[fergal]

Hi,

I'm quite new to CFX, i am currently modelling laminar and turbulent incompressible flow over a smooth flat plate. I have completed the laminar model, however when i increase the velocity (selecting the SST model) the solver crashers during the first iteration.

the error given is a floating point error; zero divide.

I'm using CFX-Meshing and i have conducted a sensitivity analysis (the laminar option works but the turbulent option doesn't using the same mesh).

thanks in advance for any help

Fergal

[ghorrocks]

Steady state or transient?

[fergal]

Hi ghorrocks,

The model is steady state, i'm unsure of what aspect of the model is giving issues. The mesh i am using is an extruded 2D mesh with an expansion of 5% from the plate.

Thanks for your help.

Fergal

[ghorrocks]

What is the error message? Please post the final sections of the output file.

But the answer almost always is to use a better initial guess to start you off. Use a laminar model as an initial condition. Even if it was done at a different flow velocity it is better than nothing. And you will probably need a smaller physical timestep to start off. Once it has started and is reliably converging then increase the time step size.

[fergal]

please see message below,

+--------------------------------------------------------------------+
| Convergence History |
+--------------------------------------------------------------------+

================================================== ====================
| Timescale Information |
----------------------------------------------------------------------
| Equation | Type | Timescale |
+----------------------+------------------------+--------------------+
| U-Mom | Auto Timescale | 1.59399E-04 |
| V-Mom | Auto Timescale | 1.59399E-04 |
| W-Mom | Auto Timescale | 1.59399E-04 |
+----------------------+------------------------+--------------------+
| K-TurbKE | Auto Timescale | 1.59399E-04 |
| O-TurbFreq | Auto Timescale | 1.06266E-04 |
+----------------------+------------------------+--------------------+

================================================== ====================
OUTER LOOP ITERATION = 748 ( 1) CPU SECONDS = 4.843E+04 (1.994E+01)
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Floating point exception: Zero divide |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| Writing crash recovery file |
+--------------------------------------------------------------------+

Details of error:-
----------------
Error detected by routine POPDIR
CRESLT = ILEG

Current Directory : /FLOW/NAMEMAP

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created. |
+--------------------------------------------------------------------+

End of solution stage.

+--------------------------------------------------------------------+
| Warning! |
| |
| The ANSYS CFX Solver has written a crash recovery file. This file |
| has been saved as |
| C:\Users\Administrator\AppData\Local\Temp\Turbulen t_rev01_5440_Wo- |
| rking\dp0\CFX\CFX\Work1\CFX_002.res.err and may be an aid to |
| diagnosing the problem or restarting the run. More details should |
| be available in the solver output section of the output file. |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| The following user files have been saved in the directory |
| C:\Users\Administrator\AppData\Local\Temp\Turbulen t_rev01_5440_Wo- |
| rking\dp0\CFX\CFX\Work1\CFX_002: |
| |
| mon |
+--------------------------------------------------------------------+


This run of the ANSYS CFX Solver has finished.


i forgot to mention that i got a k-eps model running under similiar conditions. i tried a similar problem using a mapped face meshing and SST model and it worked fine.

Thanks again

[ghorrocks]

OK, so it is diverging in the first iteration on the first set of equations. Then you need a better initial guess or smaller timesteps to start off with.

[fergal]

Hi

Thanks again for the quick response, i tried reducing the timestep and ran a K-eps model for the initial guess but it still keeps giving the same error.

i set up two models, both to model turbulent incompressible flow over a flat plate (sst).

1) the flat plate is a smooth no-slip wall (works)
2) the flat plate is a smooth no-slip wall with a small free-slip plate at the inlet (this is not working (see crash recovery file))

thanks again

fergal

[ghorrocks]

Is the no slip region planar? You might be able to make it a symmetry plane.

Also try making the timestep smaller still. How much smaller have you already gone, and what is the flow timescale? Also try starting with local timescale factor.

[fergal]

hi ghorrocks,

Thanks again for the hasty response and your help, i just ran the sst model using the results from the k-eps model and a local time-scale factor of 0.00001.
It is running . do you suggest stoping the run and changing the timescale back to automatic??(i tried this and the same problem persists)

thank you so much for the help.

Fergal

[ghorrocks]

If it needs such a tiny time step to start off then you will need to ramp it up to a sensible value slowly as the simulation progresses.

But if you need such a small value to start it off something is probably wrong anyway. Is your mesh quality good? Tried double precision numerics? What about using a symmetry plane rather than a slip wall?

And why do you want to put a slip wall in anyway?

[fergal]

Hi,

I set up a new model without the free-slip wall and it works fine. I was using the free-slip wall to reduce any negative effects at the leading edge of the plate (inlet condition).

I'm still unsure why the model runs with no free-slip region and it doesn't when the free-slip region is added to the model. This problem only exists for the SST model as the k-eps model works fine.

Is there a method within CFX of checking mesh quality?

Again thank you so much for the help.

fergal

[ghorrocks]

I have not come across a problem with free slip walls like this before. But I do not use free slip walls very much as they are not physically possible, and from your description of what you are doing I don't think you should use them either.

You can check mesh quality in the output file as a summary, or in detail using CFD-Post. Read the documentation to get a guide for how to interpret the mesh quality numbers.

[fergal]

Hi ghorrocks,

I have been going crazy with this model. I think one of the problems was drawing the geometry in mm in the design modeller (i use workbench) it seems to be sensitive to a change in units. A re-drawing of the model in metres seems to have worked. But would this have caused the problem.

I take your point on the use of free-slip walls.

Thanks for your patience and help.

Fergal

[Attesz]

I think one of the problems was drawing the geometry in mm in the design modeller (i use workbench) it seems to be sensitive to a change in units. A re-drawing of the model in metres seems to have worked.

I think it doesn't matter which unit you use. Your problem is propably related to your mesh or the boundary conditions. I did simulations on a centrifugal compressor with a very coarse mesh, and it converged in 200 iterations with automatic timescale and SST. Your model is more simple. Can you post images about the geometry or the mesh?