CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Negative Element Volume_Moving Wall

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By ghorrocks
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 18, 2022, 07:40
Default Negative Element Volume_Moving Wall
  #1
New Member
 
Jonathan Fong
Join Date: Sep 2022
Posts: 4
Rep Power: 2
Jalathan is on a distinguished road
Hello All,

I am currently running a simulation that creates a wave. In order to assess its force acting on a wall. In the pictures below, they show the mesh, blocking and other information of what my model looks like.

I am currently always faced with a negative element error. I looked in other forums, and it is not my equation since this equation works well with a reduced size model.

The reduced sized model was 20m length and the moving wall moves at 0.044m to create a 80mm wave height at a certain distance.
The size i am working with is 200m and the wall moves at 1.5m to create a 1m wave height.

I am assuming the problem is that the moving wall is folding the longer the simulation runs. Cause if i run the simulation for 20s, it is able to complete. But if i run it for 50s. The error occurs. I wish to be able to run at longer times for more accurate wave height information.

There are two parts of this model, the bigger block which is the Water Tank and the smaller back block is the wave maker.
The end wall of the wave maker is the moving wall.

I've tried changing the time steps, which did improve it by a bit, but even if i decrease it further. It would still cause an error.

I've tried refining the mesh, at the wave maker block, at the slope, at the water level. But they all worked at a certain extent. Then i tried combining both mesh refining and timesteps. It still wont work.

My latest attempt is combing the water level refinement and decrease in time step and they are currently running right now.
But time is running short, i have been running different scenarios for the past 2 months and still no luck.

There is also another picture of where the location of the error is. I used a monitor point to locate it. So i know it should be the moving wall. But i don't know much beyond meshing and timestep to help me at the moment.

Thank you

Jonathan
Attached Images
File Type: png CFX-Solver Manager Error.png (12.7 KB, 7 views)
File Type: png Error Location.png (26.4 KB, 10 views)
File Type: jpg Mesh.jpg (60.9 KB, 8 views)
File Type: jpg Blocking.jpg (38.2 KB, 7 views)
File Type: png CFX-Pre.png (34.0 KB, 7 views)
Jalathan is offline   Reply With Quote

Old   September 18, 2022, 19:57
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,231
Rep Power: 135
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
There is an FAQ on this exact topic: https://www.cfd-online.com/Wiki/Ansy..._went_wrong.3F

Try the different weightings suggested in the FAQ. Also the debugging tip should help you work on the issue much faster.

In my experience, moving mesh in CFX stretches a mesh nicely but it does not do a good job compressing a mesh as it frequently gives mesh folding errors. I used to do a lot of IC engine simulations: If I started the piston at bottom dead centre and compressed it the mesh always folded; but if I started at top dead centre and stretched it then it worked fine. This includes the next cycle where the piston returns to top dead centre, as long as I started from TDC it would work fine.

So my recommendation is to start your simulation in the location where the mesh is fully compressed and stretch it. Starting at fully extended and compressing it always leads to problems.
Jalathan likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   October 2, 2022, 21:53
Default
  #3
New Member
 
Jonathan Fong
Join Date: Sep 2022
Posts: 4
Rep Power: 2
Jalathan is on a distinguished road
Hello Ghorrocks,

Thank you so much for the reply and assistance. Apologize for the late reply as i thought it would be best to try out everything you suggested first.

From your recommendation, Yes, my moving wall starts from fully compressed and then it starts to expand.

So, my simulation has worked. But correct me if I say anything wrong since I'm not an ANSYS expert. But the problem with my simulation was because I had too many nodes and elements for the timestep i used. So, the more nodes and elements I have from my mesh, the more i have to decrease the time step. The more I decrease the timestep, the longer my simulation would take. So I didn't have the time to keep decreasing the time step and wait for the outcome. Since this simulation took around 6days to complete.

So what I did was, I decreased by meshing while at the same time trying not to compromise the quality of the mesh. Eg. 100metres = 1000 nodes. So I decreased it to around 750 or 500nodes. The quality would be at 0.998 and it would drop to 0.995. Which is fine, I guess.

Thank you for the assistance,

Blessed Week ahead
Jalathan is offline   Reply With Quote

Old   October 8, 2022, 05:22
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,231
Rep Power: 135
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
You should not guess when you set your mesh size. Getting it correct is critical. Too big and your results will be inaccurate, too small and your model will take forever to run (if you are lucky enough to have a machine big enough to run it at all).

You should do a mesh sensitivity check where you run your simulation, and then re-run it with the mesh element length halved (so 1 hex becomes 8). Compare the results of the two simulations - if they are the same within a tolerance you are happy with then the coarse mesh is OK to use. If the results are changing too much then refine it again and repeat until it does become accurate enough.

You will find most simulations require far finer meshes than inexperienced people expect.
Jalathan likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   October 8, 2022, 05:59
Default
  #5
New Member
 
Jonathan Fong
Join Date: Sep 2022
Posts: 4
Rep Power: 2
Jalathan is on a distinguished road
Hello Ghorrocks,

Thank you for that recommendation and noted. I will run a mesh sensitivity test as my current simulations are almost finished. Then I'll will use these results for comparison in the test.
Jalathan is offline   Reply With Quote

Old   October 8, 2022, 06:10
Default
  #6
New Member
 
Jonathan Fong
Join Date: Sep 2022
Posts: 4
Rep Power: 2
Jalathan is on a distinguished road
Hello Ghorrocks,

Thank you for that recommendation and noted. I will run a mesh sensitivity test as my current simulations are almost finished. Then I'll will use these results for comparison in the test.
Jalathan is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[OpenFOAM] ParaView command in Foam-extend-4.1 mitu_94 ParaView 0 March 4, 2021 14:46
Issues With Exporting From GMSH rberdon Mesh Generation & Pre-Processing 0 February 11, 2021 12:11
temperature correction limited- Star ccm+ LpSingh STAR-CCM+ 15 September 29, 2020 12:06
Divergence in AMG solver! marina FLUENT 20 August 1, 2020 12:30
channelFoam for a 3D pipe AlmostSurelyRob OpenFOAM 3 June 24, 2011 14:06


All times are GMT -4. The time now is 18:23.