CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Dynamic Mesh on Sweep Mesh (http://www.cfd-online.com/Forums/fluent/111826-dynamic-mesh-sweep-mesh.html)

siefdi January 16, 2013 07:36

Dynamic Mesh on Sweep Mesh
 
Hi CFD Experts!


1. This is my first post, even though I have following this forum for quite some times as a guest.

2. I would like to ask something, if you dont mind,

3. Currently, I am doing heat transfer simulation for a box of fluid which has several pipes inside. Let says, it has 1 meter of height.

4. The very bottom layer of the box has been mesh-ed using tertrahedral-mesh.

5. Then, I used sweep-method to swept this bottom-layer verticaly along z-direction.

6. Now, I am trying to collapsing (opposite of expanding) this box along z-axis. I am hoping that the height of the box will be shorthen (reduced) from 1 meter to 0.9 then 0.8 then 0.7 ... at a certain time steps during calculation.

7. I did try to use dynamic mesh and write an UDF for the movement of the bottom-layer. However, it didn't work for collapsing the box but strangely (at least for me) it did works for expanding the box (I just change the direction of its movement from z+ to z-).

8. Of course, I did try to educate myself by reading FLUENT manual and other references, but still confuse... So, just thinking to share it and see if someone (or maybe everyone) here could give me some advices..

9. So the question is: Did I miss something here?

10. Sorry for the bad english.

11. Thank you so much in advances.

regards,
siefdi

Marion January 17, 2013 05:55

Hi Siefdi,

What do you mean by "it didn't work for collapsing the box"? Did it squeeze the 1st mesh and then crash?

Have you tried to change the collapse factor?

And lastly: do you really need tet mesh? can't you just sweep paved (=unstructured quad mesh) faces?

Marion.

siefdi January 17, 2013 06:58

1 Attachment(s)
Hi Marion, thank you for the reply!. Appreciate it.

Regarding your questions:

Quote:

Originally Posted by Marion (Post 402403)
What do you mean by "it didn't work for collapsing the box"? Did it squeeze the 1st mesh and then crash?

What I mean was: when I tried to decrease volume of the box (opposite of expanding), there was an error of "negatif volume", so that it didn't squeeze the mesh at all. Yes, I did read (quite a lot) about it in this forum but none of the suggested solusion works for me. So that I just wondering if dynamic mesh will works on the sweeped mesh? is it? :confused:

However, I tried to expand the box by changing the movement direction of the bottom plane and it works! Which make me believe that there was no problem with the UDF I used.


Quote:

Originally Posted by Marion (Post 402403)
Have you tried to change the collapse factor?

Yes, I did try to change the collapse factor in layering option (from as small as 0.004 to about 1) but it seems that it was not affected the simulation. Maybe I missed something here..


Quote:

Originally Posted by Marion (Post 402403)
And lastly: do you really need tet mesh? can't you just sweep paved (=unstructured quad mesh) faces?

Maybe I didn't explain it brief enough, sorry for that. For a better understanding, I attached sketch of my geometry (sorry for not provide original geometry because I am not having it right now; not on my desk)

Any though will be really appreaciate it.

Thank you so much, :)

Regards,
siefdi

Marion January 17, 2013 08:30

Siefi,

Well the geomrtry you are showing can be meshed using hexahedral mesh only - il will provide better results and I think it is easier to control in Moving Deforming Mesh strategies.

I have done a lot of layering, and when you say that you get "error: negative volumes" - that's what I call crashing :)

1. Are you sure that the moving wall doesnt move too fast? i.e. if in 1 time step you move of more than your element size Fluent will crash

2. Check the definition of the boundaries (walls & fluid)

3. I've found that increasing the number of iterations and decreasing the Convergence Tolerance helps as well.

4. If you can't find anything wrong, and it still doesn't work: try it in 2D. That way you can check if it's an issue with the settings of the layering / the way you defined the motion or if it is a 3D issue.

I hope this helps,

Marion.

ghost82 January 17, 2013 09:45

Hi,
I think you can use layering only if you have hexa or wedges cells in 3d or quadrilateral in 2d; for tetra you can try to use remesh.
Better build hexa mesh with layering dynamic mesh option.
Daniele

siefdi January 21, 2013 06:18

Dear Marion,

Thank you for the reply, and please forgive me for the late responses,. I leaved my desk for a few days..

Quote:

Originally Posted by Marion (Post 402431)
Siefi,

Well the geomrtry you are showing can be meshed using hexahedral mesh only - il will provide better results and I think it is easier to control in Moving Deforming Mesh strategies.

Wow, I did write tertrahedral! I am sorry,.. my bad.. what I really mean was (unstructured) hexahedral.. (need some sleeps here)
I meshed the geometry using unstructured hexahedral, quite high skewness though, < 0.96.

