# Transient Simulation Taking Very Long TIME!!!! Help

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

 March 7, 2011, 09:19 Transient Simulation Taking Very Long TIME!!!! Help #1 New Member   phil fenna Join Date: Feb 2011 Posts: 14 Rep Power: 9 I'm running a transient simulation of my water tank, the mesh has 500,000 elements, the tank should take about 3000 seconds to fill up but when i specify an interval of 10s it takes almost 2 days to run! Is this normal? or is there a way to increase the speed of simulations? Also when running intervals of 10s my RMS Courant number is about 150 which is way too high, is this down to my interval of being to high at 10s? Is there a way to calculate a good time interval? Any help will be greatly appreciated! Thanks Phil

 March 7, 2011, 11:48 #2 Senior Member   Join Date: Apr 2009 Posts: 532 Rep Power: 14 That sounds normal. Run in parallel to speed things up. Why do you say a Courant number of 150 is too high? That sounds OK for this type of simulation, as long as it's converging OK.

 March 7, 2011, 12:04 #3 Senior Member     Attesz Join Date: Mar 2009 Location: Munich Posts: 367 Rep Power: 10 2day run for a transient is short If you want to have RMS Courrant number 5, use adaptive time step with RMS Courrant number option, and set the minimal and maximal timestep value what you can allow. But with a lower timestep, it will take more than 2 days of course. It depends on what you want to do.

 March 7, 2011, 13:16 #4 New Member   phil fenna Join Date: Feb 2011 Posts: 14 Rep Power: 9 Thank you for the prompt responses! I read on the forum that the lower the RMS number the higher the accuracy of the transient simulation, is this right? I've lowered my time step interval to every second and I'm now running in parallel and its sped up things a lot! But i have set the time step interval down to every second so it will take longer but the RMS number is about 5 . its a multiphase simulation with air, water and a solid. I want to see how solids settle in my water tank so the quicker it runs the better but eventually i want a good animation of the whole process but i dont need that for a while. So can i ignore the RMS number and let it be around 200 and have large time step intervals? or should i keep it down to 1s intervals? Thanks

 March 7, 2011, 16:15 #5 Senior Member   Ugly Kid Joe Join Date: Aug 2010 Posts: 193 Rep Power: 9 1.) Lower the Courant number, greater the accuracy. 2.) I think a Courant # of 150 is high. 3.) Adaptive time stepping is the best thing to do. If the simulation is lengthy, adaptive time stepping can save a lot of time.

 March 7, 2011, 18:26 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,313 Rep Power: 110 Courant number is not really a good way of looking at an implicit solver. It does not tell you much. To comment on Prof Chaos' comments: Yes, lowing timestep will increase accuracy but it asymptotes out. Your job is to find the optimum between simulation time and the accuracy you need. Whether this Courant number is too high depends on the simulation. For some simulations it is far too high (eg free surface with surface tension needs very small timesteps) but for others it would be fine (eg marching a simulation out to steady state). You need to do a sensitivity analysis to determine whether it is too big or small. General comments like "Courant Number = 150 is too high" are wrong. Your final comment about adaptive timestepping is exactly correct. Then the simulation can find the timestep it needs, and adapt it as it progresses.

 March 8, 2011, 05:26 #7 New Member   phil fenna Join Date: Feb 2011 Posts: 14 Rep Power: 9 Thank you everyone for you everyone for your replies, my simulation is now running quicker and should take less time. I'm using adaptive time stepping initially at 1s as the minimum and the RMS courant number set at 8, over time as the volume of water increases in my tank so does the time steps. My simulation is using free surface and water tension so i think the best way to run the simulation is to use adaptive time stepping and let the simulation decide on the intervals! Again thank you for your help

 March 8, 2011, 18:00 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,313 Rep Power: 110 Adaptive time stepping on Courant number is not very helpful, unless you have shown the Courant Number you selected is relevant to your flow. In general the best approach is to use adaptive time stepping aiming for 3-5 coeff loops per time step.

 March 9, 2011, 05:56 #9 New Member   phil fenna Join Date: Feb 2011 Posts: 14 Rep Power: 9 Ok thanks, i'll give that a try. I'm modelling a water tank with fluid and solids in and i only really want to see the settlement of the solids in the water tank, am i wrong using transient simulation for this? i know it will give show the solids settling but will steady state be able to show the solids settling over time?

 March 9, 2011, 08:20 #10 Senior Member     Attesz Join Date: Mar 2009 Location: Munich Posts: 367 Rep Power: 10 i think you should run transient simulation if you want to investigate solid motion, because steady would show the completely settled state.

