[ALBATTROSS]

Hello everyone,

I reached a steady solution in a transient simulation then I want to run another transient simulation using the steady state solution achieved in previous simulation as the initial condition for the whole domain. The geometry doesn’t changes. How can I do that?
I searched the fluent documentation, however I couldn’t find a way to patch the previous solution to the new case.

Thank you

[LuckyTran]

More info please! Same geometry doesn't tell us anything about what is the same and what is not.

Is it the same .cas file and you just change boundary conditions or what is this "new case"? Do you have a new mesh or no?

If it starts from the same .cas file then you don't need to do anything. If you have a new mesh then you export the the solution data by writing an interpolate file. Then you can import this interpolate file onto the new case.

[ALBATTROSS]

Originally Posted by LuckyTran

More info please! Same geometry doesn't tell us anything about what is the same and what is not.

Is it the same .cas file and you just change boundary conditions or what is this "new case"? Do you have a new mesh or no?

If it starts from the same .cas file then you don't need to do anything. If you have a new mesh then you export the the solution data by writing an interpolate file. Then you can import this interpolate file onto the new case.

Hi,

Yes the mesh structure and size is also the same, I will only change the boundry conditions and by new case I mean new .cas file starting from flow time = 0, In my existing.cas file when I initialize the case the solution will be erased so it’s interesting to know how to initialize a solution as initial condition in same .cas file too.
So it doesn’t have anything to do with patch?

[MKuhn]

From the previous solution. Just change the boundary conditions, and set flow-time and time-step to zero by typing to the command line (with brackets):

(rpsetvar 'flow-time 0)
(rpsetvar 'time-step 0)

Then save *.cas and *.dat with a new name.

It has nothing to do with patch under the solution initialization panel. With patch you write a constat value of a certain propertie to the cells of the selected domain.

[LuckyTran]

Originally Posted by ALBATTROSS

In my existing.cas file when I initialize the case the solution will be erased so it’s interesting to know how to initialize a solution as initial condition in same .cas file too.

Just don't initialize it and it will keep the current solution. Do not press the initialize button! You literally have to do nothing.


And then you can use the rpsetvar mentioned to reset the flow-time to 0 or whatever.

[ALBATTROSS]

Originally Posted by MKuhn

From the previous solution. Just change the boundary conditions, and set flow-time and time-step to zero by typing to the command line (with brackets):

(rpsetvar 'flow-time 0)
(rpsetvar 'time-step 0)

Then save *.cas and *.dat with a new name.

It has nothing to do with patch under the solution initialization panel. With patch you write a constat value of a certain propertie to the cells of the selected domain.

Thank you Mortiz! It helped a lot.

[AidealZohary]

Hello LuckyTran,

Since we are initializing a transient simulation with the steady state simulation earlier, from your experience how do you think this will affect the final results? I'm simulating an airfoil at Re 1million using k omega SST intermittency and notice that with different initialization values from the steady state simulation will give different lift and drag values in after running transient.

Eg: case A, initialized using steady state simulation after 300 iterations and case B, after 200 iterations.

In the transient setup, i monitor the lift, drag and max courant value in the system. Used adaptive with incremental time steps. 20 iterations per time step and timestep interval updated after 20 iterations. I stop reducing the time step once the courant monitor shows a value ~0.9. Then let it run until lift and drag give negligible change.

Please shed some light.

[smo8812]

Originally Posted by AidealZohary

Hello LuckyTran,

Since we are initializing a transient simulation with the steady state simulation earlier, from your experience how do you think this will affect the final results? I'm simulating an airfoil at Re 1million using k omega SST intermittency and notice that with different initialization values from the steady state simulation will give different lift and drag values in after running transient.

Eg: case A, initialized using steady state simulation after 300 iterations and case B, after 200 iterations.

In the transient setup, i monitor the lift, drag and max courant value in the system. Used adaptive with incremental time steps. 20 iterations per time step and timestep interval updated after 20 iterations. I stop reducing the time step once the courant monitor shows a value ~0.9. Then let it run until lift and drag give negligible change.

Please shed some light.

Hello AidealZohary,


I am dealing with something similar or equal to what you mentioned in your comment.
Did you find a good criteria or something to initialize your transient simulation?


Thanks in advance.

[Yasser]

Originally Posted by smo8812

Hello AidealZohary,


I am dealing with something similar or equal to what you mentioned in your comment.
Did you find a good criteria or something to initialize your transient simulation?


