How to continue to run previous CFD program using CFX/Solver
 

Dear all,

I don't know why CFX-Solver stopped/crashed the running simulation at 256th step (transient state) after 10 days-running. I want to continue to run it until 600th step. If someone knows it, please tell me in detail.

Many thanks in advance!

If it crashed, theoretically you lost the results right?

If you didn't close the workbench (if you use it), you can open the solver and try to run again using 'current solution'. If the solver don't find the solution to continue, you should look for backups (if you made).

If you don't know where to look the backups, they are in 'name of the project_files/dp0/CFX??/CFX/CFX_00X.dir/XXX.BAK'

If they aren't there, maybe you have a temporary folder for your project, sometimes they are there until you save the project.

.BAK is the type of the backup file.

To use this backup, open the solver again, initial condition, specify initial condition (indicate the .BAK file you want to use).

Hope it helps somehow.

Dear Ismael,
Many thanks for your quick reply!
Although I said "crashed", there are *.trn files until 256th step's trn file in *.dir file. Moreover, Workplace still shows "running".

Where is the option"current solution" in CFX-solver? I can't find it, please tell me detailed position e.g. under "File" or "Edit" etc. I used CFX not Workbench.

I also can't find *.Bak file in involved files, as why I said "crashed". How will I do to continue the simulation until 600th step?

If I find *.bak file, how could I continue this *.bak file after opening CFX-solver? Is it like as follows: File->Define run->select *.bak file in solver input file ->start run?

Many thanks in advance!

PLUS:
How to continue to run *.Bak file, meanwhile, we can change the previous initial conditions in CFX-Pre e.g. change transient time step from 600 to 1000 etc? If you know, Please tell me in detail.

Many thanks in advance!

I have seen this problem often and ditched Workbench after getting nauseous about its messy handling of transient simulations, especially if you are generating trn files frequently.

If you are simulating the standalone, set the directory.

1) Start CFD Solver, it shows you Define Run dialogue box.
2) Select solver input file as 256.trn
3) Select Initial values specification tick and use 256.trn as file name for the initialization file
4) Start the run

You may not see 256.trn if you are not saving the trn file at each timestep.
In that case, select the trn file with largest number.

You may want to ensure that it has chosen right directory to save new trn files, at the bottom.

Dear Oj.bulmer,

Many thanks for your answer. I have another question as follows:
How to continue to run *.Bak file, meanwhile, we can change the previous initial conditions in CFX-Pre e.g. change transient time step from 600 to 1000 etc? If you know, Please tell me in detail.

Many thanks in advance!

I didn't understand your question clearly, yet I would attempt.

To use *.bak file:
I guess you can use the same sequence as in my earlier post. Just instead of trn file, use bak.

To change time step in transient:
YOu dont need to go to CFX Pre to change the time step. You can do it using Tools>>Edit run in progress in Solver manager during the run.

Just make sure you save and close the dialogue box after you do the changes (time step etc)

Watch out so the HD doesn't run out of space.

Dear oj.bulmer,

Many thanks!
I followed your processes to continue running it, i.e. solver input file as 256.trn and using 256.trn file as file name for the initialization values 1's settings. But after "Start Run", it shows


+================================================= ===================+
| ****** PROBLEM REPORT ****** |
|--------------------------------------------------------------------|
| Subsystem: Input and Output |
| Subroutine name: ErrAction |
| Severity level: Fatal Error |
| Error message number: 001100279 |
|--------------------------------------------------------------------|
| Message: |
| |
| REDHDR: locating dataset failed: what=G/NZN where=EVERY |
| |
| |
| |
| |
| |
+================================================= ===================+

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

Do you know what's reasons for this error?

Many thanks in advance!

Hi!
Thanks! But what do you mean? Especially HD?

HD=hard drive

If you save lots of backup files you will fill your hard drive pretty quickly. And if your hard drives fills then the solver cannot write anything to file and the solver will crash.

Haven't heard of it earlier. Is there no other information above or below this error? Often CFX gives hints about where it found hurdles.

Meanwhile, if you are running CFX standalone, check the command prompt window that opens up with CFX standalone, to see a sign of "Out of memory." That is a sign of RAM running out. Also, as Felggv suggests, make sure you have enough space on harddisc. And saving the trn file at every timestep seems overkill, unless you want a fancy animation at the end. I would save trn results by time, typically say 0.5 seconds if my total simulation is lasting for 200 seconds. I can take time average values of last 70 seconds or so. While, even at 0.5 sec, animation is not that bad. But saves a hell of a space.

When I didnt know this, I ended up doing my first transient simulation occupying 173 GB, as I saved trn fiels every timestep!! Now thats ridiculous

The "locating dataset failed: what=G/NZN where=EVERY" occurred when I wanted to use inital value files where no mesh information was included. Meaning: When you define your .bak and .trn files you can restrict the number of Variables written to limit the use f disk space, but if you do not select "include mesh" for trn files or if you select an other option than "standard" for the bak file, CFX will NOT write out any Mesh information and therefore it will not be able to locate the Values of your variables.

same error will appear if you select for the results file smth else than "standard" and forget to check the option "include mesh". In this case you will see the error when trying to Post-Process...and the only way to get rid of it is to rerun the simulation with correct output options :(

As a guideline, you should use backup files (.bak) that export everything every now and then (every 100th iteration, every 30 min, you name it) and also use transient files (.trn) limited to only the variables you want, not exporting the mesh with it. Although trn and bak files function in the same way (and are pretty much interchangeable), they are located in different tabs for a reason.

For detailed information at every timestep from a few quantities, use monitor points.

This is the best way to have all the data you need without getting hit by too much disk space usage.

How to restart simulation in Ansys Fluent?
 

Hi all,
I have the same question but in Ansys Fluent. My simulation had run for 3 days, unfortunately it was stopped for obscure reason, thus I have to re-run it again from the last time step. Any help would be appreciated.

Did you get an error message? Maybe try the Fluent forum - you're posting here in the CFX forum...