
[Sponsors] 
January 20, 2007, 06:29 
why solver does not accept negative volume mesh?

#1 
Guest
Posts: n/a

I have on query that why solver will not accept negative volume? Is the flux will become negative and so ? or another reason?


January 21, 2007, 19:27 
Re: why solver does not accept negative volume mes

#2 
Guest
Posts: n/a

Negative volumes are nonphysical and represent a bad grid.


January 21, 2007, 23:34 
Re: why solver does not accept negative volume mes

#3 
Guest
Posts: n/a

but what is the effect on solver? i mean why solver has problem to accept negative volume grid? Is it due to convetion or diffusin term claulation going bad or another thing?


January 22, 2007, 01:19 
Re: why solver does not accept negative volume mes

#4 
Guest
Posts: n/a

I am anther question,why there is negetive volume exist? I know is mainly because of the poor quality of grid, but I really want to know where are they come from?


January 22, 2007, 02:47 
Re: why solver does not accept negative volume mes

#5 
Guest
Posts: n/a

great question!
negative volumes are created by automatic mesher, or by user mistake. It depends on the method and software you use. For example in ICEM i never run into problems with negative volumes using any of the mesh generating approaches. But I guess it's because the mesher allways crashes when he run into neg.vol.When the nodes of the mesh are propagating, or are fiddled around and the algorithm is carefull with volumes, i guess it may happen. In STARCD  when trying to handsmooth the mesh, I've ran into negative volume creation from time to time. The mesher should check for negative volumes and the clever ones does not allow you to export the mesh to solver. In the same way the solver usually check prior to the solver run for negative volumes and stops if it finds one. I'm not really meshing expert. now to your first question  why. it is really that simple  it is not physical. And if were to write the code, I would check for neg. vol. at the beginning and halt the computation. (a) you want the computation to by physical(b)from the math side (only if we extend our imagination for negative space, can you do that?)  you have a problem with definition of the surfaces too, as the code integrates fluxes on surfaces, suddenly you may have flux which is mirrored on the surface of a negative cell, as the normal of the surface is heading the oposite way than it should. there might be lot of other reasons, but they're pretty useless. matej 

January 22, 2007, 06:31 
Re: why solver does not accept negative volume mes

#6 
Guest
Posts: n/a

If you want real precision on this, it is the diffusion term and source/sink that will make your code blow up.
Sources and sinks will effectively have their sign changed, which totally messes up the physical behaviour of the equation. For example, if you switch the sign of rhs in turbulence equations, you will get turbulence "decay" to infinity instead of zero. In case there's no sources, you will blow up the Laplacian. Negative volume has the sam eeffect as negative diffusivity: all smooth profiles are converted into deltafunctions. In other words: kaboooom! The last thing you need to worry about are the face interpolation factors: they should be between 0 and 1. In inverted geometries with negative volumes, they will be outside the range, which means that (for example) you can have phi_left and phi_right bounded but the interpolate will be out of bounds. Here, you will again produce nonphysical and unbounded values for physical variables, e.g. k < 0 which will blow up the code pretty quickly. Enough? Hrv 

January 22, 2007, 06:51 
Re: why solver does not accept negative volume mes

#7 
Guest
Posts: n/a

Negative volume is simply a grid problem that will interfere in your computation giving wrong terms. Most of the discrete method follow some kind of standard when computing their matrices and vectors from the discrete domain. If you don't follow this "standard" you'll surely interfere in how these matrices and vetors are being built. Here is the problem. You'll be solving your problem with a bad constructed system of equation.
BTW, in Finite Element Method we have to compute area and volume integration in an element level. For example, for a tetrahedron we compute 6 x volume by: V6 = x21 * (z31 * y14  y31 * z14) + x31 * (z12 * y14  y12 * z14) + x41 * (z12 * y31  y12 * z31) and the element conectivity must be counter clockwise (nodes 1234) or you will get negative volume (conectivity 1324). In this case, it's very easy to solve the negative volume. Just fix the conectivity to give you a positive volume. Of course, you can also have negative volume from distorted elements. In these cases you need to fix the mesh in your mesher by doing some king of smoothing technique or fixing by hand. Hope it helps in anything Renato. 

January 22, 2007, 07:37 
Re: why solver does not accept negative volume mes

#8 
Guest
Posts: n/a

Thanks Reanato, Hrvoje Jasak, matej, jsteadman, ag


January 31, 2007, 20:37 
Re: why solver does not accept negative volume

#9 
Guest
Posts: n/a

Hi ! That's a good question.... Hmmmmm Let's take the one dimensional rod and try to solve a heat equation. If you sweep the domain from left to right or right to left you should get the same answer as long as you are consistent with the sweeping and nodes numerotation... Now if you reverse the nodes at one element ("negative volume" in 1 D) you will have your finite difference scheme (let's say an UD 1st order) mixing up the nodes at the "negative volume" 1D element producing some really odd results.... It's interesting to see is there is some condition when the solution is still acceptable ?


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
[ICEM] Negative volume error in hybrid mesh  siw  ANSYS Meshing & Geometry  4  September 3, 2014 05:25 
SnappyHexMesh for internal Flow  vishwa  OpenFOAM Native Meshers: snappyHexMesh and Others  23  August 6, 2014 03:50 
remeshing due to negative volume error  Doginal  CFX  1  August 21, 2011 21:50 
blockMesh error ...  balkrishna  OpenFOAM PreProcessing  0  August 17, 2010 02:39 
Icemcfd 11: Loss of mesh from surface mesh option?  Joe  CFX  2  March 26, 2007 18:10 