Thanks in advance.

If you have a steady solution, you don't need to initialize. Just change the solver to transient and your calculated values from steady solution is already there.

[AidealZohary]

Hi smo8812,

Yasser is correct, just change the turbulence model. Additionally here is how I approached the remaining portion of the problem in case you're interested. Also, I actually don't need the CFL number since this is an implicit case.


1. Run steady-state until your residuals are stable. In my case where I was using a structured grid via ICEM, it took me around 200 iterations.

(You don't need the residuals to drop like crazy before going to step 2, because once turning on the transition model your residuals will jump back up.)

2. Change your model using the Intermittency/Transition SST but still in steady-state. Continue with another 80 iterations.

(80 is based on my case where the residuals start to act weird at 100. So 80 just to be on the safe side.)

3. Proceed with unsteady simulation and I chose a timestep of 0.001s with 10 inner iterations. Here it is very important to let your simulation converge before using a smaller timestep. (my biggest mistake was changing to a smaller timestep when the current timestep was not properly resolved.) You can monitor your cl and cd, it will drop continuously. Once it is somewhat stable, then use a smaller timestep. It is advised that your timestep should be reduced by half. So it is something like 0.001, 0.0005,0.00025....

4. You can play around with your initial timestep size. It is case-dependent.

Tip: I find it easier to monitor my residuals when Fluent is reporting it according to my inner iterations. You can tweak this in the settings before running your calculations. This will "hide" the zig-zag shape in your monitor.

I am currently waiting for my work on the simulation to be published. Ill post it here in the future if someone wants to look at my results.

[smo8812]

Originally Posted by AidealZohary

Hi smo8812,

Yasser is correct, just change the turbulence model. Additionally here is how I approached the remaining portion of the problem in case you're interested. Also, I actually don't need the CFL number since this is an implicit case.


1. Run steady-state until your residuals are stable. In my case where I was using a structured grid via ICEM, it took me around 200 iterations.

(You don't need the residuals to drop like crazy before going to step 2, because once turning on the transition model your residuals will jump back up.)

2. Change your model using the Intermittency/Transition SST but still in steady-state. Continue with another 80 iterations.

(80 is based on my case where the residuals start to act weird at 100. So 80 just to be on the safe side.)

3. Proceed with unsteady simulation and I chose a timestep of 0.001s with 10 inner iterations. Here it is very important to let your simulation converge before using a smaller timestep. (my biggest mistake was changing to a smaller timestep when the current timestep was not properly resolved.) You can monitor your cl and cd, it will drop continuously. Once it is somewhat stable, then use a smaller timestep. It is advised that your timestep should be reduced by half. So it is something like 0.001, 0.0005,0.00025....

4. You can play around with your initial timestep size. It is case-dependent.

Tip: I find it easier to monitor my residuals when Fluent is reporting it according to my inner iterations. You can tweak this in the settings before running your calculations. This will "hide" the zig-zag shape in your monitor.

I am currently waiting for my work on the simulation to be published. Ill post it here in the future if someone wants to look at my results.

AidealZohary, thanks for taking your time and share what you did with your simulation.


I am working in an aeroacoustics problem. I am simulating a flow over a symmetrical airfoil to get the pressure data to then feed a code to get the sound pressure at some receiver points. My problem is that I initialize the simulation in steady state, but when I turn into transient the variables I am monitoring remain constant and don't exhibit any fluctuation. So in the end I cannot get any sound propagation.


I will follow the steps you mentioned because I am doubtful if my way to initialize with steady state is correct.


It would be nice to see the results of your work.


Thanks again!

[AidealZohary]

Hi smo8812,

Hopefully, the steps will help with cl and cd.

But also another important thing is once you start using time-dependent settings, and want to get the actual data, don't forget to store your data every "N" number of iterations that you may need for post-processing your pressure fluctuations.

That is maybe the reason why you're getting only constant readings. I am not familiar with aeroacoustics and maybe someone else can help.

__________________________________________________ ____________________________________________
Numerical Investigation on the Pressure Drag of Some Low-Speed Airfoils for UAV Application
https://doi.org/10.37934/cfdl.13.2.2948

Unsteady 2D simulation of the NACA 0012, NACA 4415, FX 61-184, E420, and S1223. Manually generated the body-fitted mesh using ICEM and the 3-Equation Intermittency Transitional Model was used. Good overall agreement with XFOIL and published data. Informative paper to understand the relationship between airfoil geometry and the production of pressure drag

[Nima Shah]

Originally Posted by AidealZohary

Hi smo8812,

Yasser is correct, just change the turbulence model. Additionally here is how I approached the remaining portion of the problem in case you're interested. Also, I actually don't need the CFL number since this is an implicit case.


