Learning Forum

[nisimshushan]

Hi.

I am using Ansys 2021R1 educational version to simulate a multiphase case.

I am able to get the case to start running on my PC, but when I upload it to our university HPC service, I get some persistent errors.

If anyone can help me figure out how to fix these errors, I will be eternally grateful.

Attached below are first the three errors I see, then ill attach some settings and the full error report.

-----------------------------------------------------------------------

Errors i get in the report after the case is dropped out of HPC

1)

Warning: the rp-transition-model option is not available in this solver

2)

Warning: property-info: unknown property: characteristic-vibrational-temperature

Warning: property-info: unknown property: characteristic-vibrational-temperature

Error: %cxg-ani-change-window: wta[2](int)

Error Object: #f

   parallel,

Warning: property-info: unknown property: characteristic-vibrational-temperature

Warning: property-info: unknown property: characteristic-vibrational-temperature

3)

> /solve/dual-time-iterate

Total Time [15] 15

Maximum Number of iterations per time step [40] 

Error: = (equal): invalid argument [1]: worng type [not a number]

Error Object: #f

40

--------------------------------------------------------------------------------------

Geometry Settings

[Rob]

Check the command you're using for the iterate command, if the text file came from Windows use the dos2unix command to strip white space characters out of the journal.
Not sure about the rp-transition-model warning, have you been messing with rpsetvar commands?

[nisimshushan]

Hi Rob
Thanks for your reply.
To my knowledge, I have not messed with rpsetvar command.
------------
what about the second error message?
2)
Warning: property-info: unknown property: characteristic-vibrational-temperature
Warning: property-info: unknown property: characteristic-vibrational-temperature
Error: %cxg-ani-change-window: wta[2](int)
Error Object: #f
parallel Warning: property-info: unknown property: characteristic-vibrational-temperature
Warning: property-info: unknown property: characteristic-vibrational-temperature
----------
Below is the script from the .txt file
---------
/file/rcd case2-7.cas.h5
/file/cff-files no
/file/autosave/data-frequency
1000
/solve/set/transient-controls/duration-specification-method
2
/solve/set/transient-controls/multiphase-specific-time-stepping
yes
0.8
1e-05
1
1e-05
10
0.8
1.2
1
/solve/dual-time-iterate
15
40
/parallel/timer/usage
wd case2-7.dat.h5
exit
y
------------------------
and this is the script from the _S.txt file
#!/bin/bash

#PBS -P fluent
#PBS -j oe
#PBS -N case2-7.cas.h5
#PBS -l select=16:ncpus=1:mem=1800mb
#### This is to request for 16 cores and 32GB RAM by default.
#PBS -l place=pack
#PBS -l walltime=720:00:00
#### #PBS -l fluent_lic=1;
#### this will be enabled in near future.

cd $PBS_O_WORKDIR;## this line is needed, do not delete and change.
np=$( cat${PBS_NODEFILE} |wc -l );### get number of CPUs, do not change

## Make a temporary scratch space (this should be on /scratch/)
scratch=/scratch/${USER}/${PBS_JOBID}
export TMPDIR=$scratch
mkdir -p $scratch

##--- Put your exec/application commands below ---
module load Ansys/2020R1
fluent 3ddp -g -t${np} -pshmem -ssh -i case2-7.txt

# Remove scratch space
rm -rf $scratch
exit $?

##--- END HERE ---
---------------------------------

[Rob]

Journal command looks OK, but check for white space characters as they can be added by Win10 but are seen as command syntax on Linux.
Can you post the screen shot of the start of the property error? Staff are not permitted to open or download attachments.

[nisimshushan]

Thanks, I will look for white space characters
---------------
I don't know what you mean by "property error"
Where do I find it?

[Rob]

Warning: property-info: unknown property: characteristic-vibrational-temperature

[nisimshushan]

[nisimshushan]

i think part of the reason my case is failing, is because I do not have the mesh interface figured out properly.
so I would like to ask you a few questions starting with the geometry
summary of geometry:
2" pipe, length 2m, inclined at 30deg, with brine inlet at the bottom and mixture outlet at the top.
near the bottom, I have a 1/2" air inlet and near the top I have a 1/2" salt inlet.
during the simulation, the brine is static, the air travels up towards the mixture outlet and the salt travels down and should collect on the bottom, near the brine inlet. (see image below)
the purpose is to investigate the counterflow behavior of the two phases (air and salt) in the third (brine)
so regarding the geometry:
Should I have 3 bodies and 3 parts? Should I use ShareTopo in this case?

or should I have one part and three bodies? with no SharedTopo in this case?

