CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Aspect Ratio, Mesh Expansion Factor (https://www.cfd-online.com/Forums/ansys-meshing/77857-aspect-ratio-mesh-expansion-factor.html)

 martinD July 6, 2010 09:26

Aspect Ratio, Mesh Expansion Factor

Hi,
I am simulating jet impingement. Fluid is blowing thrue a nozzle at the bottom of the plenum and impinges to the plate. we are using hexa meshing.

I ve created a blocking with 2 o-grids. one is due to the circular geometry and another to get blocks around solid walls (plenum walls). SST tur.model usage demands y+<1 which means very dense mesh at those walls, while in outer region it can be coarser.

A CFX solver output shows that the Aspect Ratio and Mesh Expansion Factor are much to big. i think that that is due to the elements at plenum bottom, where vertical mesh elements are small (y+), while in radial direction they are not, especialy in outer reagions.

My question is how to fulfil those two demands too?
one way is to increase the nodes number in radial direction, but these increase the total number too much
other way is probably the hybrid mesh with tetra elements in those areas.

 PSYMN July 15, 2010 21:44

Choices...

Without seeing a pic, I can only offer generic suggestions.

I think going with Tetra would require even more elements for a smooth transition and the final solution wouldn't be as good as with a pure hexa mesh.

I don't think the high aspect ratio elements are such a concern here because they align with the physics. However, you probably do need to reduce your growth ratio. There are two ways to do it (you pick ;) )

1) Increase your number of elements until you get the growth ratio you need.

2) Increase your initial height until you get the growth ratio you need with the number of elements you can afford.

Other than that, you could look at symmetry or sub modeling to focus your limited number of elements where you really need them.

 PSYMN July 15, 2010 21:46

Different topology

One final thought...

You might be able to fix it with a better topology... How are you modeling your impinging jet? i usually use an ogrid against the inlet for that. This lets me increase the number of elements just in the jet area without propagating them thru the whole model. If I saw a pic, I might be able to give a better (more efficient) topology suggestion.

Simon

 martinD July 16, 2010 07:31

Quote:
 Originally Posted by PSYMN (Post 267571) One final thought... You might be able to fix it with a better topology... How are you modeling your impinging jet? i usually use an ogrid against the inlet for that. This lets me increase the number of elements just in the jet area without propagating them thru the whole model. If I saw a pic, I might be able to give a better (more efficient) topology suggestion. Simon
http://www.djs.si/forum/

Problem with Mesh Expansion Factor was solved with setting up the growth ratio equal 1.2.

Regards, Martin

 PSYMN July 16, 2010 15:48

No need to penetrate the inner Ogrid all the way thru the large volume...

Is the flow going from the large plenum to the smaller space or the other way around? The smaller space is perfect, no need to change... but the larger space is wasting elements by extending the Ogrid all the way to the far wall...

When I do impinging nozzle (or collecting nozzles), I only extend the Ogrid in as far as the physics are likely to require...

So, if the large volume is the source, a short collector of no more than 2 or 3 times the diameter is needed. Split the volume about that far from he nozzle. When creating the inner Ogrid, just select that single block into the large plenum and all the blocks thru the hole and to the other side... Then just face the other side... It will save you a ton of elements.

If the jet is pointing into the large volume, then split that volume at what ever distance you think the jet will flow before slowing down significantly... Your current blocking is perfect if you expect the flow to hit the opposite wall.

If you don't get it, I could create an image.

 martinD July 28, 2010 08:59

1 Attachment(s)
Hi,
first of all thanks for your reply. The fluid is flowing from the larger plenum thrue the nozzle to the plate.

I have a questions regarding the inner o-grid. I agree with you that there is no need that the mesh is so dense all to the top. if I understand you right it should be something like that as it is shown in the picture (please see attachment). What bothers me is that the top block has no o-grid which should have due to the cylindrical shape (the mesh orthog. angle is now decreased from 35 to 13 degrees).

 PSYMN July 28, 2010 10:34

Steps...

Nope, that is not what I was suggesting... it will give bad elements at the corners of the circular face.

You can consider this model as having 2 Ogrids.

The first Ogrid is to capture the overall large cylinder. It should include all the blocks and have faces on the ends. Inner HGrid block would be associated with the outside of the nozzle.

This first ogrid would give you an outer 5 blocks and a central block on each end and a single central block in the nozzle.

Before adding the second Ogrid, you would split across the larger plenum at the depth you expect the "jet" to be. If that is the source side, just make the split about the diameter from the hole away from the side with the hole.

Now it is time to add the inner ogrid. Select the central 3 blocks. the one in the middle of the thinner disk, the one in the pipe and the first block in the larger disk. Do not select the second central block in the larger disk. Then also select the face on the wall of the thinner disk... Apply.

Get it?

 martinD July 29, 2010 02:54

1 Attachment(s)
Is that ok?
Next step is probably that o-grid around plenum bottom walls through the nozzle (actually all the blockings which I have seen have it) ?
http://www.djs.si/forum/blk_nozzle.jpg

Thanks, Martin

 PSYMN July 29, 2010 09:49

Don't get me wrong, your original and this latest are "ok", but it is not what I was suggesting. The blocking is more complex and puts a lot of elements along the wall. It will also have lower quality due to bending the boundary layer thru the hole...

If you were studying sludge or mercury sliding along the wall and falling thru the hole, this would be pretty good because it would give you extra elements to look at that viscosity...

I was suggesting a blocking more appropriate for an impingement in a lower viscosity pressurized flow where the physics would not need as many elements along the wall...

Send me the model and I will show you what I meant...

Tell me more about the flow conditions and I can improve my recommendation so the mesh can capture it better/more efficiently.

 PSYMN July 30, 2010 10:05

My suggestion.

5 Attachment(s)
Hey Martin,

I blocked it out quickly and will send you a replay file and blocking. You can see step by step what I did if you turn on "always update" and then "Do all".

I was pretty direct for the blocking, but I had some back and forth (wasted lines) with the edge params before I got to sizes I liked (for a very coarse model).

I put in the Jet Ogrid Split at the 1/3rd depth... You could adjust that based on your results (based on past tests or best guess) to get the best resolution. I marked this with #comment in the the replay file.

Then I put that second O grid in the blocks below this split with a face at the bottom.

Attachment 4261
Attachment 4262

At some later point I decided to show you how to fan this jet out (widen the plume)... Here I rescaled OGrid by 3... You should look at your results and adjust this accordingly for best resolution.
Attachment 4263
Attachment 4264
(After which, I aligned the top and removed its associations with that little circle so the mesh wouldn't contract after the expansion.)

If you had a combustor or something like that with lots of holes, you could create one of these plumes for each hole... They may be in an HGrid instead of at the center of an Ogrid, but the principle is the same. The Ogrid turns around within the plume allowing you to concentrate elements without propagating thru the entire mesh.

Anyway, here is my final mesh, it is a bit coarse and you may want to spend more time on the edge distributions, etc. but it is just to give you the idea.
Attachment 4265

 martinD August 3, 2010 04:06

Hi Simon,
really thanks for help once again. I have tried the blocking strategy you suggested and really works. The convergence of the simulation is really good.
Regards,
Martin

 All times are GMT -4. The time now is 04:40.