|
[Sponsors] |
January 16, 2013, 06:36 |
Dynamic Mesh on Sweep Mesh
|
#1 |
New Member
CFD
Join Date: Jan 2013
Posts: 23
Rep Power: 13 |
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 |
|
January 17, 2013, 04:55 |
|
#2 |
Senior Member
Marion
Join Date: Jul 2012
Location: France
Posts: 122
Rep Power: 14 |
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. |
|
January 17, 2013, 05:58 |
|
#3 | ||
New Member
CFD
Join Date: Jan 2013
Posts: 23
Rep Power: 13 |
Hi Marion, thank you for the reply!. Appreciate it.
Regarding your questions: Quote:
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. 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:
Any though will be really appreaciate it. Thank you so much, Regards, siefdi |
|||
January 17, 2013, 07:30 |
|
#4 |
Senior Member
Marion
Join Date: Jul 2012
Location: France
Posts: 122
Rep Power: 14 |
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. |
|
January 17, 2013, 08:45 |
|
#5 |
Senior Member
Rick
Join Date: Oct 2010
Posts: 1,016
Rep Power: 26 |
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 |
|
January 21, 2013, 05:18 |
|
#6 | ||||
New Member
CFD
Join Date: Jan 2013
Posts: 23
Rep Power: 13 |
Dear Marion,
Thank you for the reply, and please forgive me for the late responses,. I leaved my desk for a few days.. Quote:
I meshed the geometry using unstructured hexahedral, quite high skewness though, < 0.96. Quote:
Quote:
Quote:
I will try it out. I hope it works! Regards, siefdi |
|||||
January 21, 2013, 05:24 |
|
#7 | |
New Member
CFD
Join Date: Jan 2013
Posts: 23
Rep Power: 13 |
Hi Daniele,
Thank you for the reply, and please forgive me for the late responses,. I leaved my desk for a few days.. Quote:
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 |
||
January 21, 2013, 05:47 |
|
#8 | |
Senior Member
Rick
Join Date: Oct 2010
Posts: 1,016
Rep Power: 26 |
Quote:
can you post a sketch of your geometry with indicated boundary conditions and what you want to move? Daniele |
||
January 21, 2013, 06:07 |
|
#9 | |
New Member
CFD
Join Date: Jan 2013
Posts: 23
Rep Power: 13 |
Quote:
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 |
||
January 21, 2013, 06:22 |
|
#10 | |
Senior Member
Rick
Join Date: Oct 2010
Posts: 1,016
Rep Power: 26 |
Quote:
- fluid interior: rigid body (udf) - inlet face: rigid body (udf) - outlet face: stationary No need to add deforming zones. Daniele |
||
January 21, 2013, 08:53 |
|
#11 |
Senior Member
Marion
Join Date: Jul 2012
Location: France
Posts: 122
Rep Power: 14 |
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. |
|
January 30, 2013, 05:23 |
|
#12 |
New Member
CFD
Join Date: Jan 2013
Posts: 23
Rep Power: 13 |
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 |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Dynamic Mesh on Pintle type injector. | herntan | FLUENT | 16 | September 4, 2020 08:27 |
pls help. mesh collapsed with dynamic mesh. | wlt_1985 | FLUENT | 2 | May 7, 2020 10:42 |
Incylinder dynamic mesh with volumetric reaction | mas | FLUENT | 4 | May 3, 2012 10:22 |
dynamic mesh on a hexa grid | Manoj Kumar | FLUENT | 0 | August 21, 2007 07:41 |
Dynamic mesh + grid adapt = Crash! (Files included | BillH | FLUENT | 4 | July 24, 2007 15:31 |