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

Issue on conducting heave mode on airfoil using CFX?

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 9, 2020, 22:50
Default Issue on conducting heave mode on airfoil using CFX?
  #1
New Member
 
Andro
Join Date: Sep 2019
Posts: 8
Rep Power: 2
androm is on a distinguished road
Hello,

I am trying to do heave mode on airfoil using CFX. I used structure mesh using sizing and bias, I did make the bias too high in the y-direction to get the Yplus 1, however, when I do that it give me a negative volume in the solver or fatal overflow. How can I solve this problem?
I tried to increase the time step but still these errors come out to me. I tried increasing the coefficient loop instead of using 5 I used 7 and I even used 10 but It is still not working. I found out this is a common error if I used the mesh deformation, and the only way to overcome these errors is to make the first boundary layer far from the Yplus 1, If I used 2, or 3 I will be get result but the solution does not seem right compare to the paper that I am studying. If I used Yplus near 15, it gives me solution near the right result that is in the paper. Is there any explanation for that? I am doing laminar, and for heat transfer, I am using thermal.


Another question, I know if I used dynamic mesh option instead of mesh deformation, I may get better solution according to what I have read from several previous threads, Can anyone guide me with reference to read or tutorials that could help me?

Thanks In Advance,

AM
androm is offline   Reply With Quote

Old   February 10, 2020, 00:02
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,061
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I don't quite understand your question, but you appear to be getting negative volume errors when you have a y+=1 mesh but you are concerned about accuracy if you decrease the mesh size.

My comment on this is that you should not assume that you need y+=1. Many simulations run fine with a much coarser mesh than this. Also I would do some validation on a simple model before starting your complex heave model.

I would recommend you do a fixed mesh simulation of your airfoil shape and do a mesh sensitivity study. This will determine what mesh (and time step and convergence criteria) you require for an accurate solution. Once you know these parameters you can do the more complex heave simulation in the knowledge that your approach should be accurate. It might tell you a coarser mesh is OK, which means the negative volume element error you are currently getting is not relevant.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 10, 2020, 01:19
Default
  #3
New Member
 
Andro
Join Date: Sep 2019
Posts: 8
Rep Power: 2
androm is on a distinguished road
Yes, I am concerned about the accuracy. When I did the steady state case to check the lift coefficient and drag coefficient, they seems have the same response even if I used Yplus 15 and not 1.
For the mesh Sensitivity (time step and convergence). For the steady state case, the residuals reach the convergence value (1e-6). For the time step, how to check its sensitivity.

I have attached the residual for the steady state and transient, the Cl and Cd convergence, and Cl and Cd during the heave motion, please, can you look at them and give me your feedback. Thanks.
Attached Images
File Type: jpg SS_Residual_1.jpg (69.7 KB, 2 views)
File Type: jpg SS_CL_CD.jpg (68.7 KB, 2 views)
File Type: jpg Residual.jpg (77.5 KB, 2 views)
File Type: jpg Result_1.jpg (82.1 KB, 3 views)
androm is offline   Reply With Quote

Old   February 10, 2020, 01:49
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,061
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Mesh size - so it looks like you can use y+=15. In that case you won't get the negative volume elements error, so you don't need to fix that problem.

Time step - it is only of significance for transient simulations. You double or halve the tiem step and see if that changes your results.

Your transient results looks good so far. There is nothing obviously wrong there. But now the issue is to do sensitivity studies on anything you have not done yet (for instance time step size) to check that is OK.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 10, 2020, 02:22
Default
  #5
New Member
 
Andro
Join Date: Sep 2019
Posts: 8
Rep Power: 2
androm is on a distinguished road
I did time step checking for the transient case, I used time step equal to periodic time divide by 100 and the other one is divide by 250 and they are almost the same, this means that time step has no effect if I used 100 time step, is that time sensitivity test?

Do I get the same result if I used dynamic mesh instead of mesh deformation?
Attached Images
File Type: jpg Velocity_0s.jpg (44.5 KB, 5 views)
File Type: jpg Velocity_0s_2.jpg (31.8 KB, 5 views)
androm is offline   Reply With Quote

Old   February 10, 2020, 03:47
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,061
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Yes, that is a time step sensitivity check.

There is no fundamental between dynamic mesh and moving mesh. When a new mesh is generated with moving mesh the previous step results are interpolated onto the new mesh, which is exactly the same process as dynamic mesh. The difference is dynamic mesh can be an entirely new mesh, whereas moving mesh is just the same mesh distorted a bit.

You normally only consider dynamic mesh when the motion is too large for moving mesh to work well on. If you are getting negative volume element errors this is a sign dynamic mesh might be a good thing to consider.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 10, 2020, 15:48
Default
  #7
New Member
 
Andro
Join Date: Sep 2019
Posts: 8
Rep Power: 2
androm is on a distinguished road
I am doing low frequency in this case, but when I increase the frequency to higher value, I get negative volume, that means I need to use dynamic mesh. Please, can you recommend a reference to read or video tutorial to watch that could help me to do dynamic mesh for airfoil or cylinder or any shape? Thanks.
androm is offline   Reply With Quote

Old   February 10, 2020, 17:36
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,061
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
There are dynamic meshing tutorial examples in the ANSYS customer page. I think they are under ANSYS workbench rather than CFX.

I don't think these examples are available in the ANSYS student page. Stuff this complex is beyond what they support for students.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 11, 2020, 03:40
Default
  #9
New Member
 
Andro
Join Date: Sep 2019
Posts: 8
Rep Power: 2
androm is on a distinguished road
Thank you for your replies. I am doing my thesis and I need to learn this stuff to finish it so I will try to contact them and see if they have tutorial video or book for dynamic mesh.
androm 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
Issue plotting Cp distribution graph for an airfoil lewis donnelly STAR-CCM+ 2 November 13, 2019 14:24
Airfoil 2D simulation convergence issue frossi FLUENT 9 October 25, 2019 11:12
rhoCentralFoam inviscid airfoil issue (Foam::error::printStack(Foam::Ostream&) at ??) kmkb21 OpenFOAM Running, Solving & CFD 1 March 1, 2018 02:07
import airfoil from text file for CFX frossi CFX 2 October 30, 2016 19:00
airfoil mesh genaration and simulation with a trip on surface issue rajibroy Mesh Generation & Pre-Processing 1 December 3, 2014 03:04


All times are GMT -4. The time now is 09:32.