[Mmaragann]

Dear CFD-Comunity,

I am simulating a centrifugal pump with a inducer. When I mesh the Inducer with a tip clearance at the shroud with Turbogrid everything is fine. Then I import the mesh to cfx. In the solver - before the first time step or pseudo time step - I get the error:

+--------------------------------------------------------------------+
| ERROR #002100011 has occurred in subroutine Out_NegVol. |
| Message: |
| A negative SECTOR volume has been detected. Execution will proceed |
| but this is a possible cause of robustness problems. |
| The location of the first negative volume is reported below. |
| Volume : -0.1281E-13 |
| Location : ( -0.14604E-01, -0.12401E-02, 0.66709E-01) |
| This warning may be made fatal by setting the expert parameter |
| 'negative volume option = 1'. |
+--------------------------------------------------------------------+

I have read every post on this in the forum. The Problem is, that the location given by the error isn't even in a mesh region. It is inside the hub and there is no mesh, that means there is no mesh for me to improve.

The error appears if I run the simulation steady state or transient, with rotating frame of reference or not - it doesn't matter. Also I don't have any mesh deformation, since I'm only simulating the fluid. Has it something to do with the Out_NegVol Routine? Nevertheless the simulation runs and the solver doesn't crash. I have yet to see my results in CFD post, but I am concerned about this error.

Any help will be very much appreciated.

Mmaragann

[Antanas]

Originally Posted by Mmaragann

Dear CFD-Comunity,

I am simulating a centrifugal pump with a inducer. When I mesh the Inducer with a tip clearance at the shroud with Turbogrid everything is fine. Then I import the mesh to cfx. In the solver - before the first time step or pseudo time step - I get the error:

+--------------------------------------------------------------------+
| ERROR #002100011 has occurred in subroutine Out_NegVol. |
| Message: |
| A negative SECTOR volume has been detected. Execution will proceed |
| but this is a possible cause of robustness problems. |
| The location of the first negative volume is reported below. |
| Volume : -0.1281E-13 |
| Location : ( -0.14604E-01, -0.12401E-02, 0.66709E-01) |
| This warning may be made fatal by setting the expert parameter |
| 'negative volume option = 1'. |
+--------------------------------------------------------------------+

I have read every post on this in the forum. The Problem is, that the location given by the error isn't even in a mesh region. It is inside the hub and there is no mesh, that means there is no mesh for me to improve.

The error appears if I run the simulation steady state or transient, with rotating frame of reference or not - it doesn't matter. Also I don't have any mesh deformation, since I'm only simulating the fluid. Has it something to do with the Out_NegVol Routine? Nevertheless the simulation runs and the solver doesn't crash. I have yet to see my results in CFD post, but I am concerned about this error.

Any help will be very much appreciated.

Mmaragann

Something wrong with mesh. The volume is negative and very small. Try to create isosurface of this negative volume value in CFD-Post to reveal bad cells.

[Mmaragann]

Dear Antanas,

thank you very much for your answer. I just did what you proposed, but unfortunately there is no volume of -0.1281E-13 in CFD-Post. Also the location the error gives me is outside the mesh and the fluid domain, so at this location there are no cells. So that is my problem - that there is no mesh to fix. When you do a rotor in Turbogrid, then inside the hub you have no mesh. but the error location is given me inside the hub, where turbogrid doesnt generate any mesh.

Best regards

[cfdgremlin]

Are you using the same unit system in Post? The solver location is probably reported in SI, but if you are using a different system in Post you'll need to account for this.

Anyway, it might be a good idea to check the quality of your mesh in Post by identifying regions where the smallest elements occur.

If you are not already, then you might need to run the solver in double precision if you have very small, or very high aspect ratio, elements.

CG

[Antanas]

Originally Posted by Mmaragann

Dear Antanas,

thank you very much for your answer. I just did what you proposed, but unfortunately there is no volume of -0.1281E-13 in CFD-Post. Also the location the error gives me is outside the mesh and the fluid domain, so at this location there are no cells. So that is my problem - that there is no mesh to fix. When you do a rotor in Turbogrid, then inside the hub you have no mesh. but the error location is given me inside the hub, where turbogrid doesnt generate any mesh.

Best regards

Share your mesh.

[Mmaragann]

Oh my. I don't know how I converted the units, but now I see where the problem is. It is in the mesh. For everyone struggeling with the same problem. CFX log file gives locations in meters, so keep that in mind, if your mesh in TG is in an other unit.

The poor mesh is at the leading edge in Turbogrid. So I will try to improve that.

Thanks to everyone here!