[evcelica]

Greetings,
Just wondering if anyone has experienced this error before? It is a partitioning error, I was thinking perhaps my model is too large for CFX? I have ~50M-100M cells. which shouldn't be a problem I know, but there is probably 20k or more different bodies, which may be the problem. CFX-Pre was extremely slow, so I had to edit the ccl file manually, then import it into CFX Pre.

I'm using the large model partitioner. memory allocation factor 1.4. Should I try a different partitioning method, or is there some other problem.

Any help would be greatly appreciated.

Thanks in advance, error pasted below.


+--------------------------------------------------------------------+
| Job Information at Start of Run |
+--------------------------------------------------------------------+

Run mode: partitioning run

Job started: Fri Jan 22 17:43:47 2016

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| io_gunzip: decompressed too little data: got 400000 bytes, expect- |
| ed 581552 |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| read_compressed_dataarray: decompression failed |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| iocnt: read data failed |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| RedSht: read data failed: what=G/NFCFS where=ZN1 |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

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

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX partitioner exited with return code 1. |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| Warning! |
| |
| After waiting for 60 seconds, 1 solver manager process(es) appear |
| not to have noticed that this run has ended. You may get errors |
| removing some files if they are still open in the solver manager. |
+--------------------------------------------------------------------+


This run of the ANSYS CFX Solver has finished.

[Lance]

Originally Posted by evcelica

[...] there is probably 20k or more different bodies, which may be the problem.

100 million cells should not be a problem, but 20k different bodies?! What on earth (land portion) are you doing? I would test different partitioning methods and also bump up the memory allocation factor. Are you sure you have enough memory?

[ghorrocks]

20k bodies sounds like a good candidate for a reduced order model to me.

[evcelica]

Thanks for the input Lance.
It's only 3 domains, but it is a very complex geometry, so I had to slice it up a lot in order to mesh it well. I wish there were some way to combine the bodies after meshing. I only use ANSYS meshing, not ICEM CFD.
I then used mesh transformation in CFX-Pre to repeat part of the mesh 19 times. It takes 35GB of space just to have it open in CFX-Pre.
My computer has 64GB of RAM, and I'm distributing to 5 identical computers, but It doesn't look like it got to the distributing part yet. I'll try a different partitioning method, bump up the allocation factors more, and watch the memory usage in the Task manager to see if it uses it all up.

Glenn, what is a reduced order model?
I'm already using quarter symmetry, and simplified the model as much as feasible while still representing it well enough.

[ghorrocks]

Reduced order modelling: https://en.wikipedia.org/wiki/Model_order_reduction

For instance if you have a pipe with valves, bends and fittings. You could do a 3D simulation of the whole thing. Meshing would be difficult, it would be a huge mesh. Or you could use pipe friction factors and loss coefficients for the fittings and the system reduces down to some simple hand calculations. So a very complex 3D simulation has been reduced to some hand calculations.

Other examples are assuming a 3D flow is 2D or 1D, or even things like porous material models.

[Juniperus]

Hi evcelica!

I am facing the same issue as you did now.
My geometry is also rather big, 85 million elements, but only three bodies in one domain with fluid-fluid interfaces. I am not doing any mesh transformations in CFX-Pre or anything like that.

Did you find a partitioning method that was working out for you? Or did you find any other solution?

I would be very greatfull if you could help me out!
Thanks!

[ghorrocks]

There is the large model partitioner; and also lots of partitioning options which are less memory intensive than the default METIS partitioner. Also you can partition on one very large machine to write the partition file and use that for the solver run so it does not need to partition the mesh.

Have you tried these?

[Juniperus]

I have tried with and without the LMP.
Until now I have only tried MeTiS and the "Optimized R.C.B." until now.
I will continue to try different options.

I also tried to use the same ccl on a small dummy model, just to see if there was any error in the setup. It ran lika a charm.

The memory should not be a problem. I have 128GB on the node used for partitioning.
It seems like it is only using about 7-8GB.

I also tried to remesh it to make a slightly coarser mesh. But that didn't help either.

[evcelica]

I never found a solution, I just went with the 2D "reduced order model" Glenn suggested. I had already done that, and wanted to then do the 3D, but since it had all these problems, I just said the 2D was good enough.
Sorry I couldn't be of any help.

[Juniperus]

Hi!

I have found a possible solution to the problem.
I got a tip from a coworker that the number of surfaces could be the cause of the problem. My geometry consists of 160k+ surfaces. First, I tried to join surfaces by using virtual topology in Ansys Meshing, but it took too long time. So I tried to convert the mesh into msh format (Fluent). And then I manually loaded that into cfx pre. It works like a charm.