
[Sponsors] 
Cfx initial time choice for adaptive timestep 

LinkBack  Thread Tools  Search this Thread  Display Modes 
April 17, 2021, 07:48 
Cfx initial time choice for adaptive timestep

#1 
Member
Join Date: Mar 2016
Posts: 32
Rep Power: 10 
Hello Glenn, I’m PhD Student Naval Architect Mustafa from Istanbul/TURKEY. I have been using cfx for 10 years for calculating ressistance and self propulsion of our ship designs.
I read nearly all the posts of you about adaptive timestep abilities of CFX. Now I m working in SVA Potsdam’s VP 1302 propeller’s 2015 year cavitation tunnel test experiment validation on cfx. What I did is, 1) start the analysis with 6 million mesh with one phase (only water) with steady state till to the converge. 2) skip the steady state multiphase cavitation analysis (your suggestion) 3) then continue to the analysis With transient (35 loop with 1e4 rms) adaptive timestep to the multiphase cavitation analysis. ITTC (International Towing Tank Test Comitee)‘s recommendation for the propulsion tests on cfd, turn the propeller between 0,52 degree per timestep. When I start to the analysis I start with 40 degrees per timestep then this timestep decreases with 0,8. after 20 iteration turning speed decreases to 0,2 degrees from 40 degrees. Then 120 130 140 iteration still the program could not reach the converge. I think my problem is choosing the optimum initial timestep between max and min wall timesteps. What is the importance of initial timestep in the adaptive transient time step ? What is your recommendation for choosing initial timestep in the adaptive transient calculations. Last 2 questions 1) what is the function of transient rotor stator in the solution part(not in the pre side) of cfx 2) when I pull the cfx steady groups solution to the duplicated transient group side with wire ( steady solution to transient solution) in the main workbench table for continuening the analysis with transient, in the solver menu the initial step was locked. Only I can choose default current solution (if possible) or initial solution. Which one do you suggest for choosing for continuing the transient step ? May be both selections can be same for the results. Best. Mustafa. 

April 18, 2021, 01:19 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 
If you want an accurate time history then you need to choose an initial time step size which converges well. If it is too large then the initial results will be wrong.
If all you want is the final psuedostaeady state result then it can be OK as long as it later converges well. But if the initial time steps are so bad that it causes instability in later time steps then you need to make it smaller. It is generally a good idea to start with an adaptive time step size which is way too small and let adaptive time stepping increase it, rather than too big. If the time step is too small your simulation will still be converged and accurate, just taking a little while longer. If the initial time steps are too big the entire simulation can be destroyed. Other questions: 1) TRS is the interface at a GGI. It means the solver will move the domains and match up nodes at the interface every time step. 2) This sounds like Workbench. As you have found, I think workbench makes using CFX more complicated and it can be hard to make it do what you want it to do. If you use CFX stand alone you have much more control over these things. (In fact, I frequently use workbench to do the geometry, meshing and initial setup of my CFX simulations, but I then take it out of workbench and use it stand alone for debugging and the actual simulation. I have much more control over it that way.)
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

April 18, 2021, 01:46 

#3 
Member
Join Date: Mar 2016
Posts: 32
Rep Power: 10 
Thanks so much Glenn,
It’s no problem cavitation converging problem in the steady state side for me. But when I compare the results with experiments thrust coefficient results of the propeller are ok but the cavitation patterns are not same as with experiment. Because of the complexity of multiphase cavitation I Choosed transient solution for cavitation with your recommendations in the forum. My question is, 1) If I continue with transient cavitation analysis, What is the difference between starting from steady state “cavitation single phase or non cavitation single phase analysis” ? What is your recommendation for this ? 2) after I solve this problem I will use adaptive timestep single phase self propulsion ship calculations. First start with steady resistance analysis then continue with adaptive transient. My concern is here will the adaptive analysis Continue long time ? Because in self propulsion not only propeller but also ships hull and appendages. So I have to converge resistances of all those parameters in the transient part of the analysis. Last thing may you remembered, I’m still continue in to the steady state rigid body free surface flow with 16.2 version. But the other non rigid body analysis are continuing with 21 version. I haven’t solved the movement problem of the meshes after the 16.2 version of Ansys’s. For free surface ship resistance continue with 16.2 

April 18, 2021, 06:43 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 
Cavitation simulations are very difficult to get to converge in terms of residuals, so you should expect difficulties there. The documentation has some comments on convergence and the residuals for cavitation models, I trust you have read them.
For most simulations, if all you are interested in is the pseudosteady state results then what happens in the early time steps does not matter, providing they converge to the correct solution. But for a reasonable amount of simulations you can end up with different final conditions depending on what the initial/early state is  these simulations are especially challenging. For your full ship model, yes I would still use adaptive time stepping to find the time step size of your full ship model. It is the approach to use in most transient simulations, unless you have a very good reason not to.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

April 19, 2021, 12:10 

#5 
Member
Join Date: Mar 2016
Posts: 32
Rep Power: 10 
For The propeller transient cavitation and nominal wake analysis side, initial timestep for the adaptive is very important. I tried both starting with the large time step (for instance 40 degree per time step) and small time step (for instance 1 degree per time step) both analysis could not converged well. Now I’m trying a mid size initial time step (for instance decreasing from 810 degrees per time step). I will share the results with you Glenn.


April 19, 2021, 18:16 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 
I would go smaller than 1 degree time step to start with, not bigger. Try 0.0001 so you can get the first time step converged, and let adaptive time stepping increase it from there.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

April 21, 2021, 09:30 

#7 
Member
Join Date: Mar 2016
Posts: 32
Rep Power: 10 
Glenn what do you think about increasing number of coefficient for the cavitation analysis. You always suggest 35 loops for most transient cases. Normally ı an using that strategy. For example for the single phase analysis I perfect.But also you said we can try 610 loop inner iteration for the “tricky multiphase cases”. What do you think about number of inner iteration’s role in cavitation analysis ? Thanks so much *♂️


April 22, 2021, 19:05 

#8 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 
A cavitation model could be a case where 610 coeff loops per time step might be required. Give it a try and see if it works better than 35. Note that it will result in larger timesteps, but the solver will have more loops to get everything properly coupled. So it is not obvious whether it will help or not, so just try it and find out.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
chtMultiRegionSimpleFoam: maximum number of iterations excedeed.  Nkl  OpenFOAM Running, Solving & CFD  19  October 10, 2019 02:42 
Floating point exception error  lpz_michele  OpenFOAM Running, Solving & CFD  53  October 19, 2015 02:50 
SLTS+rhoPisoFoam: what is rDeltaT???  nileshjrane  OpenFOAM Running, Solving & CFD  4  February 25, 2013 04:13 
pisoFoam with kepsilon turb blows up  Some questions  Heroic  OpenFOAM Running, Solving & CFD  26  December 17, 2012 03:34 
IcoFoam parallel woes  msrinath80  OpenFOAM Running, Solving & CFD  9  July 22, 2007 02:58 