CFX Solver stopped with error when requested for backup during solver running
 

Hi All,

I am using ansys cfx under ansys workbench and simulating a supersonic flow. I am facing a problem that whenever I go for taking backup while cfx solver running. The solver first shows writing back up and then stopped with error. The situation is very worst as during this practice I lost 4,5 hours of solver generated data.

I have attached a snapshot of cfx solver error. Please suggest a solution as I have already lost several hours of valuable data and this problem is wasting my time.

Any help/suggestion will be appreciated.

Thanks in advance,

Faizan

I suspect your results have diverged so far that it cannot write a results file inside the reasonable bounds of the variables. To fix this you should write backup files more often so you can get some backup files before the results have diverged that far, where it will be able to write backup files.

Hi Glenn,

Thanks for your suggestion.I appreciate. I reckon you are right because when I read the output file, I found the mach no notice and it was extremely high.

I have one more query- Like you said if I take frequent back up and if my solution is diverging then will it gonna help me to get converge solution or the problem would remain the same.

Pl. suggest about it and how to control the mach no value which is going crazy.

Look forward to gear from you,

Regards,

Faizan

If you take frequent backup files, if it diverges, crashes and does not save a result file it allows you to:
1) go back to the last saved backup file and have a close look at it. You will probably find a region in the flow which is starting to go a bit crazy but has not completely blown up yet. This is a clue as to where the problem is.
2) Restart the run using the last good backup file, using a revised setup which will fix the problem (maybe smaller time steps, or more ramping of flow variables or whatever works)

Thanks again for your assistance.

Would you please elaborate more on how to identify the problematic region from backup file or output file. I had no clue about locating the exact location where crash occur.

Please suggest.

Look forward to your response,

Regards,

Faizan

It's likely that the failure has occurred when the solver is attempting to write hybrid (boundary) values, which are calculated for the results and backup files for post-processing.

The bounds error is the Density falling below zero, so first check where the density is very small and try to figure out why that is happening (low or negative absolute pressure, for instance).

Although the solver crashed, you may be lucky - sometimes it leaves an incomplete backup/results file (usually with an odd name like 'zlkiisddan ...') in the run directory which can still be read into CFD-Post.

CG

Hi cfdgremlin,

Thanks for your suggestion- I checked the file you mentioned but it only showed the values on legen bar but on the graphic window.

Can you suggest me as how to locate the problematic region in the 3D model. I mean location in x,y,z terms. I am still unsure if it is happening because of mesh. Because I generated the fine mesh to capture the supersonic flow. I used GGI interface to assemble 3 fluid and one solid domain.

Please suggest.

Regards,

Faizan

I would write a backup file every iteration until the failure. You need to check the absolute pressure and the density values to make sure they are physical.

This problem can sometimes happen if your reference pressure is set to zero and the solver calculates a zero relative pressure during the calculation. You might get round it by specifying pref=1atm and setting your pressure boundary conditions relative to this.


Hope this helps.

Hi cfdgremlin,

Thanks for highlighting an important point. Yes you are right, I checked the reference pressure and it is set to 0 bar.

Now I need your assistance to set pressure value as per your suggestion.

I set total pressure and total temperature boundary condition at inlet. The values are total pressure = 25 bar; total temperature = 550 celsius

Please suggest as how should I play with these pressure values to set ref pressure equal to 1 atm- which is 1.01325 bar in general. Also please shed some knowledge about its implication on numerical results and outcome.

Thanks for your helpful suggestions once again.

Look forward to hear from you,

Thanks in advance

Regards,

Faizan

Hi Maxim,

Thanks for your suggestion. I have gone through the documentation which is quoted below:
"""
1.2.8. Setting a Reference Pressure
In CFX, you must specify a Reference Pressure for your simulation. The Reference Pressure is specified
on the Basic Settings tab of the Domains form, but is a property of the entire simulation so all domains
must use the same value. Each time you create a new domain or apply a change to an existing domain,
the Reference Pressure in that domain is applied to all domains.
All relative pressure specifications set in CFX are measured relative to this Reference Pressure value.
The Reference Pressure will affect the value of every other pressure set in the simulation.
The reference pressure is used to avoid problems with round-off errors. These can occur when the dynamic
pressure change in a fluid, which is what drives the flow, are small compared to the absolute
pressure level.
For example, low speed atmospheric air flow may have dynamic pressure changes of only a few Pascals
or less, but the changes are relative to the atmospheric pressure of around 100,000 Pa. If you are dealing
only in absolute pressure terms, these small pressure changes can get lost in round-off errors when
performing calculations (for example, a change of 1 Pa is a change to the sixth significant digit). To
rectify the situation, you should set a sensible Reference Pressure level. In this case, the local atmospheric
pressure of 100,000 Pa is suitable. This value will be used as the new datum (instead of 0 Pa)
about which all pressures are calculated. A change of 1 Pa will now be a change to the first significant
digit.
As a counterexample, a reference pressure of 0 Pa can be used without any problems when the dynamic
pressure changes are significant compared to the absolute pressure level.When modeling a liquid flow
where nothing depends on the pressure level, there is no need to specify an atmospheric reference
pressure.
When boundary and initial conditions are specified, they are set relative to the reference pressure. If
you require a boundary to have an absolute pressure level of 100,000 Pa, you could:
• Set a relative pressure value of 0 Pa for the boundary if the reference pressure is 100,000 Pa or,
• Set a relative pressure value of 100,000 Pa for the boundary if the reference pressure is 0 Pa.""""

