface instead of submerging. In 2D case, how did you specify the volume of the sphere. I believe in the 6DOF property UDF, you are giving mass and moment of inertia as the required inputs.

Regards,

dear mate,
no need to specify volume, because fluent compute it by geometry.
you just need to enter mass of sphere via udf and density will be computed by "density=mass/volume".
a circle in 2d is actually a cylinder which has one meter depth so in order to compute volume just multiply section are by one.
to solve your problem just make sure that density of sphere is higher than fluid.
if there is still problem, send your email address to send you case&data&udf.

Hi Sadjad,

Thanks for your reply.

Earlier, I calculated the mass based on a sphere which is actually a cylinder in 2D. This caused the problem since cylinder volume considered by FLUENT is higher than the sphere and consequently density of solid became lower than the fluid.

I have fixed the problem now.

Thanks again!

Regards,

solid body floating using
 

Hi Sadjad,

Although the dynamic mesh model worked for heavier particle (density > liquid). for lighter particle (particle density < liquid density), it seems there's some problem. The particle bounces off the interface instead of floating on the liquid. Any suggestion?

Regards,

hi mate,
if you are sure that particle must go up (i.e. density of particle is less than liquid density), then you must use very little time step.(even in order of e-7)
as it is obvious, particle will throw up very quickly, so in order to catch motion, use little time step.
as a suggestion, the order of time step should be in a way that in each time step, your body moves less than cell height.

I did the same! :)

Hi!
I was able to simulate a buoyant particle fully immersed in a fluid just setting the acceleration of gravity = 0 and the operating density ( in operating conditions) equals to the fluid density. It works.
For your case...have you seen the ansys tutorial about a 2D buoyant box? This is the video of simulation http://www.youtube.com/watch?v=UpFCF-ctMp0 , but you can find the tutorial on web http://www.scribd.com/doc/92954775/F...2d-Falling-Box.

2D airfoil O Grid- negative volume
 

Hi,

I'm carrying out a 2D pitching airfoil simulation using dynamic meshing with a "O" Grid.It is a structured mesh. The dynamic conditions i have given were
1) airfoil - rigid body with UDF with pitching over X=0.25
2)interior - deforming with the min and max length scale from zone scale info
3) fluid -deforming with the min and max length scale from zone scale info.

The spring constant i gave was 0.001 and
convergence tolerance 0.0001
No of iterations 150.

The time step tat i used is 0.001.

After running the iterations and after about 500 time steps i'm getting the following error

negative volume detected
dynamic mesh update failed.
i have worked around with the spring constant and also with the time step nothing worked.
could someone help me out rectify this issue..
thanks in advance,
sam

negative volume - dynamic mesh failure
 

Hi Sam,

In dynamic mesh problems, the mesh around the solid body keeps deforming during each iteration. Now, when the mesh becomes too distorted that the centroid of the cell lies outside the cell boundary, a negative volume is detected triggering the solver failure.

In a structured mesh, cell distortion is always higher than the unstructured mesh. You may tighten the the remeshing criteria i.e. the minimum cell size, skewness ratio etc. however the best way to get rid of the problem is to use "unstructured" (tri/tetrahedral) mesh. This works.

hi

The message "Note: zone–surface: cannot create surface from sliding interface zone" simply means the boundaries of the non–conformal interfaces match exactly, such that there are no non–overlapping sections on either side of the interface.

chek this file for more details

https://events.prace-ri.eu/event/156...l/slides/5.pdf

Please any one help me ..how can L solve this problem which appears to me
( application error in CFD_post
error the doesn't exist or is not readable )
So what the reson and what solution? ???
Please. ..

6-DOF buoyant wooden box
 

Thank you for your kind hints.
I have a similar project , but i have a floating box. actually this is a Wave Energy Converter which starts oscillating as a result of wave. I have tried both reducing the time step size and fine meshing but still face the same error as you. dynamic mesh failed. negative volume detected. would you please share your Dynamic mesh setting with us?
Thank you in advance.
Megan.