[KR]

Hi Unless you have any moving or rotating parts in your simulation (performing MRF or moving mesh analysis), I'd perform a share topology on the geometry.
Karthik

[nisimshushan]

Thanks Karthik There are no moving/rotating parts in my model.
So considering the mesh interface which needs to be sorted later, you think that 3 parts, 3 bodies, and SharedTopo is the right way to go for this multiphase case?

[nisimshushan]

ok, so assuming the geometry with 3 Bodies, P parts and SharedTopo is the way to go
I would like to clarify something about my Mesh.
For the air inlet at the bottom and the salt inlet at the top, feeding into the main pipe, do I need to insert a Connections -> Contacts -> Contact Region for each one?
or do I need to create a Mesh Edit -> Contact Match Group -> Contact Match for each one?
Or both?
------------------------------
Another question about the Mesh.
In the case of 1 part 3 bodies, the mesh of all the bodies matched up nicely, but using 3 parts 3 bodies, the mesh doesn't allign.
How do I make the mesh of the main pipe and the small inlet pipes match up in the 3 parts 3 bodies case?

[KR]

Hello Regarding both your questions, I think is key is in share topology. If the share topology gets applied properly on this geometry, then you will not have any mesh connections. Also, you will see a conformal mesh between all your bodies (you will have one to one connections in your mesh).
Have you applied share topology on this yet?
Karthik

[nisimshushan]

In the version with 3 bodies and 3 parts, I have activated ShareTopo
But then to get a nice structured mesh I need to use "slice" in geometry and then "Edge Sizing & multi-zone" in Mesh
Does the "slice" affect the ShareTopo?
Should I have done auto-detect for the contact regions? or should I delete them?

[nisimshushan]

In another version I am trying, I have combined all the pipes into 1 body 1 part
So I sacrifice the structured mesh, in order to remove the complexity of the interfaces later in the setup.


The case runs fine on my PC
But once again, when I try to upload to HPC, I get the two persistent errors
The first error I don't understand at all!
The second is also a mystery since my script looks fine for the dual-time-iterate command!

[nisimshushan]

I have started again with a simpler geometry.
But my mesh has some inconsistencies.
I think that I have selected things correctly, so I don't understand why I am getting this error.
How do I resolve this kind of problem?
Will this affect my solution?

[Rob]

It's worked so I'd not worry too much. Check how the blocking aligns with any edge nodes as that may trigger a warning.

[nisimshushan]

OK, so i used another version of my Mesh and now I am not getting that error anymore.
Skipping forward, I have managed to get my case to run on HPC.
However, when I try to add a 'report' to my case, I get those persistent errors from earlier.
So to generate a report for Static Pressure for example I am doing the following:
then HPC gives me this error message

plus the persistent error messages from earlier.
And the case does not run
------------------------------------------------------------------------------
Is there another way to set the report? Maybe there is a script I could add to my txt file to generate the report?

Thanks for your help
Nisim

[Rob]

Turn off the "Plot" option and see what happens.

[nisimshushan]

Rob, you are a genius!
I turned off "Report Plot" and "Print to Console" and it is running!
Thank you very much

[Rob]

Thanks, I may link my boss on this one! :)
That suggests there's something odd with the graphics on the HPC. Make sure you save case and data before trying any post processing.

[nisimshushan]

Hi again I have a few contours that i am looking at (they are all marked as valid and work properly)
And for some of those i have created animations.
However, no file is saved for the animation.
Could this be linked to the "Storage Directory" being greyed-out?
I have tried switching the "Storage Type" to AVI, JPEG etc' - but it doesn't make any difference.
What have i done wrong?
Thank you
Nisim

[Rob]

It should store the files in the working directory. Given plots aren't working, but contours are there's something odd with either the case or the graphics. I tend to save many contour plots and then create animations externally, it's a habit formed as I've used Fluent longer than the animations have been available.

