[alloveyou]

Hi all, I started one transient simulation of cavitation in a turbine by using a steady state simulation as the initial guess. The transient simulaiton is based on the steady state simulation and I only change the steady items to the transient items.
When i start transient simulation and in the first time step it stoped at the 6 COEFFICIENT LOOP ITERATION and the mistake showed below:

COEFFICIENT LOOP ITERATION = 6 CPU SECONDS = 1.773E+03
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-Bulk | 1.37 | 5.4E-03 | 2.0E-01 | 3.9E-02 OK|
| V-Mom-Bulk | 1.41 | 5.5E-03 | 2.6E-01 | 2.3E-02 OK|
| W-Mom-Bulk | 2.75 | 2.7E-03 | 8.1E-02 | 3.2E-02 OK|
| P-Vol |11.96 | 2.1E-03 | 2.5E-01 | 29.1 8.7E-02 OK|
+----------------------+------+---------+---------+------------------+
+--------------------------------------------------------------------+
| ****** Notice ****** |
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 0.9% of the faces, 0.2% of the area) |
| to prevent fluid from flowing into the domain. |
| The boundary condition name is: OUTLET. |
| The fluid name is: vaporair. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead. |
+--------------------------------------------------------------------+
+--------------------------------------------------------------------+
| ****** Notice ****** |
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 0.9% of the faces, 0.2% of the area) |
| to prevent fluid from flowing into the domain. |
| The boundary condition name is: OUTLET. |
| The fluid name is: liquidair. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead. |
+--------------------------------------------------------------------+
+--------------------------------------------------------------------+
| ****** Notice ****** |
| A wall has been placed at portion(s) of an INLET |
| boundary condition (at 100.0% of the faces, 100.0% of the area) |
| to prevent fluid from flowing out of the domain. |
| The boundary condition name is: inlet. |
| The fluid name is: vaporair. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead. |
+--------------------------------------------------------------------+
+--------------------------------------------------------------------+
| ****** Notice ****** |
| A wall has been placed at portion(s) of an INLET |
| boundary condition (at 100.0% of the faces, 100.0% of the area) |
| to prevent fluid from flowing out of the domain. |
| The boundary condition name is: inlet. |
| The fluid name is: liquidair. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead. |
+--------------------------------------------------------------------+
| Mass-liquidair | 1.16 | 4.8E-03 | 2.7E-01 | 6.1 8.6E-03 OK|
+----------------------+------+---------+---------+------------------+
| H-Energy-vaporair |11.14 | 1.4E-01 | 5.3E+00 | 1.5E-06 OK|
| H-Energy-liquidair | 1.32 | 1.1E-01 | 3.2E+00 | 6.1 3.6E-03 OK|
+----------------------+------+---------+---------+------------------+

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

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine C_FPX_HANDLER: |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

Besides, I have changed many things including timesteps, boundary conditions, turblence model and transient scheme, but it still don't convergence.

Now I'm confused and anyone can help me and give me some advice?
If need message in detail please contact with me.
Thank you very much!

[Liam]

I had a similar 'overflow' error in a completely different simulation when I'd made a mistake in the setup and an incredibly large number resulted while it was being solved.

I would say your problem is in the setup stage somewhere, sorry I can't be more specific.

[Doginal]

Read the notices that have come up.

You have flow trying to enter at a place where you have an outlet boundary condition and you have flow trying to leave where you have an inlet condition. The inlet is most significant considering 100% of that boundary the flow is trying to leave.
This is what is probably causing the error. When flow tries to go through a portion of a boundary in the wrong way (out an inlet or in an outlet) it treats that portion as a wall and just stops the flow from happening. This notice is usually seen when people specify an outlet in an area where recirculation is occurring.
In your case 100% of the inlet is seeing flow trying to leave that boundary. My first guess is that you have an error with your boundary conditions. Check the following
- If you specify an inlet velocity, check if it should be negative or positive
- If you specify a momentum source, check if it should be negative or positive
- Check your boundary conditions at the correct boundary (make sure you didn't put your inlet at your outlet or something like that)

I'm fairly certain it is just a error in boundary conditions but if not, you may want to then look at a slightly different meshing strategy, or at least that's what I would do.

Thank You,

DM

[alloveyou]

Originally Posted by Liam

I had a similar 'overflow' error in a completely different simulation when I'd made a mistake in the setup and an incredibly large number resulted while it was being solved.

I would say your problem is in the setup stage somewhere, sorry I can't be more specific.

Thank you,liam.
I have checked the setup stage several times and changed a lot, but I still didn't get the correct solver.

[alloveyou]

Originally Posted by Doginal

Read the notices that have come up.

