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

STAR-CCM+ - Unsteady Turbulent Solution not converging

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 17, 2019, 18:42
Default STAR-CCM+ - Unsteady Turbulent Solution not converging
  #1
New Member
 
James
Join Date: Jul 2019
Posts: 5
Rep Power: 3
mrstew is on a distinguished road
Hi All,

First-time poster here, been lurking for a while and thought I might as well ask this, as other posts with similar titles haven't helped.

I've been running some unsteady simulations on a pair of wings, one is a standard NACA profile and one is the same profile with some geometric modifications, that primarily impact the boundary layer (in theory!).

I've been trying to get the simulations to work for months, using different sized meshes, different models, different domain sizes, etc. etc. to no avail.

I was hoping someone here might be able to help me work out what's wrong with my setup. I've attached some pictures to help illustrate the problem.

I'd imagine that in an ideal (converged) case, the lift, drag and spanwise force values would flatten out and only oscillate slightly due to vortex shedding, but in my simulations, they started off increasing/decreasing smoothly only to freak out and start oscillating wildly.

Further info:

The domain is 4m long, 1m high, and 0.02m deep (spanwise). The wing is around 0.15m in chord length and is right in the centre of the domain. There are periodic boundaries to the left and right of the wing, and all walls (other than the wing surface) are set to no-slip.

There are around 2.6m cells in the domain, one of the images should show the mesh around the wing itself. I plan on doing mesh independence testing, but I think I need the baseline sim to converge first.

The 'inlet' wall is set up as a velocity inlet, with a velocity of 20m/s, and the outlet is a pressure outlet with a pressure of 0Pa (reference pressure is 1 bar).

The time step is 2E-04, and there are 50 iterations per time step.

I hope this is enough info to go off if anyone is willing to help, if more info is needed I can attach screenshots etc. in the replies.

Cheers,
J
Attached Images
File Type: jpg Courant and Spanwise.jpg (115.1 KB, 18 views)
File Type: jpg Mesh Medium.jpg (198.3 KB, 21 views)
File Type: jpg Wall Y+ and Drag.jpg (113.5 KB, 19 views)
File Type: jpg Residuals and Lift.jpg (100.9 KB, 14 views)
File Type: png Physics.PNG (33.6 KB, 13 views)

Last edited by mrstew; August 17, 2019 at 18:43. Reason: Added time step
mrstew is offline   Reply With Quote

Old   August 18, 2019, 05:59
Default Including pictures of dodgy mesh on one simulation
  #2
New Member
 
James
Join Date: Jul 2019
Posts: 5
Rep Power: 3
mrstew is on a distinguished road
Possibly contributing to this problem, on one of the simulations, there is a region filled with dodgy-looking cells. It's almost as if the cells are just missing, and there are many strange-looking cells of random shapes.

I checked the surface geometry and it seems fine, so I'm a bit confused by this.

Info;

I'm using the advancing layer mesher with 30 layers, a thickness of 0.005m and a stretching factor of 1.17, with a base size of 0.05m.

Does anyone know how I might fix the mesh?

Cheers,
J
Attached Images
File Type: jpg Broken Mesh.jpg (124.6 KB, 21 views)
mrstew is offline   Reply With Quote

Old   August 19, 2019, 07:47
Default
  #3
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 2,551
Rep Power: 35
flotus1 will become famous soon enoughflotus1 will become famous soon enough
What's the result of checking the mesh? Any high volume jumps, bad surface quality, negative volumes...
The boundary layer mesh seems odd. First thing I would try is getting the layer thickness of the last cell in the boundary layer to be of similar size as the first cell in the core mesh. Otherwise it defeats the purpose of a prism layer near the surface. And maybe the meshing algorithm struggles with such a thick boundary layer mesh.
__________________
Please do not send me CFD-related questions via PM
flotus1 is offline   Reply With Quote

Old   August 19, 2019, 11:30
Default
  #4
New Member
 
James
Join Date: Jul 2019
Posts: 5
Rep Power: 3
mrstew is on a distinguished road
Quote:
Originally Posted by flotus1 View Post
What's the result of checking the mesh? Any high volume jumps, bad surface quality, negative volumes...
The boundary layer mesh seems odd. First thing I would try is getting the layer thickness of the last cell in the boundary layer to be of similar size as the first cell in the core mesh. Otherwise it defeats the purpose of a prism layer near the surface. And maybe the meshing algorithm struggles with such a thick boundary layer mesh.
Hi Flotus, thanks for your response,

How would I go about checking the volume mesh? If the plane section view of the mesh is anything to go by, I'd expect a mesh analysis to highlight at least a few dodgy cells so that sounds useful.

