CFX5.6 error message #001100279
 

Hi guys,

I get this error message while running the solver in CFX5.6:

ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | c_fpx_handler: Overflow

It stopped at 9th iteration. I used the SST turbulence model, a blend factor of 0.75, autotimescale, RMS of 1e-7.

It's a steady state curved duct flow problem with the velocity profile as the inlet boundary condition and zero static pressure (opening) as the outlet boundary condition. The fluid is water at 25C.

The tet mesh is generated by ICEM CFD.

Anyone know how to get rid of this error? :( Please kindly advise me. Thank you very much.

Re: CFX5.6 error message #001100279
 

Hi Jenny,

We'll need more information to help you diagnose the problem. How was convergence going before it crashed? What about the imbalances? Save a backup file before it crashes and have a look at it in Post. Is the simulation going berko in some region? Maybe it is going berko everywhere?

I have not come across that exact error before, but on the face of it I suspect it is from either a non-physical setup, a mesh size problem or a timestep size problem.

Glenn

Re: CFX5.6 error message #001100279
 

I will look at it now and get back to you asap. Thanks for offering help.

Glenn, can you please tell or direct me to any notes that talk about "non-physical setup, a mesh size problem & timestep size problem"? I don't exactly sure about what you are saying here. Thanks.

Re: CFX5.6 error message #001100279
 

Hi Jenny,

A non-physical setup is where you are asking the code to solve a flow which is not phyiscally possible. A few examples could be a steady state flow with 1kg/s flowing in the inlet, but 2kg/s flowing out the outlet; or in compressible flow trying to pull a mass flow rate larger than the choked flow possible for that geometry at that condition. Both of these simulations would cause the solver to crash in weird ways.

Mesh size can lead to problems as if it is too coarse it does not resolve the flow enough to give a sensible answer. Too small a mesh can also be a problem but it is rare to get this problem.

Time step size is a major cause of mysterious problems in transient flows as if the timestep is too large it makes the solver unstable. Easily fixed with smaller timesteps (once you've identified that it is the problem - that's the hard bit!)

Glenn

Re: CFX5.6 error message #001100279
 

Hi Jenny / Glenn, I've experienced this error usually in one of two ways. Firstly it was due to large time steps, and secondly due to partitioning problems. The second is easiest to check provided you have enough ram. If this is the problem then you can try using different partitioners or partitioning in a different direction. Glenns suggestions should solve the time stepping problems. Good luck

Bob

Re: CFX5.6 error message #001100279
 

Thanks, Bob. I'm using the auto time step. Should that be enough for steady state simulation? Are there any criteria to determine the time step manually? Or I just have to try until the problems disappear....

The server has about 24G of Ram. It should be sufficient to solve the the steady state curved duct flow (with about 700K of elements), right?

To Glenn: I have more than 20 elements across the diameter & 5 inflation layer. It should be fine enough, I think. I also check the tet mesh quality & problems in ICEM CFD b4 exporting that to Pre.

The flow is assumed fully developed & turbulent. Boundary condition for inlet is velocity profile & for outlet is opening (with zero static pressure, reference press=0pa). It's bounded by the smooth wall(internal flow problem). I think it should be physically correct.... Please let me know if you can spot the error? It's not the problem of using SST turbulence model. I tried different option and ended up with same error message.

I can't find any info about the imbalance in the out file. Here is a picture of my solver screen: http://www.angelfire.com/ab7/cfdwork/error.jpg

Can you please take a look and see if covergence is okay? Sorry that I can't really tell from the chart if the convergence rate is weird or not.

Now, it left with the time step problem as mentioned by Bob. I have little idea of how to tackle this.

Any suggestions from you guys? Thank you for helping me. *__*

Regards, Jenny

Re: CFX5.6 error message #001100279
 

Jenny,

Looks like it's blowing in the turbulence equations. Up until then convergence is looking fine, but really it's still in the startup phase after 9 iterations. I would look at a few things:

1. Initial guess. Was your initial guess automatic or did you actually attempt to set something that conforms to your geometry.

2. Timescale. Sometimes the autotimescale may not be appropriate. Try selecting a physical timescale that is 1/3 -> 1/5th of the characteristic Length/Velocity scale for your duct.

3. Get rid of the opening at the outlet. Use an average static pressure condition instead. Only use the opening condition if you are positive there might be some reverse flow. It doesn't sound to me like there is any chance of reverse flow with your geometry.

Neale

Re: CFX5.6 error message #001100279
 

Neale:

Thank you for your response here. I re-ran the simulation with outlet instead of opening. It ended up with the same error. (Stopped after 12 iterations, the RMS error went flat in the last few steps!)

I used catersian velocity (0 0 Wprof) as an initial guess and set others as default.

I will look at how to specify the timescale right now. Does CFX do the same thing for its default?

It's kind of weird. When I used CFXBuild(5.5.1) to generate the mesh (although the mesh quality is not very good), it didn't show me such an error. However, I get this error when I create the mesh using ICEMCFD. Could that be the mesh problem? Anyone know how to analyse if mesh is a problem or not? I have already done all the mesh check & smoothing in ICEMCFD.

Thanks for your time in helping me, guys.

Regards, Jenny

Re: CFX5.6 error message #001100279
 

Hi Jenny,

Next thing to try is Neale's suggestion of a better initial condition. Run a model using the zero equation model and upwind differencing scheme. This model is pretty robust and should converge. The result it gives will be pretty inaccurate, but should be a far better initial guess than what you are currently using. Use that result as the initial condition for a run using the turbulence model you want to use, and second order differencing and hopefully your convergence will be improved.

Glenn