Why don't we use domain interface to solve this problem?
 

Hi,

May I ask you a question about O-grid generation? :confused: Here is a picture. I'd like to generate a picture like B. But since I can't rotate my block, I always obtain A. How to solve this problem?

Best regards and many thanks,
lnk

what u want to do?

A=B. So it does not make any difference.

Here is the problem. The geometry I'd like to mesh is a connection of a tube with a cube. If I have the O-grid like A, I can't correct the bad quality meshes at the connection part of the tube and cube. So I try to rotate the O-grid to solve this problem.:confused:

Best regards and many thanks,
lnk

This is easy case for ICEM Hexa. If you can share your files, we can give a quick try.

just create points at the 2 exits of your model and associate the vertices of your o-grid to modifiy its shape. Then align the internal vertices of your o-grid with the vertices of the 2 exits of your model and you are all good !

Here is my file. Thanks you very much!

Best,
lnk

What do you mean by 'exits'? Won't that change my geometry?:confused:

Far, Broly. this geometry is not easy...very tricky... i've been fighting with it for more than 4 hours now.i thought may be li's strategy for blocking was incorrect, so i erased his blocking and tried to came up with a better one using bottom-up approach. I couldn't, then i came back to li's blocking, realized that he can never get a good quality because he needs ygrid when the arc's circle meets the tangent line, alse noticed that geometry needs some cleanup, there are additional surfaces inside (tube), maybe that's why. I don't understand why and how li did that blocking... i need a break. i hope i can wake up the morning and find your approaches...
@li i'll come back to your geometry tomorrow to finish it... i saw another thread where you're asking about ygrid, you have to merge before, and select the triangular shape, but i just don't know how you can do that with your blocking...

i'm going on a vacation on Sunday... like you said FAR may be this is easy geometry, i just need vacation...

Those kind of geometry are hard because your circle geometry meet the corner of a rectangular shape. So I think you can avoid bad elements at the intersection of those 2 shapes.
I don't have much type to take a look at the geometry, will try this week :S

Ok finally, I took some time to have a look.
Attached an example of blocking. you only need to do the association and maybe improve the position of some vertices.

You can't avoid some bad elements between the corner of your rectangle and the print of your tube, but 1/4 of O-grid help to handle it.

I tried that but I can't improve the quality because of the same reason. The quality at the attachment is the best I can do. :o

You can incraese the number of nodes, move the vertices in order to optmize the blocking. But you have to know that at some point, you won't be able to improve the mesh because of your geometry.

Yes. That's the problem. I can't make all my meshes have quality over 0.5.

Yep, but your biggest issue is not about the determinant, but about the min angle ... You can get a min determinant around 0.2, which is not that bad.
But there are few cells which min angle is between 0 and 9°, which could crash your solver ...
If you work hard and moving the vertices of the 1/4 of O-grid, maybe you could improve a little bit your mesh ...

Or maybe someone else could provide another blocking ?

Have fun ;)

You have to ask yourself one question:

Is it important that the geometric feature (the sharp angle) is represented by the mesh?

Or wouldn't the flow field be almost exactly the same if the sharp angle is not represented by the mesh? In this case: change the geometry to allow better meshing.

The blocking is wrong...
@stief, that's exactly what i was thinking. you are right. Why do we have to follow the geometry ?
how about something like this
https://dl.dropbox.com/u/35161486/manifold.JPG
someone correct if i'm wrong...

I correct some errors in the blocking (see attached).

And I fully agree with flotus ;)

I did in this way at the first time. It didn't work so I changed to make the mesh follow the geometry.

The pipe is not inside the cube. It goes through the cube. If the mesh doesn't follow the geometry, the mesh will have problem at the connection part too which is, I think, also difficult to correct. You can see my attachments. It is even clear at the mesh picture.


Best,
lnk

If the mesh doesn't follow the geometry, what should I associate the edges at the connection part to? To the circle or the rectangle? I tried both of them but neither of them shows a good result. If I just leave them there without associating, it turns to the result of the picture above (at the previous post) which is same as associating to the rectangle. At this attachment, you can see what if I associate it to the circle. The mesh at some places are missing.

that's what i'm trying to fgure out ...

a little update...
Here is what i tried today:
https://dl.dropbox.com/u/35161486/manifold2.JPG
Only one problem: i couldn't do this blocking after i changed the geometry by keeping only the tube and the small box in the middle, i couldn't do it whith the hole geometry. I don't know why...

This blocking is nice but doesn't change the fact that the elements at the conection between the circle and the rectangle are very bad. You can't avoid this, unless you change your geometry.

I think what flotus suggested was to redo your geometry by deleting the triangle parts ... because it might not be relevant for your calculation. And then, redo another blocking which would be simpler.
Flotus, correct me if I misunderstood you ;)

That is exactly what I meant.

If you give some Information about the flow you want to simulate, then maybe we can figure out how the geometry can be changed without altering the flow field significantly.

We can modify the blocking in the corner inside the box , but i think there is no option at the two extreme corners where lines have to be tangent to circle.

We can use options:

1) modify the geometry

2. apply tetra meshing in the box surrounding the circular pipe.

As in this picture, the flow is from the z direction in the tube. Some go y direction, some go -x direction, some still go z direction in the tube. The flow speed is quite low. The flow regime is basically laminar.:)

Best regards and many thanks,
lnk

you guys are right, i'm stubborn...

It's a quality to be stubborn when you have to deal with blocking ;)

Hi. Here is the problem we talked about a lot. I'm thinking about why don't we use domain interface to solve this problem? We don't have to make the nodes match at the connection part any more with the domain interface at CFX.

Since I'm fresh to this method, I'm wondering is the domain interface method accurate or not? By this method we can solve every geometry very easily. But life shouldn't be that easy. What's the drawback of the domain interface problem?

Best regards,
lnk

If you can wait until tomorrow, I can show you a picture which illustrates the drawback of non-conformal interfaces.
The accuracy is poor and the interpolation slows down the solution process.
Before adding interfaces, i would rather choose tet or poly meshes.

Edit: Here are the results of a simple heat conduction case with nonconformal interfaces. There are three interfaces in X-direction. You can clearly see the discontinuities in the temperature distribution, even when the mesh size on both sides of the interface is similar.

Thank you very much for your answer. May I ask if the accuracy is always this bad, in what case should we still use it?:confused:

Best regards and many thanks,
lnk

Hi

I'd like to test GGI to solve the problem. May I ask which button may I use to unmatch the mesh across the connection part?

Best,
lnk

The two faces of the meshes you are trying to join via an interface have to contain non-conformal nodes.
If the meshes are identical on the two faces, fluent matches the nodes automatically and creates an internal interface. I don't know how to prevent this.

So the easiest way is to create meshes with non-matching nodes at the interface.

Concerning your first question: as always, it depends on what you are trying to simulate. Non-conformal interfaces are definitely a no-go in a LES for example, but for the steady-state calculation of a global parameter like pressure drop between inlet and outlet the interpolation might be no problem.
As you can see, the question cannot be answered universally, so checking the influence for a specific case is definitely a good idea.