1. Run steady-state until your residuals are stable. In my case where I was using a structured grid via ICEM, it took me around 200 iterations.

(You don't need the residuals to drop like crazy before going to step 2, because once turning on the transition model your residuals will jump back up.)

2. Change your model using the Intermittency/Transition SST but still in steady-state. Continue with another 80 iterations.

(80 is based on my case where the residuals start to act weird at 100. So 80 just to be on the safe side.)

3. Proceed with unsteady simulation and I chose a timestep of 0.001s with 10 inner iterations. Here it is very important to let your simulation converge before using a smaller timestep. (my biggest mistake was changing to a smaller timestep when the current timestep was not properly resolved.) You can monitor your cl and cd, it will drop continuously. Once it is somewhat stable, then use a smaller timestep. It is advised that your timestep should be reduced by half. So it is something like 0.001, 0.0005,0.00025....

4. You can play around with your initial timestep size. It is case-dependent.

Tip: I find it easier to monitor my residuals when Fluent is reporting it according to my inner iterations. You can tweak this in the settings before running your calculations. This will "hide" the zig-zag shape in your monitor.

I am currently waiting for my work on the simulation to be published. Ill post it here in the future if someone wants to look at my results.

Hi AidealZohary,
I have a question regarding the continuation from steady state to transient. I have a CLSVOF simulation with the steady state and some report files have been generated.
The RMS for mass conservation is stable but is in the order of 1e-2. Can i continue from that point on with just changing the model to transient and not initializing?
I have faced the error : SIGSEV on one of the nodes. (attached below FL_2Lit Paralle...)
Is it because of the mass conservation, timestep size which is 0.0001 or the autosave options?
I wonder if you can let me know how I can proceed with same setup but just changing the model from ss to transient and the settings for autosave.
Regards

[AidealZohary]

Hi Nima,

Can you please describe your problem? I see that you have reversed flow at the outlet

[Nima Shah]

Originally Posted by AidealZohary

Hi Nima,

Can you please describe your problem? I see that you have reversed flow at the outlet

That is a venturi tube with an inlet from air directly to the neck.
The initial conditions for inlet_air is pressure inlet = 0 (atmospheric)
Inlet water velocity inlet resulting in some specific lit/min and in turbulent k-eps realizable.
The implicit body forces is activated and the VOF combined with level set. The reverse flow is not that much important I guess, the main concern is how I need to initialize?
Currently I initialize from all zones patching the air vf to be zero at fluid domain. I have tried other sources such as from inlet air or water inlet though they are not close to the real problem.
Water flows at high speed and sucks the air.
The mesh is also attached.
steady setup was 10000 iterations and unsteady should be finally, 0.0001 timestep size for about 1500 total timesteps
Regards

[MAHESH9966]

Hi Everyone,


I am working on Electric motor ( Permanent Magnet Synchronized motor ) conjugate heat transfer analysis. Currently i am simulating the steady state simulation and completed around 8000 iterations using the SIMPLEC method.


Now i want to move ahead with Transient-simulation with different loss densities for coils and magnets. My problem is can i change the source terms of coils & Magnets in the same steady state simulation setup along with changing the steady state option to transient???


Do i need to re-initialize the system to continue with transient simulation???


I searched the fluent tutorial guide but i couldn't figure out any command or procedure. It will be very very helpful if anyone give me some suggestions. Hoping for positive answers soon

[AlexanderZ]

it is good practice to use steady state simulation results to initialize transient simulation
so you don't need to reinitialize case to run transient

[MAHESH9966]

Originally Posted by AlexanderZ

it is good practice to use steady state simulation results to initialize transient simulation
so you don't need to reinitialize case to run transient

Thank you so much for your kind reply.


Actually which part i want to clarify is, In my case motor is running at low rpm with certain losses and then running at peak power. so initially i want to run with low rpm case losses so that motor got stabilized after that i want to continue with the same simulation for peak power losses in transient case. Could you please help me how to change the source terms of coil & magnets and continue with transient simulation.


once again thank you for your reply