 March 9, 2011, 13:49 #11 New Member   phil fenna Join Date: Feb 2011 Posts: 14 Rep Power: 9 ghorrocks just ot clarify when setting up adaptive timesteps for number of coeff loops. does this set up seem ok? in Analysis type Timesteps option - adaptive first update time - 1s update frequency - 1 initial timestep -1s timestep adoption option - num. coeff. loops min timestep - 1s max timestep - 200s target min loops - 3 target max loops - 5 timestep decrease factor - 0.8 timestep increase factor - 1.06 Do i need to change anything in the solver control i've left it as default settings thanks

 March 9, 2011, 19:43 #12 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,313 Rep Power: 110 Looks good. The only point is the first update time and max and min timesteps. Make sure these are wide enough so you do not hit the limits in the normal course of events.

 March 9, 2011, 20:12 #13 New Member   phil fenna Join Date: Feb 2011 Posts: 14 Rep Power: 9 So if im not sure what they should be would it be best to initially set the minimum time step to a very small number and very large for maximum timestep? Thanks

 March 10, 2011, 07:19 #14 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,313 Rep Power: 110 Why not start off with minimum 1e-20 and maximum 1e20? Then let it find what ever time step works. If it starts getting silly you should stop it and fix the problem (in this case the problem is unlikely to be in the time step size but elsewhere).

 November 2, 2017, 09:53 adaptive timestep taking too small time steps #15 New Member   jayotpaul chaudhuri Join Date: Jun 2016 Location: Dortmund Posts: 8 Rep Power: 3 Dear community, I have a similar problem. I have a bit of a complex 3 phase system with air, free oil droplets and captured oil droplets where oil is captured in a porous media. I have a converged steady state solution and want to investigate the transient behaviour. As GHORROCKS said, i am also using adaptive with covergence control (1-10 internal loops). Now the problem is using adaptive time steps CFX is decreasing the timestep to around 1e-8/9 whereas my process timescale is in minutes. So even running on 32 cores for 3 days , doesnt really help me. I am afraid to increase mesh size, because that woul increase the time required for each time step i am guessing. Correct me if i am wrong! Any ideas what can be done to fasten it up is appreciated.

 November 2, 2017, 17:43 #16 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,313 Rep Power: 110 Here is some ideas: * Get more parallel licenses * Look at the simulation and work out why somewhere is having problems converging. * Improve mesh quality. Better mesh = better convergence = faster simulation * Double precision numerics * Do a mesh size sensitivity study to determine the mesh you really need

November 3, 2017, 04:27
#17
New Member

jayotpaul chaudhuri
Join Date: Jun 2016
Location: Dortmund
Posts: 8
Rep Power: 3
Quote:
 Originally Posted by ghorrocks Here is some ideas:
2. Look at the simulation and work out why somewhere is having problems converging- I know which area is giving problem (end of porous media, where absorbed oil is draining), i also think i should refine in this area, was just worried if aspect ratio change will give more trouble. i have a simple structured mesh (rectangular block of porous media), if i refine locally, aspect ratio gets bad.
3. Improve mesh quality. Better mesh = better convergence = faster simulation
5. Do a mesh size sensitivity study to determine the mesh you really need-
I have a Q, wheather i can do a mesh study on steady state and use same results for transient. Couldnt find any information on this.

November 3, 2017, 05:07
#18
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 14,313
Rep Power: 110
Quote:
 I know which area is giving problem (end of porous media, where absorbed oil is draining), i also think i should refine in this area, was just worried if aspect ratio change will give more trouble. i have a simple structured mesh (rectangular block of porous media), if i refine locally, aspect ratio gets bad.
Also have a look at the porous media expert parameters and detailed settings. There are some alternate solver options which may converge better.

Also note finer meshes tend to be hard to converge, not easier (as finer meshes have less dissipation). So refining the mesh is going to make convergence harder. You should determine the mesh size you need from a mesh sensitivity study and use that so you get the accuracy you require.

Quote:
 wheather i can do a mesh study on steady state and use same results for transient
In general yes. As long as the physics is equivalent between the two it will be valid.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post irishdave OpenFOAM Running, Solving & CFD 31 January 25, 2018 04:03 Travis FLUENT 4 January 15, 2009 12:48 Richard CFX 0 October 10, 2008 09:50 CP CFX 1 November 12, 2007 17:22 Anurag CFX 2 March 28, 2005 12:09

All times are GMT -4. The time now is 20:43.