|
[Sponsors] |
Chance in time step size is causing instabilities? |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Niklas
Join Date: Jun 2016
Posts: 17
Rep Power: 10 ![]() |
Hello everybody,
I'm currently simulating a transient Problem with a moving mesh. Itīs a Cylinder and its top surface is moving downwards. I ran in a bit of trouble when I did a mesh refinement. My convergence limit is Max 1e-6 with a maximum 50 Coefficient loops, but for the adaptive time stepping I chose a target of 4-6 Coefficient loops. Im starting with an initial tilmestep of 1e-8 s. I got 2 questions: 1) It takes about 100 time steps before the Residuals reach 1e-6. Do I have to worry about this? Should it happen faster? 2) My main concern: As soon as I reach 1e-6, the number of coefficient loops drops and CFX is increasing the timestep size. When this happens, the mean pressure starts to fluctuate (Monitor 1), even if the timestep decreases back to the initial stepsize. The small fluctuations might have something to do with the pressure bend factor at the outlet, but at 3 points when the stepsize increases, there are major fluctuations of the pressure, which I need to get rid off. Does anybody has any idea, what is going one here? Thanks a lot! |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,902
Rep Power: 144 ![]() ![]() ![]() ![]() |
If you want a time accurate history you need to get it to converge from the first time step. So start with an even smaller time step.
Your report is a bit strange as defining convergence at MAX=1e-6 is very tight convergence. Most simulations have converged well before this. But the pressure variations you report suggest it is not converged. Can you please post your CCL or output file?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Niklas
Join Date: Jun 2016
Posts: 17
Rep Power: 10 ![]() |
Hey,
thanks for your answer! I'm not really interested in the first few time steps, so I'm not worrying to much about the convergence there. I'm also suprised, since a max residual of 1e-6 is actually pretty good from what I know. I tried to change the timesteps a little and set the min time step higher to 1e-7 s, which made the Simulation much more stable at the beginning. There are still small fluctuations every time the timestep is changing. At the end the time step size is almost at 1e-6s and suddenly the pressure is dropping really fast. I'm gonna provide the ccl file in the next post. It might be worth mentioning, that the Fluid Domain is pretty small (around 1 mm) and the moving mesh is moving relatively fast. |
|
![]() |
![]() |
![]() |
![]() |
#4 |
New Member
Niklas
Join Date: Jun 2016
Posts: 17
Rep Power: 10 ![]() |
CCL File attached
Edit: And I'm using double precision, single precision seems to make even more problems. |
|
![]() |
![]() |
![]() |
![]() |
#5 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,902
Rep Power: 144 ![]() ![]() ![]() ![]() |
There are some cases which require convergence much tighter than normal. Your case might be one of those cases.
Try specifying a tighter convergence criteria and see if that helps. You will probably need to reduce the minimum allowable time step size as well when you do this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#6 |
New Member
Niklas
Join Date: Jun 2016
Posts: 17
Rep Power: 10 ![]() |
Thanks again for your reply. I tried to set the convergence criteria to MAX 1e-8 and the initial and Minimum time step size to 1e-9s. Unfortunatley I still got these fluctuations every time the time step is increasing or decresing. The timestep only increases one or two times and goes back to 1e-9 afterwards. Unfortunatley I'm not able to complete the simulation since it's gonna take way too long.
I'm actually pretty suprised, why CFX is having so much trouble solving this, since it's a pretty simple set up without turbulences and so on ( I even got an analytical solution). When I did the calculation with a mesh which was less fine, I didn't run in those troubles. Do you have any more ideas? Thanks in advance! Best Niklas |
|
![]() |
![]() |
![]() |
![]() |
#7 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,902
Rep Power: 144 ![]() ![]() ![]() ![]() |
Now that you have shown it is not convergence I think the problem is elsewhere. Can you try it again using first order time differencing? You can relax the residual tolerance back to your previous value.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#8 |
New Member
Niklas
Join Date: Jun 2016
Posts: 17
Rep Power: 10 ![]() |
I set the time differencing to first order. And started with a minimal time step of 1e-8. The little fluctuations seem to be within a time step (during the coefficient loops) so we shouldn't worry about them. CFX needed around 7 coefficient loops so it stayed at the minimal time step. After ~600 and ~630 Iterations I decreased the minimal time step to 5e-9 and 1e-9. The fluctuation is due to the decrease of time step. The decrease didn't really support convergence of P-MASS, it still needed 7 coefficient loops, but the other residuals seem to be tighter now.
The behavior seems to be the same. When there is an decrease in time step size, the pressure is fluctuating. Maybe Lowering the Timestep Increase/Decrease Factor could be an option? But it still seems weird to me. |
|
![]() |
![]() |
![]() |
![]() |
#9 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,902
Rep Power: 144 ![]() ![]() ![]() ![]() |
Are your plots showing the results at each iteration, or just the final converged result at each time step?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#10 |
New Member
Niklas
Join Date: Jun 2016
Posts: 17
Rep Power: 10 ![]() |
Sorry, I was busy changing my model a little and didn't have time to reply. While changing I might have found the problem. The Displacement of my mesh is being calculates by an expression. As far as I know, the expression is calculated with single precision. I'm working with Displacements in order of 0 to 1e-3 with a total time of (now) ~ 0.1 seconds and time steps down to 1e-9.
The use of small time steps and the change of the timestep size seems to cause difficulties while calculating the expression for the wall/mesh displacement, since its not accurate enough for my problem. This causes fluctuation of the displacement/mesh velocity due to rounding errors. I feel like it might help to calculate the displacement using milliseconds and millimeters, but I'm not sure how CFX is treating the units internally thus whether it's gonna make a difference. I'm gonna try to change this on Monday. I still would be glad if anybody had some advices. |
|
![]() |
![]() |
![]() |
Thread Tools | Search this Thread |
Display Modes | |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Transient simulation not converging | skabilan | OpenFOAM Running, Solving & CFD | 14 | December 17, 2019 00:12 |
pressure in incompressible solvers e.g. simpleFoam | chrizzl | OpenFOAM Running, Solving & CFD | 13 | March 28, 2017 06:49 |
simpleFoam error - "Floating point exception" | mbcx4jc2 | OpenFOAM Running, Solving & CFD | 12 | August 4, 2015 03:20 |
Problems in compiling paraview in Suse 10.3 platform | chiven | OpenFOAM Installation | 3 | December 1, 2009 08:21 |
Could anybody help me see this error and give help | liugx212 | OpenFOAM Running, Solving & CFD | 3 | January 4, 2006 19:07 |