[YOUNS]

Hello everyone!

I want to make a CEL that RPM is increase step by step.
For example, 1500 > 3000 > 5000 > 10000 > 50000 > 100000 > 154,000

I'm trying to analysis centrifugal compressor(RPM:154,000 and mass flow at outlet: 0.1056 kg/s). But, it occur "Fatal Over Flow" error message and stopped solving.

so, I think that cause of error is high RPM because, initial pressure is 1[atm] but, if impeller is suddenly rotating for 154,000rpm, pressure difference is very high.
or it is geometry or mesh problem.

Have you idea about this error?

At result~!!
I want to how to make a CEL that RPM is increase step by step.

teach me

thanks for read.

Heave a nice day!!!

[urosgrivc]

You can make either a:

+conditional IF expresion like this:
if(acumulated iteration number >10, than something, else something)
else something can be a nother if sentence.
if you are doing transient than acumulated timestep can be used
usualy changing parameters in stedy state has only wery limited use.

or:
+user defined function (a table of values)
you first set your units
than make a table first column could be seconds[s] and the second one can be revolutions per minute [radian s^-1] or what ewer.
than you set your values in the table,
0,0
1,100
this would mean that the rpms would be ramped up to 100 in 1second
You than use this function in an expression an put (t) in the end vhich means the expresion is time dependant
but this is not limited to time it could be T=temperature dependant or other.

probably best thing for vhat you vant is the first case as as i understand you are doing a steady state

[urosgrivc]

In your case I vould rather try decreasing the timescale factor at the begining of your simulation

[AtoHM]

The steps might produce some steep gradients as well, so you can also try a continuous increase. I did something similar a few weeks back.
Use your standard RPM expression and multiply it by an expression Scaling (for example): RPM * Scaling
Then you can just use the Time variable to scale it like:
if (Time<(Time Step Size * 100), Time / (Time Step Size * 100), 1)
which gives you a linear scaling during the first 100 time steps, which you can adjust to your needs.

[ghorrocks]

I don't think you want to increase the rotation speed every time step as it will never converge and could tie itself in strange knots. I would recommend starting with a constant speed and keeping the speed constant until you get monotonic convergence. Once you get monotonic convergence you know it has the fundamental flow field and then you can increase the speed.

And you should not need to do it in 7 steps like you initially suggest. Two steps is all required in most cases, 3 in exceptional cases. If you still cannot obtain convergence then something more fundamental is wrong, this FAQ might help: https://www.cfd-online.com/Wiki/Ansy...gence_criteria