[PSYMN]

1) I would go with option a or b... Except create a material point instead of a "body". If you let it create its own, you end up spending more time at the end figuring out which material is where...

2) Not sure... I see the pic you sent, but it is hard to know why it would do that. Are there points or curves pulling the mesh? Is there a periodicity setting pushing it? Maybe adjusting the edge criterion or triangulation tolerance would fix it... Maybe you have a smooth option on that allows nodes to move off the surface... Not sure.

[Ehab44]

Dear Mr. Simon,






Thank you for your reply.


Please check your email.


When I computed the mesh and export it to Fluent, I found new surfaces detected in Fluent which are random triangles and I found the mesh missing some cells as the photo I sent you before.






Yours,
Ehab

[PSYMN]

Hey Ehab,

I took a look at your model, specifically that particular part where you were having problems.

The little triangles everywhere was ICEMCFD trying to close holes. You can see it put those all into a subset so you could zoom in and find the problems. When I turned on the surfaces, I saw that they were sloppy.

Ehab_TriTol_001.jpg

Can you see all the little gaps? The mesh sees it and guesses at what it should do. In some cases, it sees it as a hole and tries to pave over it.

If you increase your tri-tolerance (I went to 0.00001), it looks better, but then since your geometry actually does have holes (in other parts), you get some leakage...

Ehab_TriTol_0001.jpg

Ehab_TriTol_00001.jpg

I tried it again after dropping the edge criterion from 0.2 down to 0.1... That looked better, but it still said there was leakage between two material points (not between the materials and the outside). You could delete a material point and try again or sort out the geometry problems between them.

I didn't have time for those, so I just choose the "only shells" option, then smooth the heck out of the surface mesh and run a delaunay fill to get the volume mesh back again. Delaunay volume mesh looks better than Octree anyway.

Ehab_TriTol_00001_Meshed.jpg

[PSYMN]

Oh yea,

You best bet for an easy mesh is to try and get a cleaner version of the geometry. Where did you get it? If it was IGES, can you get ACIS or some other higher format? Maybe native CAD import?

[Ehab44]

Dear Mr. Simon,


Thank you for your reply.

I created the geometry in Inventor and I created the zones in Design Modeler.

The question is: when I was using Ansys meshing, these problems never happened !!. I mean the geometry should be ok.




Yours,
Ehab

[PSYMN]

So this came into ICEM CFD from an AGDB file? Interesting.

In ANSYS Meshing, they have the concept of the solid. This gives it some advantages with geometry like this.

Why not use ANSYS Meshing then?

Best regards,

Simon

[Ehab44]

Dear Mr. Simon,

I was already using AM for approximately one year. But I faced a big problem which is I can not obtain a consistent mesh. If I used the advanced sizing or even if I let it Off and I meshed the model manually, each time I obtain a mesh with different number of elements although I am using the same parameters. And this difference in the mesh leads to different results in Fluent.

I am really confused .... That is why I tried to use ICEM.

I know I am wasting your time, but I do not know what to do ??.



Yours,
Ehab

[PSYMN]

Small changes in mesh count should not significantly affect your Fluent results. If you found that they did (same model, just meshed a second time), you probably need a finer mesh or other changes to your setup anyway.

When you make a parametric change to the model, any tetra/prism mesher will give you a different number of elements anyway.

If you really want the same mesh topology between parametric runs, then ICEM CFD Hexa can do that for you.

If you want that with a tetra/prism mesh, you may need to look into morphing technology. I recommend RBFMorph. There is also some morphing technology built right into Fluent.

Best regards,

Simon

[Ehab44]

Dear Mr. Simon,


Will ICEM CFD Hexa work for this complex geometry ?. If yes, will it be difficult or what ?.

Also, where can I find the morphing technology you are talking about ?.



Yours,
Ehab

[Ehab44]

Dear Mr. Simon,


If you see that AM can fulfill the job. One of the problems that I faced was the Aspect Ratio when I used inflation.

How can I solve this problem ? The max AR reaches 1000 but the average value is about 10.



Yours,
Ehab

[Ehab44]

Dear Mr. Simon,


I really confused. I am sending you another tetin file (please check your email) in which I just change the maximum size for different parts.


When I computed the mesh and export it to Fluent, No missing cells and everything is OK.


How does it come ?.






