[UsamaQ]

Hello everyone,

I am trying to run simulation of compressor but I am getting error again and again, I have checked boundary conditions, changed time scale, model everything but the solution is diverging. Can someone please look at output file and tell me what is wrong. I have checked CFX wiki but still couldnt solve the issue.

Thank you

[AtoHM]

Something is at least wrong with your mesh, look at the expansion ratios it shows in the Mesh Statistics section. And your Mach number is skyrocketting, its related I guess.

[UsamaQ]

Hey. Thank you. I believe this is due to the mesh because I checked antoher converged solution of kinda same geomtry but less than 1000 expansion ratios. I will try to improve mesh. Will let you know

[ghorrocks]

The rapidly diverging Mach number means that the FAQ on floating point error is relevant here (it is a very similar problem): https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F

* The mesh quality issue is very important, definitely need to improve that.
* You have viscous work turned on. Unless you need it turn it off.
* Are you sure the flow is not choked?
* As the FAQ says, the first things you try in this case are: double precision numerics, smaller time step, improve mesh quality, better initial conditions.

[Gert-Jan]

Another 50 cents:
You have challenging boundary conditions. And you use them all starting from iteration 1, without any initial guess.
I would start with a lower massflow and rotational speed. Get it converged and then restart with tougher settings. Do it over and over, until you get where you want to be.

Although CFX can be quite forgiven for bad mesh and tough boundary conditions, I think you push it too far. You want to be on top of a mountain and try to jump to get there at once. But you need to climb and take a rest a few times.

[UsamaQ]

Thank you so much guys. I refined the mesh, reduced mass flow rate and velocity and it finally converged. One thing is still confusing me, the direction of rotational velocity. I have attached the image, can you please tell me for clockwise rotation about z-axis (from the top view), should input velocity be positive or negative? How can I check it in post?

[Opaque]

Your last question is ill-posed. You are showing the impeller, and a coordinate frame in a viewer, but you have not explicitly stated/described nor shown which direction for the axis you selected.

You can still in the domain models panel select -Z as the axis, and any answer to your question will be wrong or right.

For anyone to help, you need to state the direction of the axis by either showing the panel, or indicating which axis direction you have selected.

Hope the above helps,

[UsamaQ]

Hello. Sorry for the missing information. I selected the positive Z-axis (axis 1.3) as axis of rotation.

[Opaque]

For a compressor, the impeller must rotate from the Y-axis towards (using the shortest angle) the X-axis; therefore, then you must set a negative value for the angular velocity in the panel.

[UsamaQ]

Thank You. I already set negative value. was just need confirmation if doing it right or not.

[UsamaQ]

Hey Guys, I am facing aproblem regarding inflation layer. I am trying to place inflation layers around blades by appropriate first layer thickness (y plus 1), the inflation layer is generated but the mesh quality decreases and Aspect ratio + Expansion ratios becomes very high. This is causing the solver to diverge.

How can I solve this issue? If I remove inflation layers, the solution converges.

[Gert-Jan]

Go to ANSYS' Mesh & Geometry forum and add a few pictures. Otherwise people can't help at all.

[Opaque]

"boundary layer" meshes have very high aspect ratio. That is the norm.

Once your aspect ratio goes above 1000, you should use the double precision solver, and also beware that you are resolving additional features you did not capture with the coarser meshes.

As Gert-Jan suggested, a picture is worth a thousand words.