nodal initial conditions

Prabin Pradhananga_22497

Hi experts,

I want to know more about pre-compute velocity, temperature, etc. that come when lauching acusolve. As far as i know they are nodal  initial conditions. How would they impact the simulations? Where can i find a documentation on these?

Thanks.

acupro

Those pre-compute flow and pre-compute turbulence help to establish something of a realistic field (based on the boundary conditions) prior to starting the first time step.  They 'translate' to intialize_stokes and initialize_turbulence in the TIME_INTEGRATION command of the input file.  They are discussed towards the bottom of this page:

https://2022.help.altair.com/2022.1/hwcfdsolvers/acusolve/topics/acusolve/time_integration_acusolve_com_ref.htm

Prabin Pradhananga_22497

Hi guys,

I want to know more about Default initial conditions: Static pressure and Velocity in the above dialog box. What is the effect when i change these values if I have outlet pressure of 8 MPa?

I found that changing the values in the above dialog box significantly affect the result. I would be grateful if you would explain why.

Thanks!

acupro

Prabin Pradhananga_20428 said:

Hi guys,

I want to know more about Default initial conditions: Static pressure and Velocity in the above dialog box. What is the effect when i change these values if I have outlet pressure of 8 MPa?

I found that changing the values in the above dialog box significantly affect the result. I would be grateful if you would explain why.

Thanks!

I would be interested in seeing the input (.inp) and Log files for the cases where the only thing changed is the initial conditions.  If both cases reach similar levels of convergence, I would expect the solutions to be basically the same also.

Prabin Pradhananga_22497

acupro_21778 said:

I would be interested in seeing the input (.inp) and Log files for the cases where the only thing changed is the initial conditions.  If both cases reach similar levels of convergence, I would expect the solutions to be basically the same also.

These are the ones with 8MPa nodal initial condtion which works fine as expected. The outlet pressure is 8Mpa. This is a simple flow over cylinder problem.

 

Prabin Pradhananga_22497

Prabin Pradhananga_20428 said:

These are the ones with 8MPa nodal initial condtion which works fine as expected. The outlet pressure is 8Mpa. This is a simple flow over cylinder problem.

 

These are the ones with just nodal initial condition pressure changed to 0Mpa. The outlet pressure is 8Mpa in both cases.

acupro

Prabin Pradhananga_20428 said:

These are the ones with just nodal initial condition pressure changed to 0Mpa. The outlet pressure is 8Mpa in both cases.

First - on the nodal initial condition.  The 0 setting creates a very different flowfield at the start.  The high value at the outlet and the low value inside wants to force flow into the domain from the outlet, as shown by all the 'inflow at outflow' warning messages in the Log file, then that will take a long time to 'wash out' - and it may not ever completely wash out.  Depending on what is done with the user-function body force, there may be effects with that also.

Second - on the case with the 8 MPa initial condition - I noticed the dissipation rate equation is not solving anything - all zeroes:

acuSolve: diss.-rate res ratio = 0.000000e+00
acuSolve: GMRES No iterations = 0 (0.00)
acuSolve: GMRES 0/1/n norms = 0.000000e+00 0.000000e+00 0.000000e+00
acuSolve: GMRES Iter. CPU/Elapse = 0.000000e+00 4.410744e-05
acuSolve: diss.-rate sol ratio = 0.000000e+00

You may want to try a different choice for the inlet turbulence type and parameters.  Have you considered the Spallart-Allmaras model instead of standard k-epsilon?  Or even realizable k-epsilon instead of standard?

Prabin Pradhananga_22497

acupro_21778 said:

First - on the nodal initial condition.  The 0 setting creates a very different flowfield at the start.  The high value at the outlet and the low value inside wants to force flow into the domain from the outlet, as shown by all the 'inflow at outflow' warning messages in the Log file, then that will take a long time to 'wash out' - and it may not ever completely wash out.  Depending on what is done with the user-function body force, there may be effects with that also.

Second - on the case with the 8 MPa initial condition - I noticed the dissipation rate equation is not solving anything - all zeroes:

acuSolve: diss.-rate res ratio = 0.000000e+00
acuSolve: GMRES No iterations = 0 (0.00)
acuSolve: GMRES 0/1/n norms = 0.000000e+00 0.000000e+00 0.000000e+00
acuSolve: GMRES Iter. CPU/Elapse = 0.000000e+00 4.410744e-05
acuSolve: diss.-rate sol ratio = 0.000000e+00

You may want to try a different choice for the inlet turbulence type and parameters.  Have you considered the Spallart-Allmaras model instead of standard k-epsilon?  Or even realizable k-epsilon instead of standard?

I tried changing the turbulence model and i could see that dissipation rate equation is being solved. But again, I could see huge difference between results obtained just by changing the nodal initial conditions.

acupro

Prabin Pradhananga_20428 said:

I tried changing the turbulence model and i could see that dissipation rate equation is being solved. But again, I could see huge difference between results obtained just by changing the nodal initial conditions.

Yes - as expected.  If the initial conditions (initial guess to the solution) are so far away from the actual solution, the solver may have a very difficult time getting there.  In this case you likely have poor convergence, a high degree of reverse flow at the outlet, etc.  Best to use initial conditions closer to expected solution.

Prabin Pradhananga_22497

acupro_21778 said:

Yes - as expected.  If the initial conditions (initial guess to the solution) are so far away from the actual solution, the solver may have a very difficult time getting there.  In this case you likely have poor convergence, a high degree of reverse flow at the outlet, etc.  Best to use initial conditions closer to expected solution.

One more question, what is 'automatically define pressure reference' in launch acusolve dialog box?