Now I wish to inform you that as suggested in the documentation, I have set 0 ref pressure and 100000 Pa relative pressure. But the issue is that as highlighted by cfdgremlin that negative density zones are appearing. I am very much agreeing with cfdgremlin point of view because i have checked every other things, mesh is also fine. So my question is that "How should I manipulate reference pressure in my existing code to avoid solver crashing and to avoid result accuracy damage?"

If I put any random ref. pressure then the results will be dodgy. How do you reckon?

Please suggest.

Any expert help would be much appreciated.

Thanks in advance,

Faizan

you wrote that you've tried setting the reference pressure to 0 Pa. Have you also tried setting the reference pressure to 1 bar/1atm as the quoted documentation suggests?

It seems that you also have problems locating the problematic regions in Post from your backup files? You could insert a 'point' location and use 'minimum value' of pressure/density etc. Or insert an isovolume with the setting 'values below 0 Pa' for example. Look at streamlines for strange backflows etc. If you don't know how to insert/create those things, the tutorials or documentation will help you.

Hi Maxim,

Thanks for your assistance and suggestions. No I haven't tried with 1 bar. I would try and let you inform if problem still exist.

thanks for your time. I appreciate.

kind regards,

Faizan

You mentioned earlier in this thread the inlet pressure of 25 bar; have you specified a zero pressure boundary condition (perhaps an outlet) anywhere? This could be where the problem lies.

Hi cfdgremlin,

yes I put 25 bar total pressure and 750C total temperature at inlet of the nozzle. No I haven't used any outlet boundary condition anywhere. Instead I put Opening boundary condition on three surfaces of cylindrical surrounding domain.

The only 0 bar pressure was set as reference pressure which I mentioned in my earlier post.

Pl. suggest.

Thanks

Faizan

The reference pressure is an issue, but probably a minor one. If he defined zero reference pressure where it should have been 1 atmosphere that means he is only off by 1 in 25 atmospheres, and that is not much in the scheme of things.

Right back at the start of this thread Faizan mentioned that his simulations were diverging. I presume this is the real problem with this simulation, he wants these simulations to converge.

If this is the case then these FAQs are relevant (although on slightly different topics):
http://www.cfd-online.com/Wiki/Ansys...gence_criteria

http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

And of the tips on these pages by far the most important is mesh quality. Improvements in mesh quality make a massive difference in ease of convergence.

Dear Glenn,

Hi,

Thanks for your expert suggestions. I appreciate. To be very honest with you- I have gone through these pages several times. I have only one doubt which you mentioned that mesh quality of my current CFD case might not helping in convergence. But my intention is to develop the CFD case on optimized mesh not with fine or extra-fine mesh elements. As you are aware that with fine or extra-fine mesh it increases the simulation time to several weeks or months which I can not afford at the moment.

My worries is that even if it is a bad quality mesh then then there should be some technique to control the divergence or avoiding solver from failure. I know I could sound stupid but I need a solution for this. Refining mesh or increasing mesh elements would only increase time unnecessary.

I am saying this because even with solver failure or divergence the results of my CFD case are realistic and close to experimental data. I plotted it on CFD post using backup files.

I would appreciate if you can suggest some smart tips of achieving convergence without increasing mesh elements. I would be grateful to you.

Thanks in advance,

Regards,

Faizan

Do not get confused between mesh quality and mesh density. Mesh quality is how orthogonal, regular and well shaped the mesh is - it has nothing to do with how fine the mesh is. Mesh density is how many nodes you have and how large the elements are.

Improving mesh quality will always make convergence easier and faster. Increasing mesh density (ie a finer mesh) will make convergence harder and slower.

I recommend you look at your meshing technique to improve the quality, not the density. As you say, you increase the mesh density once the coarse mesh simulations are working well.

Hi Glenn,

Thanks for your clarification and identifying the valid point.

I am posting a screenshot of Mesh Statistics of my running simulation on 1e-9[s] physical time scale. Just for your info. It's running since 7 days continuously and right now iterating loop is 3403.

I reckon the quality of mesh is sufficient to undertake a supersonic gas flow at high pressure and temperature.

Please have a look and suggest.

I will be grateful.

Thanks in advance,

Regards,

Faizan

Is that right? What do you base that opinion on?

If you are up to iteration 3403 then you have a major problem with convergence. I suspect this FAQ is important: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

That FAQ suggests methods to get it to converge as it is, but everything will be easier if you improve mesh quality. Trust me :)