High skewness problem
 

Hi,


I had a problem with my skewness in a rectangular model of a room. But I solved it with inflations and sizing. Now its under 0.86. But my first question is, can it be under 0.94 to be acceptable?

My second questions is that now I am modeling a room with an entrance (two rectangles and i made a small hole, about 1.4 meter long and 0.05 m high as a opening. Now my skewness is so high, in the area of the hole of the door. And it will not let me do first layer thickness.

Any ideas how to solve this?

Thanks again for all help here :)

With regards to your first question about the skewness metric value of 0.94 the following general guidance is given in the ANSYS Meshing Online Training Material (Lecture 7: Mesh Quality & Advanced Topics):

Skewness
0 to 0.25: Excellent
0.25 to 0.5: Very good
0.5 to 0.8: Good
0.8 to 0.94: Acceptable
0.95 to 0.97: Bad
0.98 to 1.0: Unacceptable

Orthogonal Quality
0 to 0.001: Unacceptable
0.001 to 0.14: Bad
0.15 to 0.2: Acceptable
0.2 to 0.69: Good
0.7 to 0.95: Very good
0.95 to 1.0: Excellent

This material is on the ANSYS Customer Portal and as a commercial or academic customer you can (and should) download and read this.

To better help with the second question you should post some images of the problem mesh.

Hi miquiita,

To remove high skewness near holes you have to give small element size near holes. Use of 'sizing' function under mesh will help you in that.

You may also use 'Sphere of influence' if you know the area where you have high skewness.

Hope it helps

Cheers
KAPI

Hi thanks guys, I just got the information about the skewness to be less than 0.86 from some colleges here at my University. I read the documentation, but got confused due to this information. They told me tetra should have under 0.86 in skewness.

I posted a photo of the room and the places of high skewness. The room is two rectangular areas connected together.

Also if you guys have tips of how to solve the probelm of chosing a timestep, I read the guide and tried the tips of calculating a physical timestep and so, but my model ran 2000 iterations on 0.1s without coming to a low residual of e-004.

Thanks.

Here is the mesh also

by quick search I found this

http://www.cfd-online.com/Forums/flu...time-step.html

Hope it helps

Cheers
KAPI

Hi thanks, I had a look at that already and tried it, does not work well for me though my smallest cell is very small and then the velocity only around 2-3 m/s

Why dont you try and give a lower timestep say 0.001 and see what you get.

What i do personally( depends on different geometry and mesh) is to start with 0.001 and see how it goes for few iterations and if I see it is going fine I increase my timestep.

Try and do this and you mite get right answer to your question.


KAPI

Hi thanks I done that too. But it got worse, take so long for my iterations to go and I have no time to do that. But seems like this will have to be the solution then. But I solved the problem with the skewness.

Solution with high skewness is not very accurate.
You need to first reduce skewness and then mesh again and run, thi sway the result accuracy will increase.

Can you share your geometry? From the pictures you posted, I'm sure you can create a hexa mesh and the skewness issue will be resolved.

Best,
Rahul

Hi here is the geometry of and the mesh I am trying to solve. The problem is in the smaller corner of the bigger part of the room. I have a skewness of 0.99 now.

So to the question, I have no idea of the timestep, due to I tried so many different numbers but they flats out after 70 iterations of e-002 and what I know is that they do not increase again after that.

Thanks for any help really wanna finish my thesis now.

Hi miquiita,

As I said before you should first fix your mesh then worry about time-step and solution.
0.99 skewness is quiet bad and it will not give you result close to accuracy.
As I suggested before try to use "sizing" function on your mesh and your skewness will drop dramatically.
Select the body/face/edge which has high skewness and give it right element size and try to use "behavior = hard" when you do sizing.

Once you are satisfied with your mesh, you will see that your solution will converge fast in less iteration.

Hope it helps,

Cheers
KAPI

Sorry this is the problem area

Hi miquiita,

You did a good job by splitting the rotational region and the stationary regions in your geometry. I'm sure, if you use Mapped Face meshing along with Sweep method, you can create a much better hexa mesh and reduce the skewness drastically. The problem regions as shown in the attached figure, are the regions which can easily have a hexa mesh.

Refer "Introduction to ANSYS Meshing" from Ansys Portal and specifically go through the tutorial "Mixing Tank" to get a better picture of how the mesh should be.

Best,
Rahul

Thanks so much for the information but when I try this method my inflations of the ceiling fan does not work...do you know why?

Hi miquiita,

Refer attached tutorial from Ansys Portal. You can see how to set the inflation for your case.

http://goo.gl/KhxIlI

Best,
Rahul

Hi the problem lays in the small box connected to the bigger one and its faces connected that gives high skewness. How can that be fixed?

As I told you before, create a hexa mesh in all the regions except for the rotary fan region. If you use tets in your case, you will face skewness problems in your mesh.

Best,
Rahul

Hi thanks I try again, why would hexa mesh be better? I am just curious.