Run abortion due to transient output

AtoHM · April 26, 2019, 03:52

Hey guys,
I am experiencing a strange issue. My simulation is a single-phase water tank with constant inflow. To account for the increasing amount of water inside the tank, I stretch part of the mesh to increase domain volume. The setup works fine, mesh is moving as desired. It runs almost 4 times as fast as a free-surface simulation by the way. The setup includes an additional variable which enters with the inlet mass flow. It is used to determine residence time.
Now I wanted to get a full transient result every half hour (physical time) and set it up accordingly: Option: Standard, File Compression: Default, no residuals or extra output variables, Output Frequency Option: Time Interval of 0.5 [h]
Then the Solver stops right before the first iteration with:

ERROR #001100279 has occurred in subroutine ErrAction.
Message:
c_fpx_handler: Floating point exception: Invalid Operand

There are no other errors or warnings giving anything away. I searched the forum and google for that error and it seems to be mostly related to wrong expression evaluation and basic problems with the simulation setup. In my case however, the simulation runs without any issues and the error is actually caused by choosing transient output. Strangely enough, writing backup files works fine - same settings with a timestep interval. Any ideas?

ghorrocks · April 26, 2019, 07:08

I have seen this before where it runs fine but crashes when you write the results file. If you have any user variables, especially user field variables defined by CEL expressions, then check them carefully that they are defined everywhere, including boundaries, walls and inlets/outlets.

But in your case I suspect the issue is more to do with the moving mesh. Have you tried the "include mesh" option? I would try a few other options on the transient results file as you might find one which will do as a work-around.

AtoHM · April 26, 2019, 08:00

I will check on your first suggestion again.

But I can rule out the moving mesh as source, the run with two-phase and free surface (therefore no moving mesh) had similar issues when writing transient results. I will check the additional variable again and maybe contact cfx support and update this post.

Opaque · April 26, 2019, 11:25

Alternatively, you can reduce the variables written to the results file from Standard to Essential.

That means it only writes what is in memory required to obtain the solution (which has not failed yet). The standard option includes a set of derived quantities such as user-defined variables which may not be well defined everywhere and trigger a floating point exception.

If the Essential file is written successfully, you would have found that one of the derived quantities is the problem.

AtoHM · May 20, 2019, 07:36

Update: I was able to circle in on the actual problem. I used Output Frequency -> Time Interval 10 min. There seems to be a bug in CFX Version 19.0. If we switch to Timestep Interval 600 or so, the solver runs normally.

I didn't think it would matter and switched that option when I tested full/partial transient output. So the problem is not with full output but with the output frequency setup. According to ANSYS support this issue was fixed for the latest version(s).

April 26, 2019, 03:52	Run abortion due to transient output	#1
AtoHM Senior Member M Join Date: Dec 2017 Posts: 703 Rep Power: 13	Hey guys, I am experiencing a strange issue. My simulation is a single-phase water tank with constant inflow. To account for the increasing amount of water inside the tank, I stretch part of the mesh to increase domain volume. The setup works fine, mesh is moving as desired. It runs almost 4 times as fast as a free-surface simulation by the way. The setup includes an additional variable which enters with the inlet mass flow. It is used to determine residence time. Now I wanted to get a full transient result every half hour (physical time) and set it up accordingly: Option: Standard, File Compression: Default, no residuals or extra output variables, Output Frequency Option: Time Interval of 0.5 [h] Then the Solver stops right before the first iteration with: ERROR #001100279 has occurred in subroutine ErrAction. Message: c_fpx_handler: Floating point exception: Invalid Operand There are no other errors or warnings giving anything away. I searched the forum and google for that error and it seems to be mostly related to wrong expression evaluation and basic problems with the simulation setup. In my case however, the simulation runs without any issues and the error is actually caused by choosing transient output. Strangely enough, writing backup files works fine - same settings with a timestep interval. Any ideas?

April 26, 2019, 07:08		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	I have seen this before where it runs fine but crashes when you write the results file. If you have any user variables, especially user field variables defined by CEL expressions, then check them carefully that they are defined everywhere, including boundaries, walls and inlets/outlets. But in your case I suspect the issue is more to do with the moving mesh. Have you tried the "include mesh" option? I would try a few other options on the transient results file as you might find one which will do as a work-around. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[swak4Foam] outputTime in Swak function	immortality	OpenFOAM Community Contributions	20	October 6, 2022 13:08
Transient simulations: how to tell its converged (I've read the FAQ & user guides!)	JuPa	CFX	12	March 27, 2020 18:24
Output transient body forces in text file during analysis	karachun	CFX	2	February 27, 2019 05:31
SU2 basics - displaying output and ending a run	kmiller	SU2	3	August 25, 2018 20:00
Transient run continues from last time (when startover is desired)	bongbang	CFX	2	March 23, 2015 00:05

April 26, 2019, 08:00		#3
AtoHM Senior Member M Join Date: Dec 2017 Posts: 703 Rep Power: 13	I will check on your first suggestion again. But I can rule out the moving mesh as source, the run with two-phase and free surface (therefore no moving mesh) had similar issues when writing transient results. I will check the additional variable again and maybe contact cfx support and update this post.

April 26, 2019, 11:25		#4
Opaque Senior Member Join Date: Jun 2009 Posts: 1,880 Rep Power: 33	Alternatively, you can reduce the variables written to the results file from Standard to Essential. That means it only writes what is in memory required to obtain the solution (which has not failed yet). The standard option includes a set of derived quantities such as user-defined variables which may not be well defined everywhere and trigger a floating point exception. If the Essential file is written successfully, you would have found that one of the derived quantities is the problem.

May 20, 2019, 07:36		#5
AtoHM Senior Member M Join Date: Dec 2017 Posts: 703 Rep Power: 13	Update: I was able to circle in on the actual problem. I used Output Frequency -> Time Interval 10 min. There seems to be a bug in CFX Version 19.0. If we switch to Timestep Interval 600 or so, the solver runs normally. I didn't think it would matter and switched that option when I tested full/partial transient output. So the problem is not with full output but with the output frequency setup. According to ANSYS support this issue was fixed for the latest version(s).