Transient Simulation Taking Very Long TIME!!!! Help
 

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

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.

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.

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

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.

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.

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

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.

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?

i think you should run transient simulation if you want to investigate solid motion, because steady would show the completely settled state.

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

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.

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

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).

adaptive timestep taking too small time steps
 

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 :eek:, 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!:confused:
Any ideas what can be done to fasten it up is appreciated.

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

Thanks For your suggestions
1.Get more parallel licenses- ;)
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
4.Double precision numerics- Already done
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.

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.

In general yes. As long as the physics is equivalent between the two it will be valid.