[UsamaQ]

Hello everyone,

I previously posted about getting this error in CFX everytime when I try to run simulation with user defined material.
I checked the FAQ section regarding this error and checked everything. I then tried to run the simulation with defualt material Air and it converged. So, basically my setup is okay because it converged.

Now moving on to next step, i checked the material properties as if they are correct and I am using Refprop and the values are fine.

But the error still persists, its been 4 weeks I am stuck at this point and cannot proceed further. Can someone help me?

I can provide files too if needed.

Using ANSYS 19.2.

[Gert-Jan]

I would start with uploading your complete output file. Not only small parts as in the previous posts. So we can check your setup and where the error occurs.

[ghorrocks]

Please post your output file as Gert-Jan requests.

Don't forget that most of the simple build in materials (eg the default air model) are very numerically stable. This means they should converge quickly and easily. But if your material model is unstable (which looks highly likely), even if it is correct, the simulation will diverge with a floating point error. It is normal to have to take measures to improve numerical stability when you use complex custom material models.

[UsamaQ]

Hello,

Thank you for reply.

I have attached the output file.

[Gert-Jan]

Advice 0: Simplify. Go 2-3 steps back.
Advice 1: start with a simple geometry, something like a pipe. And test your material there first in the range of pressures and temperatures that you expect. If it works there, then you can progress to more complicated setups like your geometry.
Advice 2: Use more significant numbers in polynomial coefficients. If you have something like a*T^5 it makes quite a difference if a is 0.002 [K^-5] or 0.002049 [K^-5]. (Double precision won't save you). Test your polynimial equations over and over and over in a spreadsheet. Make sure the numbers are realistic.
Advice 3: start with a lower rotational speed. You can always increase speed on a restart. If you want to get to the top, don't jump, but climb, or crawl.
Advice 4: You use a pitch of 1. That means 360°. Then, don't use a pitch, but just automatic.

[ghorrocks]

I have given it a quick look. An obvious major problem is the out of bounds error in pressure vs enthalpy. You will need to fix this by the methods it describes as it will never converge when your material properties are being clipped.

You are also getting speeds of Mach 11 on the first time step - this is likely linked to the clipping.

Once you have fixed the clipping problem you should look at the comments listed in the FAQ. They describe the things you should consider as a first try to get convergence.

[UsamaQ]

Thank You. I will try to do that step by step.

[Opaque]

May I ask the rotational speed in layman units, ie. RPM?

Your setup is at 50 000 [rad s^-1] --> 477 000+ [rpm]

I do not think the model will ever converge using a timescale of 2E-5 [min], which means the impeller basically turned more than 1 [rev] in a single timestep.

[UsamaQ]

Thank you @Opaque for highlighting that silly mistake. I didn't see it was set to 50000 rad/s. It is 50000 RPM and now i see It didn't show the same error. Thank you everyone. I hope it will work fine now.

Will let you know if something happened.