You have flow trying to enter at a place where you have an outlet boundary condition and you have flow trying to leave where you have an inlet condition. The inlet is most significant considering 100% of that boundary the flow is trying to leave.
This is what is probably causing the error. When flow tries to go through a portion of a boundary in the wrong way (out an inlet or in an outlet) it treats that portion as a wall and just stops the flow from happening. This notice is usually seen when people specify an outlet in an area where recirculation is occurring.
In your case 100% of the inlet is seeing flow trying to leave that boundary. My first guess is that you have an error with your boundary conditions. Check the following
- If you specify an inlet velocity, check if it should be negative or positive
- If you specify a momentum source, check if it should be negative or positive
- Check your boundary conditions at the correct boundary (make sure you didn't put your inlet at your outlet or something like that)

I'm fairly certain it is just a error in boundary conditions but if not, you may want to then look at a slightly different meshing strategy, or at least that's what I would do.

Thank You,

DM

Thank you,Doginal.
I set the boundary condition like this: inlet: Total pressure and Total temperature;outlet: static pressure.
I also changed the mesh like increase or decrease the mesh.
But it still didn't work.
What i wondered is that if it is the problem of boundary condition or mesh ,why the steady can be simulated and the transient can't...

[ghorrocks]

The error you are getting is typical of a big numerical divergence. Assuming the problem setup is correct (ie inlet pressure higher than outlet), then you need to improve the numerical stability of the simulation. In this case where you are restarting from a steady state run I suggest using a much smaller timestep is recommended. Also double precision numerics is highly recommended for cavitation due to the large pressure differences.

[Doginal]

Originally Posted by ghorrocks

The error you are getting is typical of a big numerical divergence. Assuming the problem setup is correct (ie inlet pressure higher than outlet), then you need to improve the numerical stability of the simulation. In this case where you are restarting from a steady state run I suggest using a much smaller timestep is recommended. Also double precision numerics is highly recommended for cavitation due to the large pressure differences.

It just seems very odd that all the flow is trying to exit the inlet and that's what leads me to believe its a CFX-Pre error in boundary conditions.

You mention that your using total pressure and static pressure to define your inlet/outlet. Make sure its not set up so that your static pressure is higher than the defined total pressure.

Also try running the simulation to a point that you know it wont crash yet (so only a couple timesteps) or even stop it and look after you do a steady state simulation. Look at the pressure profiles and velocity and make sure the flow is doing what you expect.

[ghorrocks]

You can get weird reverse flow like this even when the pressure difference is correct when the simulation is diverging badly. So if you reckon the BC setup is correct then it probably is a convergence problem.

As I said, I recommend using far smaller timesteps and double precision numerics as that may help the convergence.

[alloveyou]

Originally Posted by ghorrocks

You can get weird reverse flow like this even when the pressure difference is correct when the simulation is diverging badly. So if you reckon the BC setup is correct then it probably is a convergence problem.

As I said, I recommend using far smaller timesteps and double precision numerics as that may help the convergence.

Thank you very much,ghorrocks!
I have checked the inlet and outlet boundary conditions,and I think it's right and can simulate under the steady condition.Here, you mentioned the "double precision numerics", I don't know what it specifically means and how to set it.Does it set in the solver?
Thank you!

[ghorrocks]

Look at the solver manager when you define a run, under advanced.

[rahpooye313@yahoo.com]

change "outlet" boundary type to "Opening" boundary type with same condition.
(Opening/opening outlet)

[sheikh nasir]

Hello
i am getting floating point error:invalid number in my thesis ie train moving in tunnel. Can any body help me. My email is sheikhnasir39@gmail.com
thanks

[ghorrocks]

Do a search on the forum for floating point error - there are lots of posts on this and what to do. When I get time I will write an FAQ on it.

[coolguys]

Dear ghorrocks, I got the floating point overflow error, than i reduce the physical time scale up to 0.0002 sec. and select the " Double precision" but still I have confusion is that select only double precision or also select double precision with override . please reply me.

[Mina_Shahi]

Originally Posted by ghorrocks

The error you are getting is typical of a big numerical divergence. Assuming the problem setup is correct (ie inlet pressure higher than outlet), then you need to improve the numerical stability of the simulation. In this case where you are restarting from a steady state run I suggest using a much smaller timestep is recommended. Also double precision numerics is highly recommended for cavitation due to the large pressure differences.

Hi Glenn

I have the same problem i switched to double precision, i used smaller time step, they helped to have better convergence but still i get this message

--------------------------------------------------------------------+
| ****** Notice ****** |
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 100.0% of the faces, 100.0% of the area) |
| to prevent fluid from flowing into the domain. |
| The boundary condition name is: Outlet_Air. |
| The fluid name is: Fluid 1. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead.

switching to opening boundary condition won't work because we shouldn't have back flow. What do you suggest? Can be the mesh causing the problem?

[brunoc]

You might have placed your boundary condition near a recirculating region. Save a backup file and check the flow near the outlet region.

The CFX documentation has guidelines for correctly placing an outlet boundary condition in your domain. Search the documentation for 'Using Inlets, Outlets and Openings' and look at the explanation under 'Openings'. You'll see a comparison of bad, better and ideal locations for placing your outlet region.

Cheers