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

Transient Convergence

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

Like Tree1Likes
  • 1 Post By lingdeer

Reply
 
LinkBack Thread Tools Display Modes
Old   November 20, 2011, 14:50
Default Transient Convergence
  #1
Member
 
Elaine
Join Date: Jul 2011
Posts: 47
Rep Power: 5
lingdeer is on a distinguished road
Hi,

I am running 2 way FSI of blood vessel, with a tetrahedron mesh with 2XXXX elements and solid surface body of 7XXX elements. My waveform is a pulsatile sinusoidal flow waveforms.

I ran already 10 cycles to ignore the effect of the initial condition. However, when I monitor the velocity and mesh displacement, there is some cycle-to-cycle variation even at the later cycles (8,9,10th) cycles.

I wonder if I should run even more cycles to ensure my solutions are correct? Or should I refine the mesh if it is too coarse? The geometry is pretty cylindrical so I would assume I don't need a very fine mesh.

Thanks in advance!
zengqiang2006 likes this.
lingdeer is offline   Reply With Quote

Old   November 20, 2011, 17:48
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,758
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This sounds like exactly the sort of thing you need to do sensitivity analysis for. Run to 20 cycles and see if it has converged to an accuracy you are happy with. Likewise you should also do a mesh refinement study to ensure the mesh is adequate.

So you should run an analysis on both settling time and mesh sensitivity. Whil you are at it I would also do it on convergence tolerance, time step size and any other physics you are converging on.
ghorrocks is offline   Reply With Quote

Old   November 28, 2011, 15:58
Default
  #3
Member
 
Elaine
Join Date: Jul 2011
Posts: 47
Rep Power: 5
lingdeer is on a distinguished road
Thanks ghorrocks.

I think the reason why the convergence it bad is because the coupling data transfer convergence is not tight enough.

My geometry is a symmetric pipe and I monitored mesh displacement at two points at symmetric positions. When I used the coupling data transfer convergence target of 0.01, the two symmetric monitor positions give different results.

In my previous simulations:
CFX convergence criteria: RMS 1e-4
Mesh displacement convergence : 1e-4 (min 1 iteration, max 30 iterations)
Coupling data transfer: 1e-2

I ran up to 30 cycles but transient convergence was bad and like I said the two symmetric monitor points are not equal.

In the new simulations, I ran:
CFX convergence criteria: RMS 1e-5 (From rigid simulation I figure this is needed)
Inner CFX coefficient loop (min: 1, max: 3)
Mesh displacement convergence : 1e-4 (min 1 iteration, max 30 iterations)
Coupling data transfer: 1e-4
max no. of coupling iterations: 500

The results are good for now (for 1/4 of total timesteps), as the two monitor points are equal and consistent. However the simulations take really long time to run.
There is no underrelaxation but I did add a source term.

Solid mesh elements: 7XXX
Fluid mesh elements: 1XXXXX


I wonder anyone has experience in simulating blood vessel and what coupling solver setup do you use for satisfactory results?
Right now I am running those cases (changing different parameters that ghorrocks mentioned, but computer resources are limited and I want to have the results asap)
Thanks!
lingdeer is offline   Reply With Quote

Old   November 28, 2011, 17:49
Default
  #4
Senior Member
 
Join Date: Apr 2009
Posts: 503
Rep Power: 11
stumpy is on a distinguished road
When you say you are using a source term I assume you mean that zero mass source with a coefficient set for stability. What do your displacement/force monitor points look like *within* a timestep? If your continuity source coefficient is too big then you'll be damping the solution a lot, which means a lot of iterations would be needed to get convergence. If your monitor points are not showing a critically damped response within a timestep then reduce that coefficient.
stumpy is offline   Reply With Quote

Old   November 28, 2011, 18:04
Default
  #5
Member
 
Elaine
Join Date: Jul 2011
Posts: 47
Rep Power: 5
lingdeer is on a distinguished road
Thanks for your reply.
I used a value of mass flux pressure coefficient of 300. If I used lower values (e.g. 100, 200), the solid solution tends to diverge and crash within a few time steps.
lingdeer is offline   Reply With Quote

Old   November 29, 2011, 11:06
Default
  #6
Senior Member
 
Join Date: Apr 2009
Posts: 503
Rep Power: 11
stumpy is on a distinguished road
Are you starting the transient solution with a zero relative pressure field in the fluid and zero relative pressure at the boundary conditions? If not, you can expect a start-up bump that would probably cause failure. If you have a non-zero initial relative pressure field, then you would need a steady-state 2-way FSI case to initialize the transient solution.
stumpy is offline   Reply With Quote

Old   November 29, 2011, 11:33
Default
  #7
Member
 
Elaine
Join Date: Jul 2011
Posts: 47
Rep Power: 5
lingdeer is on a distinguished road
Yes I started with the steady results as initial conditions
lingdeer is offline   Reply With Quote

Old   November 29, 2011, 14:35
Default
  #8
Senior Member
 
Join Date: Apr 2009
Posts: 503
Rep Power: 11
stumpy is on a distinguished road
Steady FSI or just steady fluid results?
stumpy is offline   Reply With Quote

Old   November 29, 2011, 14:38
Default
  #9
Member
 
Elaine
Join Date: Jul 2011
Posts: 47
Rep Power: 5
lingdeer is on a distinguished road
Steady FSI results (both ANSYS.db and .res) of the steady run
lingdeer is offline   Reply With Quote

Old   November 30, 2011, 16:37
Default
  #10
Senior Member
 
Join Date: Apr 2009
Posts: 503
Rep Power: 11
stumpy is on a distinguished road
Hmm, not sure why you need to converge so much. This is 13.0 right?
stumpy is offline   Reply With Quote

Old   November 30, 2011, 17:10
Default
  #11
Member
 
Elaine
Join Date: Jul 2011
Posts: 47
Rep Power: 5
lingdeer is on a distinguished road
Because the cycle to cycle variation of mesh displacement is big
(attached)

Each of my cycle has 100 timesteps so here are 10 cycles.
The blue and green lines are supposed to be symmetric.
And the red line is the force on the FSI interface.


Also attached to the outlet monitor points (30 cycles). I used static pressure = 0 Pa as Neumann boundary conditions at the outlet. And again, the transient convergence is not satisfactory and I don't know which cycle I should process since they are not repeating and fluctuating a lot.

lingdeer is offline   Reply With Quote

Old   November 30, 2011, 17:10
Default
  #12
Member
 
Elaine
Join Date: Jul 2011
Posts: 47
Rep Power: 5
lingdeer is on a distinguished road
And yes it's ANSYS 13
lingdeer is offline   Reply With Quote

Old   December 1, 2011, 18:22
Default
  #13
Senior Member
 
Join Date: Apr 2009
Posts: 503
Rep Power: 11
stumpy is on a distinguished road
Could you zoom in and show those plots over just a few timesteps? It's important to check that the quantities are converging within each timestep.
stumpy is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Convergence Centurion2011 FLUENT 21 November 18, 2014 05:17
Force can not converge colopolo CFX 13 October 4, 2011 23:03
Transient axial rotor/stator convergence issue? Nicola Viscanti CFX 3 March 17, 2010 06:15
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 02:17
Poor Convergence for Transient Subsonic Diffuser sims with flow separation TWaung CFX 1 April 16, 2009 09:25


All times are GMT -4. The time now is 09:44.