After a lot of tries, i just dont know how to improve this mesh quality
 

Hi, basically im working a vineyard simulation which domain is a 400 mts x 400 mts x 50 mts high air volume with files of vines trees at the bottom. The vines trees are modelled as rectangular prisms, as seen in the figure attached.

Ive tried different things but im gettin skewness 0,99999 and orthogonal quality around 1 E-5 all the time. I guess the cause of that is because the size of the front face of each file of vine trees is 1 mt x 1 mt (see image attached), but i dont know how to adress it.

My meshing settings right now are:

Face sizing front face: 0,5 mt element size, behaviour hard
Edge sizing file of trees: element size 5 mt, behaviour hard
Body sizing domain with air: element size 5 mt
Face sizing "ground": element size 0,4 mt

Ive used the mesh quality to spot the bad elements and all of them are situated close to the floor and/or near the intersection with the files of vinetrees.

Ive tried to use patch independent tetra on the air domain but the domain is so large that the computer doesnt mesh it, even after a couple of hours.

Every piece of advise is highly appreciated (:

Thanks in advance!

im using cfx mesh btw

You are using a tetrahedral mesh method on a geometry that could be filled with hexahedral elements, that will improve the quality.

Why do you have to model so many rows of square cylinders? Cannot you model a few and use symmetry or periodic boundary conditions?

Well i forgot to mention a detail. In the middle of the whole air volume there is a geometry like 30 cm x 30 cm big (see picture attached). That being said, according to the mesh control tools there are no bad elements near that geometry, all of the them are placed near the ground.

I tried using hex dominant method on the air domain(with and without all quads activated) but the mesh quality doesnt improve that much (skeewness stay the same and orthogonal quality goes from 1E-5 to 8E-4).

What else can i try?

The hex dominant method is not suitable for CFD, rather it is more an option for FEA of non-thin bodies.

Yeah ive heard that, but i tried anyway, im running out of ideas...

It is difficult to see from your pictures but could you slice the geometry (e.g. in DesignModeler) so that the local geometry (in the separate last picture) can have a local tetrahedral mesh in that local region and the rest of the volume can be made using hexahedral elements. It should be straight forward to slice the domain into nine or more rectangular regions and use; e.g. patch conformal tetra method of the volume with the complex shape in it and MultiZone for all the others. Whether you need to have conformal nodes at the interface is up to you and the needs of the simulation. You have considerable geometry scales: ones of millimetres for the vines to hundreds of meters for the fluid domain: that's a factor of 100,000.

Hello,

Sometimes it is better to leave it automatic.

In my experience, avoid hard settings unless clearly necessary. Set local sizing for problematic features. Use pinches for features causing bad elements and use mesh defeaturing. Play with tolerances. If you use Proximity refinement then play with the number of layers in gaps. Star from a coarser mesh. And play with growth rates.

I'd also suggest to part the geometry into simpler zones. It has worked for me in some complicated situations. This will require you to deal with zone interfaces, but the mesh can be improved.

Also your geometry seems sweepable. This would be a huge improvement.

Cheers,
Fole.

I didn't read the non-sweepable thing of your geometry.

I am used to mesh with T-grid, anyway I can try to give you some tips as well.

The face mesh size seems to me quite big: 0.5m when the face file has a length of 1 m will make just two cells (if I am not wrong with the meaning of face size).

Moreover, I think there is an automatic defeaturing applied to your case, if so your geometry could be deformed and this could explain some bad cells.

Are you generating as well a BL?


To have some better ideas of the ongoing problem it would be helpful to visualize the mesh on a plane perpendicular to z at different z. If you can post those pictures we can have a better look to the mesh and try to understand what is the problem.

Good luck!

Thanks for your tips guys. I tried them but didnt work. What i finally did was change the shape of the rectangular prisms from a square to a circle (so they became a lot of cilinders) and that way it worked like a sharm.

Be careful to cylinders, it is not straightforward that you get the right flow topology around them

Sent from my D5503 using CFD Online Forum mobile app

What exactly do you mean by flow topology?

They are meant to be a porous domain by the way...

In general the flow around a cylinder is not an easy task to reproduce by CFD. Now if they are porous media it may work but I never used them