Yours,
Ehab

[Ehab44]

Dear Mr. Simon,



Please check the attached file at your email. This is the tetin file for one of the cases that I was running.
I computed the mesh first then I computed the mesh again after checking "create prism layer" and I told him to Merge the new mesh not Replace.
As I told you before the program hangs at a certain point and you can check it.

Is this issue related to the quality of the mesh (tetra, prism, .....) or not.


Yours,
Ehab

[PSYMN]

1) Hexa is certainly doable, but I would not consider this a good case for your first hexa model. You need to work your way up to this level.

2) changing the mesh size (particularly increasing it) reduces leakage and all those sorts of problems go away. ICEM CFD is very forgiving of sloppy geometry if the mesh size is larger than the flaws.

3) "Merge" just means to load the new tetra/prism mesh along with the previous tetra mesh... In your case, it means you have two overlapping meshes. You should have picked "replace". The program shouldn't hang though... Maybe you had memory problems or some other issue. ICEM CFD doesn't care if you accidentally load two overlapping meshes.

[Ehab44]

Dear Mr. Simon,


You wrote me before "I recommend running separate steps. One for tetra, then check it, maybe smooth it and then run prism as a separate step."

What do you mean by several steps if what I did by using merge is incorrect. Please advise ...

Also, you wrote in your last post that increasing the mesh size may solve the problem of strange surfaces. You mean the total number of elements or the maximum size that we define under global mesh settings. I am asking about this point because I decreased the maximum size under global mesh settings.



Yours,
Ehab

[PSYMN]

Not sure why decreasing the mesh size (max size) would help... Don't have time to look into that now either.

Running separate steps is fine... It will take your tetra mesh and run prism... The output from the prism process is the prism.uns file, which it will offer to load. This prism.uns includes all your shells, tetras and prism elements. So you don't want to merge it with your previous tetra mesh, you want to replace it.

Best regards,

Simon

[Ehab44]

Dear Mr. Simon,


Thank you for your reply.

It seems you did not understand me.

I mean what do you mean by several steps ??. I mean I will create the mesh first without prism, then I will re-create it using prism and I will use Replace ... this means that I am creating a new mesh. So where are the several steps we are talking about ?.




Yours,
Ehab

[PSYMN]

You mentioned that you generate tetra/prism mesh in one step... You click that "prism" button, so it goes from geometry to tetra prism in one compute step.

I usually do not click that button. I generate only a tetra mesh... I smooth it several times (some with Laplace option on and then off). I may even delete the tetra mesh and refill with delaunay mesh and then smooth that.

Then I go into prism and generate a prism mesh.

When the prism mesher is done, it wants to load the new mesh (which includes tetras and shells), so I replace my old mesh with the newer one that includes the prisms...

Have a good week, I am going on vacation. In the mean time, try some tutorials or go back to ANSYS Meshing and don't worry so much about the small mesh changes...

[Ehab44]

Dear Mr. Simon,


First of All, Thank you for your continuous support.

My last question and then you can enjoy your vacation away from me but I will be waiting for you when you are back and I will tell you if there is any progress.

Based on your experience and according to my geometry, WHAT IS YOUR FINAL ADVICE ? ANSYS MESHING OR ICEM ?

I WILL GO FOR WHAT YOU DECIDE.


Yours,
Ehab

[PSYMN]

If it is working for you in ANSYS Meshing and giving you acceptable results, then why go anywhere else?

Only switch over to ICEM CFD (with its steeper learning curve, broken out process, etc.) if ANSYS Meshing isn't giving you the level of interaction you need or can't handle your model in a reasonable amount of time.

Small differences in the mesh are not a problem. If your solver is varying between different meshes of the same model, then you have a mesh dependence issue and need to fix it with solver settings and/or a finer mesh.

[Ehab44]

Dear Mr. Simon,


I hope you are fine.

I know you are in a vacation, so please reply when you are back.

I returned back to Ansys meshing as you told me. Then I installed Ansys 14 as I knew that its meshing module includes more options.
My problem now is that I feel that the Fluent solver is running slower than version 13. I have core i7, so I have eight processors and I am using parallel processing option.

The other thing is that if I defined the number of processors less than 8, I receive the following message (repeated as the number of the processors):
Rank = 3: Process affinity not being set (6)

In the same time, when I check the cpu performance through task manager, I find it from 85 % up to 95 %.

I do not know if there is something wrong or what ?



Yours,
Ehab