CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Overset meshing with rotational periodic BC for a wind turbine blade

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

Like Tree1Likes
  • 1 Post By dmirel

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 14, 2019, 00:26
Default Overset meshing with rotational periodic BC for a wind turbine blade
  #1
New Member
 
Islam H. Mohamed
Join Date: Oct 2014
Posts: 8
Rep Power: 7
Islam Hashem is on a distinguished road
I am working on CFD simulation of a wind turbine blade using STAR CCM+. I am using overset meshing; I made my mesh in Pointwise for the background (180 deg. segment with degenerate line "axis") and the blade (O-grid). Then I imported the volume meshes to STAR CCM+. I used sliding mesh technique to let the blade mesh (O-grid) rotate alongside two rotational periodic faces have a common line "axis". I checked the overset cell status and it was very nice as shown in the attached snapshots after switching the overset interpolation option from "Linear" to "Distance Weighted" as Linear gave an error when I initialized the interface. However, after one time-step (1 deg.), I got an error message telling me that 50 in-active faces are found in the background region. Do anyone here can help me to solve this problem ?

By the way, I set "axis" boundary condition to the degenerate line of the background mesh with the 180 deg. slice. Is that correct or not?

I uploaded some snapshots to help anyone to figure the problem out.

Thank you in advance.
Attached Images
File Type: jpg bg.jpg (85.2 KB, 26 views)
File Type: jpg blade.jpg (63.0 KB, 22 views)
File Type: jpg overlapping.jpg (183.0 KB, 27 views)
File Type: jpg degenerate line.jpg (122.2 KB, 20 views)
File Type: jpg blade-acceptor cells-before calculations.jpg (84.0 KB, 20 views)
Islam Hashem is offline   Reply With Quote

Old   November 14, 2019, 00:28
Default to be continued
  #2
New Member
 
Islam H. Mohamed
Join Date: Oct 2014
Posts: 8
Rep Power: 7
Islam Hashem is on a distinguished road
These two snapshots illustrate the error message after only one time step (1 degree of rotation)
Attached Images
File Type: jpg error.jpg (94.4 KB, 18 views)
File Type: jpg error2.jpg (95.6 KB, 10 views)
Islam Hashem is offline   Reply With Quote

Old   November 14, 2019, 11:15
Default overset mesh problem
  #3
New Member
 
demirel suleyman
Join Date: Apr 2017
Location: Turkey
Posts: 28
Rep Power: 5
dmirel is on a distinguished road
Hello Islam,

I had the same problems and fixed them following these steps.

For transient problems with moving bodies, set the time step such that the movement of the overset region within one time step meets the following conditions:
*When the time integration is set to the 1st-order Euler scheme, the maximum movement is the smallest cell in the overlapping zone.
*When the time integration is set to the 2nd-order implicit time integration scheme, the maximum movement is half the smallest cell size in the overlapping zone.

Hope it helps.

dmirel
Islam Hashem likes this.
dmirel is offline   Reply With Quote

Old   December 2, 2019, 00:05
Default the problem is fixed
  #4
New Member
 
Islam H. Mohamed
Join Date: Oct 2014
Posts: 8
Rep Power: 7
Islam Hashem is on a distinguished road
Hello dmirel,

Thank you so much for your reply. I am very grateful for your help. I agree with your answer but the problem in my case was in the definition of the motion as I have defined a motion for the blade mesh only. However, when periodic boundary conditions is employed, one should define the motion for both, the background and the blade.Now, the problem is solved after I set the motion to the background mesh too.

Kind regards,
Islam
Islam Hashem is offline   Reply With Quote

Old   April 19, 2020, 02:01
Default
  #5
New Member
 
Marium Mou
Join Date: Mar 2020
Posts: 29
Rep Power: 2
Marium is on a distinguished road
MR. ISLAM,
I'm also trying to import volume mesh from Pointwise to star. The problem is I have no parts, so I can't progress further. I don't know how to go further. it will be helpful for me if you can guide me on how to progress after importing volume mesh in star.
Marium is offline   Reply With Quote

Old   April 19, 2020, 11:38
Default Reply to Marium
  #6
New Member
 
Islam H. Mohamed
Join Date: Oct 2014
Posts: 8
Rep Power: 7
Islam Hashem is on a distinguished road
Quote:
Originally Posted by Marium View Post
MR. ISLAM,
I'm also trying to import volume mesh from Pointwise to star. The problem is I have no parts, so I can't progress further. I don't know how to go further. it will be helpful for me if you can guide me on how to progress after importing volume mesh in star.
Hello Marium ;

In my case, I haven't face any problem during importing my volume mesh from Pointwise to STAR-CCM+. I suppose that you choose your Solver in Pointwise to be STAR-CCM+ before exporting your volume mesh.

Hereby, I am attaching some snapshots for my steps from 1 - 5, I hope that could help you to solve your problem. It is supposed that every thing could work correctly after you followed the mentioned steps.
Attached Images
File Type: jpg 1.jpg (59.6 KB, 12 views)
File Type: jpg 2.jpg (58.2 KB, 12 views)
File Type: jpg 3.jpg (78.1 KB, 14 views)
File Type: jpg 4.jpg (80.9 KB, 11 views)
File Type: jpg 5.jpg (94.3 KB, 11 views)
Islam Hashem is offline   Reply With Quote

Old   April 19, 2020, 12:37
Default
  #7
New Member
 
Marium Mou
Join Date: Mar 2020
Posts: 29
Rep Power: 2
Marium is on a distinguished road
Thank you so much for your reply.
I have imported and run the simulation. The new problem that I faced is that i can not fathom the origin of the ship and that's why i can not set the isosurface for free surface view. As you can see, the free surface is quite lower than the draft line. 1.PNG
Can you share some insights on how I can change the isosurface in draft line? or how I can change the origin of the ship?
Marium is offline   Reply With Quote

Old   May 9, 2020, 10:22
Default
  #8
New Member
 
Marium Mou
Join Date: Mar 2020
Posts: 29
Rep Power: 2
Marium is on a distinguished road
Mr hashem I am having negative volume problem when importing mesh from pointwise starccm+. After running 40 mins/252 iterations it shows error implying that there is non-positive volume cell and the expanded error message shows reversed flow and matrices problem. I have used the mesh diagnostic before running, it shows the mesh has no negative volume. I have examined the mesh volume component in pointwise too and it shows a few negative cells
Can you suggest me what to do?
Marium is offline   Reply With Quote

Old   May 11, 2020, 02:25
Default
  #9
Senior Member
 
Ping
Join Date: Mar 2009
Posts: 460
Rep Power: 16
ping is on a distinguished road
if you are using a flat wave to apply the vof physics then you simply change the point on the water setting to move the water level.
or you can transform the whole mesh in either parts or in regions.
i would recommend you should be meshing in star for any ship type cfd to make use of the special mesh refinement features
ping 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
Wind Turbine blade in 120 wedge - boundary conditions Fcamp OpenFOAM Running, Solving & CFD 1 December 2, 2019 06:47
[ICEM] turbine blade meshing sk0pa ANSYS Meshing & Geometry 21 September 10, 2015 07:06
wind turbine blade flow simulation rsskarthikeyan FLUENT 0 May 27, 2015 05:40
Problem in conducting CFD of analysis of wind turbine blade atulpat CFX 16 August 17, 2013 04:09
Calculating lift force of a wind turbine blade problem LittleBart CFX 4 June 29, 2011 02:33


All times are GMT -4. The time now is 22:06.