[Muh]

Hi,

I am new to STAR-CCM+ and I wonder how one can run multiple simulations consecutively? I have a simulation which I want to run with different inlet velocities. I want to run one simulation with a certain velocity during 3000 iterations and then run another simulation during 3000 more iterations and so on.

I tried some syntax definitions under Tools>Field function but could not understand how to Wright it and then initiate it.

[ThatGuy]

Hi,

if I understood it right, I think that you should run the first sim with a stopping criterium of 3000 steps, then you change the conditions, shift the stopping criterium to 6000 steps and run again. This way the simulations are consequent

[Muh]

Yes thats correct, I did something like this.

$Iterate < 3000?1:$Iterate < 6000?2:$Iterate < 9000?3:

Then I also set stop solution at 9000 steps and I also autosave at each 2999 iterations. Here I say iterate 3000 iterations with velocity 1 m/s and then run 3000 mre iterations with velocity 2 m/s and so.

[ThatGuy]

Yes, maybe you automated what I suggested you do manually. That's the way

[Muh]

thanks man,

Do you have any suggestions on the syntax definition? I have made the stopping criteria but some how the velocity is not included in the definition. I tried to some other syntax definitions but did not work. So my problem is in the syntax definition including the velocity

[ThatGuy]

I'm quite a newbie on star ccm+, so I never studied the syntax it uses. I think, but this is just a guess, that you have to pass through field functions.
Unfortunately I can't help you with this, maybe the user guide will give you some more hints. I don't even know what kind of code it uses.

[Owain_Parry]

Hello.

You need to define your own field function call it something like "0Inlet_Velocity" Putting the '0' at the start ensures it appears at the top of the field function list.

Then modify the following example to match your case:

$Iteration < 3001 ? 1.0 : $Iteration < 6001 ? 2.0 : $Iteration < 9001 ? 3.0 : OTHER CASE

The logic steps in the above algorithm is not optimal but it's the easiest approach for you to learn.

After this step you must now tell the inlet boundary to use the output from this field function as it's physical value for velocity. Go in to the inlet boundary definition in the regions tab. Under the physical values tab set the velocity magnitude method to "Field Function" and then the value must be set to the field function which you've just created "0Inlet_Velocity". I suggest you use the field function browser thing so that you get the syntax correct.

[Muh]

Thank you so much Owain_Parry. I did that and the only thing that was missing, was to define the boundary value as My Field function, just as you describe. :-)