Regarding the sizing of the boundary layer, I thought 5mm absolute would be a safe cover-all size, but perhaps not. I've reduced the thickness to 4mm with a thickness ratio of 1.15 reduced from 1.18, this should shrink the larger exterior cells so they're closer in size to the volume mesh cells and I'll adjust it further if this change doesn't fix it.

Would you suggest a different size for the boundary layer, given the dimensions of the wing and the flow characteristics (20m/s, turbulent, AoA 4deg)?

Cheers,
J
mrstew is offline   Reply With Quote

Old   August 19, 2019, 11:49
Default
  #5
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 2,551
Rep Power: 35
flotus1 will become famous soon enoughflotus1 will become famous soon enough
A quick mesh->statistics should give you a first overview of some cell quality criteria.

Based on your images and the spanwise dimension of 20mm (I don't know the wing thickness), I would suggest starting with 1mm total thickness, 10 layers, expansion ration 1.1-1.2. The last layer should ideally be about the same size as the first non-prism layer cell.
__________________
Please do not send me CFD-related questions via PM
flotus1 is offline   Reply With Quote

Old   August 19, 2019, 12:26
Default
  #6
New Member
 
James
Join Date: Jul 2019
Posts: 5
Rep Power: 3
mrstew is on a distinguished road
I'm just waiting for the re-mesh to complete then I'll try and analyze it as suggested.

Regarding the wing dimensions, the maximum thickness is 15mm, the chord is 150mm and the span is 200mm (with a repeating boundary).
mrstew is offline   Reply With Quote

Old   August 20, 2019, 14:32
Default
  #7
New Member
 
James
Join Date: Jul 2019
Posts: 5
Rep Power: 3
mrstew is on a distinguished road
Flotus,

I've implemented the changes you suggested, I ended up using a boundary layer of 1mm, 10 layers and a thickness ratio of 1.5, which results in the outer-most cell layer being of roughly the same size as the volume cells.

I ran the Mesh->Diagnostics and there are no negative volume cells in either mesh, 100% of surface cells are at a quality of 1.0 and 99% of volume cells have a volume change between e-1 and e-0, with the remaining cells being between e-2 and e-1.

The Y+ is also around 1 on both simulations, after testing a few time steps. I'll re-run these from scratch though, as the mesh now has half as many cells thanks to the smaller prism layer so should be very quick.

Another question, if you're happy to help further;

Is the courant number of vital importance in an implicit unsteady simulation such as this? I know that both Y+ and CFL/Courant are vital for explicit simulations, but I'm not sure where they stand with regard to implicit schemes.

Cheers,
J

Last edited by mrstew; August 20, 2019 at 14:37. Reason: Added note regarding mesh diagnostic
mrstew is offline   Reply With Quote

Reply

Tags
convergence, drag, lift, turbulence, wing

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
How to Run Unsteady Simulation in Star CCM+? Andi_Didi STAR-CCM+ 4 November 13, 2017 01:41
Error while importing Solid Works Model into Star CCM Sandy7 STAR-CCM+ 3 December 19, 2016 11:21
Star ccm 9.02 - unsteady flux dissipation correction fivos STAR-CCM+ 4 April 28, 2014 09:37
How can i animate an unsteady simulation in Star ccm eleazar STAR-CCM+ 1 July 7, 2011 08:30
About the difference between steady and unsteady problems Lisa Main CFD Forum 11 July 5, 2000 14:37


All times are GMT -4. The time now is 13:51.