[gyr]

Dear all,

I meet this problem as follows:
ERROR #001100279 has occurred in subroutine ErrAction. Message:Stopped in routine ADDOPE
what is ADDOPE mean or refer to for solving the problem
thanks

[Opaque]

you posted an incomplete error message. More information is required.

[gyr]

thanks for reply.here error message
+--------------------------------------------------------------------+
| Job Information at Start of Run |
+--------------------------------------------------------------------+

Run mode: partitioning run

Host computer: DESKTOP-IBDVA9M (PID:16084)

Job started: Wed Nov 6 21:58:20 2024

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

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


+--------------------------------------------------------------------+
| The following user files have been saved in the directory |
| C:/Users/Ansyscfx/AppData/Local/Temp/WB_Ansyscfx_9220_2/wbnew_pen- |
| ding/dp0_CFX_Solution/CFX_001: |
| |
| trace |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| For CFX runs launched from Workbench, the final locations of |
| directories and files generated may differ from those shown. |
+--------------------------------------------------------------------+


This run of the ANSYS CFX Solver has finished.

[ghorrocks]

It looks like it is failing in the partition step. In that case try different partition algorithms, or allocating more memory to the partitioner. Also try the large problem partitioner.

In other words: don't bother trying to figure out the problem, just try a bunch of options until you find something which works.

Note: CFX error messages are useless. There is nowhere you can look up the numbers for a description of the error. The only thing you can do it try to figure out what the problem is.

[gyr]

thank I ll try

[Opaque]

Originally Posted by gyr

thank I ll try

What are you doing out of the ordinary?

Have you set up several expressions, CEL? Have you used suffixed variables such as Pressure, Gradient X, or the like?

What specific multiphase model have you activated?

[gyr]

im using the Euler–Euler multiphase approach verified by AIAD module implementation.there are more than 70 equations used in the simulation.its about predition of droplet size spectrum of oil&gas flow in 45-inclination pipe to a vessel.

[gyr]

i tried different partition algorithms, and allocating more memory to the partitioner.i still dont know what this error mean

[Opaque]

Originally Posted by gyr

thanks for reply.here error message
+--------------------------------------------------------------------+
| Job Information at Start of Run |
+--------------------------------------------------------------------+

Run mode: partitioning run

Host computer: DESKTOP-IBDVA9M (PID:16084)

Job started: Wed Nov 6 21:58:20 2024

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

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


+--------------------------------------------------------------------+
| The following user files have been saved in the directory |
| C:/Users/Ansyscfx/AppData/Local/Temp/WB_Ansyscfx_9220_2/wbnew_pen- |
| ding/dp0_CFX_Solution/CFX_001: |
| |
| trace |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| For CFX runs launched from Workbench, the final locations of |
| directories and files generated may differ from those shown. |
+--------------------------------------------------------------------+


This run of the ANSYS CFX Solver has finished.

I would contact Ansys CFX support line, and provide your output file and the file named "trace" listed at the end of the message.

[ghorrocks]

there are more than 70 equations

In that case I would do a test case with the same geometry but with the expressions removed, or a least simplified. This is not to get an accurate answer, just to test whether it runs. Then you will know whether your 70 equations are the problem.

i still dont know what this error mean

As I said, there is no way of looking the error up and finding what it means. You just have to do general debugging, usually by trial and error, to get it working.

[gyr]

No expression errors were issued even they contain gradients of velocity and shear.but I doubt about the mesh as it's cfx mesh imported by ansa software.i ll mesh the geometry by ansys mesher and check

[Opaque]

Originally Posted by gyr

No expression errors were issued even they contain gradients of velocity and shear.but I doubt about the mesh as it's cfx mesh imported by ansa software.i ll mesh the geometry by ansys mesher and check

There is a problem with the physics setup. You can run the same physical model using any of the meshes for the tutorials, and it will fail the same way.

Summary: it is not the mesh.

[gyr]

remeshing didn't solve the problem as you said opaque
also physics setup checked precisely all are fine.no error in cfx screen.its so difficult to try the study on tutorial cases for similarity consideration.thanks for you all for help.i ll try to implementation with basic AIAD and see what happen

[Gert-Jan]

Do you have periodic boundaries?
If so, can you test if it runs after replacing these with something else? E.g. Symmetry.

[gyr]

Originally Posted by Gert-Jan

Do you have periodic boundaries?
If so, can you test if it runs after replacing these with something else? E.g. Symmetry.

A good hint.but periodic bc don't reflect the true flow as multiphase behavior but half pipe symmetry to some extent is encouraging

[ghorrocks]

We are not trying to make an accurate simulation, we are just trying to find which bit of your setup is causing the problem. So replace the periodic boundaries with symmetry boundaries and see if it runs. That will tell you if the periodic boundaries is the problem.

Likewise, my suggestion about removing the CEL is also just to see if the CEL is the problem. You can get weird CEL errors at run time which CFX-Pre does not catch. All it will tell you is if the CEL is the cause of the problem or something else.

[gyr]

OK ghorrocks I got it will try all hope solve the problem

[Gert-Jan]

No it will not solve the problem.

Currently we don't know where to look. By changing your system, the output of CFX might change. From this we might learn where and what the problem is.

I was triggerd by the error message. It has the 3 characters PER. My suggestion is that this refers to periodicity. Therefore, make symmetry BC, run the definition file, and see if the message changes.

Furthermore, it would help if you could share some pictures of your case. A picture tells more than 1000 words.

[gyr]

Run with symmetry plane "half pipe" finally went smooth no error.but results didn't reflect expectation.liquid mass flowrate@gas outlet is too small while in actual has excessive carryover with thick smoke.l got droplet size is too large which has more inertia than small one leads to good separation which is not the case.i appreciate everybody posted to help.really I need to simulate the whole pipe but still face the error

[Gert-Jan]

Congratulations. You found where the problem is. Apparently it is at the periodic boundaries. That is already quite something.

Now the problem is either in the mesh, the mutual connection, or specification.
If you want further help, you should share a screendump of the Periodic boundaries in Pre, share the settings, or the output file.
Otherwise, we are looking into the dark. You at least should shed a light.

Please use "Go Advance" to upload files and/or pictures