[nisimshushan]

Hi again I may have found the reason that HPC is not generating the animations i need.
A few months ago, when i reinstalled ansys on a new HD, Ansys asked if i wanted the Pro, Premium Or Enterprise version.
I believe that i kept default as Pro version.
Now i understand that this version offers reduced functionality including when using HPC.
I have been reading through the Ansys Capability Chart 2021 R1
How do i check if i have the Pro or other Version?
How do i change the version?

[Rob]

Not sure, Pro reduces what the solver can do, but gpu support isn't linked to the display it's whether you can use the gpu to accelerate the solver.

[nisimshushan]

It also affects my Cell Zone Condition options
I am trying to fill my inlets with different phases (air and salt) than the main pipe (brine)
But the option is not available on the pro version
I think ill try to uninstall Ansys and reinstall selecting Premium version

[Rob]

You do lose access to some of the solver functions, including the more complex turbulence models. That will explain the transitional error you see - that's one of them. But that should prevent the model running rather than stopping images being saved.
The level used is set by the licence server, not the install so it's more a question of what is set in your licence. will know what to look for.

[ANSYS_MMadore]

When launching FLUENT there is a dropdown in the launcher to select which level of licensing to run. If you only have Pro, you won't be able to run with any other level. You can look at your license file and see which cfd_solve_levelX licenses you have. Pro=level1, Premium=level2, Enterprise=level3.

[nisimshushan]

When i right click on Setup from workbench, a 'settings' window opens instead
Is there a workaround?

[ANSYS_MMadore]

As this is ANSYS Student this would be a limitation on the license. Could you confirm?

[Vishal Ganore]

Ansys Student version is limited to 4 cores of the HPC license.

[nisimshushan]

But can I change a student license to "Premium" instead of "Pro" to access the additional functions?

[nisimshushan]

So i can run Fluent directly off our University Server and then I get the option to choose Pro, Premium or Enterprise.
My question is, if I setup the case on the server, with the extra features and then export the case and data files Will I then be able to load them on my home desktop student version and continue to run the solution or adjust the case?

[Rob]

Student is a node and core limited licence for Fluent. Otherwise it's pretty much full functionality so it should read back onto the home machine. From a licencing point of view you do need to be careful, and the terms you signed off are available here https://www.ansys.com/academic/terms-and-conditions

[nisimshushan]

Thanks, Rob No worries, as the 50-mile access radius from the institute covers the whole of Singapore.
Still no luck getting the university HPC to produce animations.
Also, accessing Fluent via the VPN did not make the missing features available i.e. assign secondary phase to a body from the Cell Zone window, which is a big surprise.

[Rob]

You don't assign a secondary phase to a cell zone via Cell Zone. You'd assign a fluid or mixture (for multiphase). If you want to patch a volume fraction you want the Patch function in Initialisation. Multiphase isn't in CFD Pro so you won't see it.

[nisimshushan]

I tried using patch but it doesnt save the selection.
I click on patch and nothing changes in the case.

[nisimshushan]

Hold on a minute, when I untick the "volume fraction patch options" - then it works!
Fantastic!

[Rob]

In the second image you've set a different phase. If the initial condition was all air nothing will change. You then patch "salt" into the salt region which will overwrite the air that's present. Initialise again and plot a contour of air and one of salt.

[nisimshushan]

The inclined pipe is full of static brine.
Then I set salt in the top inlet (will flow down the pipe) and air in the bottom inlet (will flow up the pipe)
My aim is to look at the hydrodynamics in the mid-pipe region when they counterflow.
I have set the salt as a high-density viscous fluid with the granular option activated and added salt particle injection to monitor additional behavior.
I am not sure if that is the right way to model a salt flowing. How would you model the salt? Or even sand for example?

[gmteke]

Hello
Please did we understand the meaning of this warning?

Warning: the rp-transition-model option is not available in this solver

[gmteke]

Hello
Please did we understand the meaning of this warning?
Warning: the rp-transition-model option is not available in this solver

[nisimshushan]

Hi gmteke Sorry i dont remember this particular error, but i can say that once I stopped trying to "write to file" on HPC, then my simulations ran without the errors I used to see

[Rob]

What other models are switched on?

[f_antonelli]

Hi, looking at the warning I think you were just loading the incorrect version of fluent on the HPC. I think you created your model with a version newer than that you used on the HPC. In the submission file you should have a line that looks like this: module load ANSYS/2022R2. Make sure that you are not using an older version on the HPC.