[Omarspace]

Hi Dear all,
I have searched the previous threads about this topic but i still need help in this so i am sorry if some of my questions were repeated and i didn't see them in the forum.
I am working on meshing Aortic Arch. I am trying to make tetra mesh + prism.
I have setup global mesh parameters , surface mesh parameters
Then I compute mesh using Octree
Then smoothing
Actually my initial mesh is nice w.r.t quality , Aspect ratio and orthognolaity.
then I try to add my boundary layers using prism option.
I set it to give me my boundary layer within 7-9 layers. I have tried to make it using one layer then subdividing or calculating the 9 layers directly.
then I do smoothing on 2 steps according to manual Aorta problem
First when PENTA_6 is freeze and second when it is smooth.
whatever the number of iterations .. my mesh is very poor ! very very high aspect ratio and poor orthog. near to zero actually.
Also, i got some errors while checking the mesh such double , volume orientation so ICEM will remove one of doubled elements and re-order nodes to get right orientation.
When I run my problem in Fluent it is unstable in the period of reversed flow and the solver diverges and exit
Do any one have recommendations about what i should do ?
Please help me If u can.
I appreciate all of your comments
Omar

[shereez234]

Do you perhaps have an image of your mesh? whats your y+ value and whats the initial layer height? If the Aspect ratio is big that means the transition between the octree and the prisms are too large I guess. ?

[Omarspace]

Hi,
Thanks dear for your answer
I am attaching images of my mesh at outlet and interface as well.
my Y+ didn't exceed 2.5 during Fluent run and I want it to be from 1-1.2 because i am using K-W sst or K-Epsilon family.
my Initial height was 0.02 ( the mesh is in mm ) I want 7-9 layers to reach 0.2 mm total height
Yes I think the same too as you
The inflated or prism cell has very low height because we want to see boundary layer but not very enough width because it will increase all of the mesh elements homogeneously
Thanks again

[shereez234]

Originally Posted by Omarspace

Hi,
The inflated or prism cell has very low height because we want to see boundary layer but not very enough width because it will increase all of the mesh elements homogeneously
Thanks again

Sorry for the late reply. My advice would be to make sure you calculate the correct inital height and total number of layers for the prism layers. And have a look into what ratio of prism growth you are using? perhaps 1.2 would be the good to go for I guess. You can use Pointwise website to calculate first layer height etc... And generate the Octree Volume mesh with correct curve sizes and surface triangle sizes..

After you are done convert the Octree mesh to a Delunay mesh ( You can use Delaunay Standard or Tglib with AF if you are using 14.5 or later I guess). before you run make sure you select use existing mesh and disable creating prism layers as they were already generated while octree volume meshing was running. And if you have more problems post a picture of a slice plane. Good luck

[shereez234]

And I forgot to say. The reason for this is Delaunay has a smoother transition than Octree So solvers like fluent like this kind of mesh

[Omarspace]

Hi Dear ,
Sorry for my late reply. I have did your recommendations and they affected my mesh greatly. I have realized that despite that overall mesh looks great but there are some elements in critical places with very low orthogonal quality. I am not sure that those are the reason of my divergence but i think so. what do you think ? They are in the inlet of Aortic Arch with almost zero quality + Reverse flow ... maybe really are they the reason of this divergence ? "It is turbulent problem too " I am attaching picture of those elements. Their number is small didn't exceed 50 or 100 while mesh is 500,000 but they are in boundary layer inlets and outlets.
How Can I change their orthogonal quality individually ?
Regards
Omar

[Omarspace]

The actual orthogonal quality in histogram for those elements ranges from 0-0.05

[shereez234]

If you don't mind share the project files from drop box or something. I might be able to have a look into it during this weekend.

[Omarspace]

Oh Thanks for your reply I wish I could but it is unfortunately forbidden by contract
Thanks again for your reply Shereez

[shereez234]

Oh okay my bad. My only advice now would be to smooth the mesh with orthogonality option chosen. And also are you using relaxation factors to control the equations in Fluent? turbulence viscosity, energy? which solver settings are you using?

If any one else have any experience in this problem please share your views to help out this user.

[shereez234]

Or you could create a subset for the worst orthogonal quality elements and smooth them - I guess

[Omarspace]

Hi Shereez, yes thanks a lot I solved it by increasing number of elements it is the only thing that worked.
Thanks for you

[Omarspace]

Hi Dear Sheerez,
Sorry to bother you again don't you know how can i mesh this stl geometry into hexa ? There is no points or curves how can i fit my blocks then ?
Thanks in Advance

[shereez234]

I have not personally worked with STL geometries. I do not know the exact procedure. Hope some one else helps you around here. But my guess is you run build topology with a small tolerance to extract curves

[ftab]

Originally Posted by Omarspace

Hi Dear Sheerez,
Sorry to bother you again don't you know how can i mesh this stl geometry into hexa ? There is no points or curves how can i fit my blocks then ?
Thanks in Advance

Hi Omar,
In biological cases you work more often with STL files received from segmentation of imaging outputs. So I do recommend you to get your hands dirty with them.
With STLs you can even triangulate the surface and base your volumetric mesh on the surface mesh and build up with Delauny.
You just import the STL file, build the topography with appropriate tolerance and then proceed defining the inlets, outlets and walls. Based on the fact that you want to use the already generated surface mesh, or making your own mesh you proceed with Delauny or Octree, respectively.
Checking and smoothing the mesh is also a very import. You can even do the check and smooth step in 2D on surface and make your own mesh from your own surface mesh into 3D with Delauny.
Simon Pereira (PSYMN) has explained the process clearly in several replies in the older posts.
If you need help, I can also give you some hints as I am also working in BioFluid Dynamics and CFD.
Good Luck!