Quote:

Originally Posted by Marion (Post 402431)
I have done a lot of layering, and when you say that you get "error: negative volumes" - that's what I call crashing :)

Ah oke, noted :)


Quote:

Originally Posted by Marion (Post 402431)
1. Are you sure that the moving wall doesnt move too fast? i.e. if in 1 time step you move of more than your element size Fluent will crash

I did play with the velocity and time step to ensure that moving wall doesn't move too fast. In fact, I reduce time step to a very small number, as small as 0.001 s just to make it sure. However, it still crash, unfortunately.

Quote:

Originally Posted by Marion (Post 402431)
2. Check the definition of the boundaries (walls & fluid)

3. I've found that increasing the number of iterations and decreasing the Convergence Tolerance helps as well.

4. If you can't find anything wrong, and it still doesn't work: try it in 2D. That way you can check if it's an issue with the settings of the layering / the way you defined the motion or if it is a 3D issue.

I hope this helps,

Marion.

Thanks for the suggestions, really aprreciate it!
I will try it out. I hope it works!


Regards,
siefdi

siefdi January 21, 2013 06:24

Hi Daniele,

Thank you for the reply, and please forgive me for the late responses,. I leaved my desk for a few days..

Quote:

Originally Posted by ghost82 (Post 402444)
Hi,
I think you can use layering only if you have hexa or wedges cells in 3d or quadrilateral in 2d; for tetra you can try to use remesh.
Better build hexa mesh with layering dynamic mesh option.
Daniele


Thank you for the suggestions,. I did use unstructured hexa mesh and layering dynamic mesh as you suggested.
Well, my set up are as follows:
- bottom layer : rigid body (moving with a certain velocity defined by UDF)
- internal fluid : deformed
- symmetry layer surrounding the box : deformed
- outlet layer: stationary

Any advices will be appreciate it..


Regards,
siefdi

ghost82 January 21, 2013 06:47

Quote:

Originally Posted by siefdi (Post 403069)
Hi Daniele,

Thank you for the reply, and please forgive me for the late responses,. I leaved my desk for a few days..




Thank you for the suggestions,. I did use unstructured hexa mesh and layering dynamic mesh as you suggested.
Well, my set up are as follows:
- bottom layer : rigid body (moving with a certain velocity defined by UDF)
- internal fluid : deformed
- symmetry layer surrounding the box : deformed
- outlet layer: stationary

Any advices will be appreciate it..


Regards,
siefdi

Hi Siefdi,
can you post a sketch of your geometry with indicated boundary conditions and what you want to move?

Daniele

siefdi January 21, 2013 07:07

1 Attachment(s)
Quote:

Originally Posted by ghost82 (Post 403075)
Hi Siefdi,
can you post a sketch of your geometry with indicated boundary conditions and what you want to move?

Daniele

Hi Daniele,

Thanks for the reply,

Actually I don't want to move anything, I just want to shrink (opposite of expanding) this geometry (attached) on the Z-direction so that its height will be decreased by the time; with the body itself just stay still.

As for boundary condition,
- bottom layer : input,
- surrounding wall layer : symettry
- top layer: output

Thanks in advances for your help,.

Regards,
siefdi

ghost82 January 21, 2013 07:22

1 Attachment(s)
Quote:

Originally Posted by siefdi (Post 403082)
Hi Daniele,

Thanks for the reply,

Actually I don't want to move anything, I just want to shrink (opposite of expanding) this geometry (attached) on the Z-direction so that its height will be decreased by the time; with the body itself just stay still.

As for boundary condition,
- bottom layer : input,
- surrounding wall layer : symettry
- top layer: output

Thanks in advances for your help,.

Regards,
siefdi

So, if I understand well, I would set:
- fluid interior: rigid body (udf)
- inlet face: rigid body (udf)
- outlet face: stationary

No need to add deforming zones.

Daniele

Marion January 21, 2013 09:53

If you put the fluid in rigid body then I think Fluent will try to move this part (i.e. all the cells) as a whole, nothing will deform.

Here is what I would do:

Inlet = moving rigid body --> apply the motion to that, and in the MDM panel specify the size of the elements in the fluid zone.

It should work with only this defined.

But sometimes it doesn't... and then you have to specify the symmetry and fluid as deforming, and the outlet as stationary.

This is why I like to start with 2D, to make sure the problem is identified. it takes 30 min and it is worthwhile.

Last but not least, to be independent from udf problems, I use profiles for velocities.

Regards,

Marion.

Marion.

siefdi January 30, 2013 06:23

Hi Daniele and Marion,.

Sorry for the late responses,.. as I travelled around recently.
Well, I still trying to solve this case but I need to halt it at the moment as I have to solve a new different case first.
Anyway, thank you so much for all the helps. Really appreciate it.

Regards,
siefdi


All times are GMT -4. The time now is 09:51.