How to recover an unfinished solver run?

altomos · September 1, 2011, 01:39

Hello expertens,

Does anyone how to recover an unfinished CFX solver run?

When my transient simulation is running in Solver, it's suddenly stopped due to my computer's HDD free space.

The I really one either:

- To continue the run after freeing up more space, or

- To generate a .res file with all finished trn results files.

Here I attached an image, please help me, this is very important for me,

Thank you a lot!

ghorrocks · September 1, 2011, 03:01

It looks like you were saving full transient results files. You will have to go to the last successfully saved full transient results file. You will be able to recover all results up to that point from there, but anything after that will be lost.

altomos · September 1, 2011, 03:23

Quote:

Originally Posted by ghorrocks

It looks like you were saving full transient results files. You will have to go to the last successfully saved full transient results file. You will be able to recover all results up to that point from there, but anything after that will be lost.

Thank you a lot, Mr. Ghorrocks!

I did as you said and luckily, I recovered my simulation result.

Thanks a lot, this is very nice!!!

brunoc · September 1, 2011, 13:37

Hi altomos,

The fact is you shouldn't be saving full transient files. That is equivalent of saving full result files everytime and is probably not what you're looking for. Besides it is both to disk space and time consuming. Instead, try changing you transient result file option to 'Selected Variables' and save only the variables you're interested in. You'll save plenty of space doing that.

Cheers

altomos · September 1, 2011, 15:01

Quote:

Originally Posted by brunoc

Hi altomos,

The fact is you shouldn't be saving full transient files. That is equivalent of saving full result files everytime and is probably not what you're looking for. Besides it is both to disk space and time consuming. Instead, try changing you transient result file option to 'Selected Variables' and save only the variables you're interested in. You'll save plenty of space doing that.

Cheers

One more useful advice, thank you a lot, Mr. Brunoc!

ghorrocks · September 1, 2011, 22:48

Quote:

The fact is you shouldn't be saving full transient files.

I do not agree. If you have the space then why not save everything and delete it if it is not needed? I save full results files all the time. When you are setting up or debugging a simulation this is extremely useful.

Once a run is set up and going well then it makes sense to cut the results file back down only to what is needed. But blanket statements saying you should not save full files are not correct.

brunoc · September 1, 2011, 23:20

Hi Glenn,

Sorry, but it's not a blanket statement. A CFX results file is filled with dozens (sometimes hundreds) of different 3D fields that are important during the solver calculation. But I find it hard to believe that an engineer will need to analyze every single one of these fields in order to draw conclusions. Saving only the variables you're interested in do save time and disk space.

In my opinion, even for debugging saving the full results is a bad procedure, since CFX will save some (or lots of?) complete 3D fields of unneeded stuff. For instance, saving the mesh every timestep on a fixed domain simulation is a true waste of space. Same goes for material properties for fluids with constant properties. The list could go on.

Last, it's amazing how many people run long simulations without a clue of what to look for (not your case, of course). Saving only some variable forces the user into thinking what he wants from the simulation from the beginning.

So yes, I maintain my idea that users shouldn't generally save full transient files.

Cheers.

ghorrocks · September 1, 2011, 23:37

Quote:

A CFX results file is filled with dozens (sometimes hundreds) of different 3D fields

Yes, and those fields allow for smoother restarts (or restarts at all in some circumstances). I do not analyse them.

If you do not save the mesh in the results file and the run crashes you will not be able to recover anything. You need the mesh in final results file to read the intermediate ones.

And as I previously said, if the run completes OK and they are not needed then you just delete them. But if you need them they come in very handy.

If you save lots of full results files and don't delete the ones you don't need and don't use reduced results files where suitable then yes, you will fill your hard drive pretty quickly.

brunoc · September 1, 2011, 23:52

I think we're talking about different things. I was talking about transient intermediate files, which I don't believe should be saved with full results settings. I agree you might need complete results for restarts, but that's why CFX has backup files (and different tabs and settings for transient, backup and results files). Saving full backup files is obviously a good practice, and full result files needs no comments.

ghorrocks · September 2, 2011, 02:20

No, we are talking about the same thing.

Previous releases of CFX had problems with backup results files in transient runs. I think it was fixed way back in V5, but since then I had never used backup files in transient runs. I understand that bug is fixed now and they work fine, but I am set in my ways

I commonly setup two sets of results files in a transient run, a minimum set of results files with the variables I always use (velocity, pressure, temperature) at a time interal suitable for later animations, and a second set of results files which are a full results file simply to act as a backup in case the run crashes or the computer goes down.

Mina_Shahi · September 3, 2011, 16:07

Dear CFX users

I am running a transient file in Workbench ansys. when i stop simulation and then continue that, it seems that in the time step that i stoped solving and then contine there is a jump in MONITOR FILES, which i don't know why it happens. it looks that just in this point it goes by a line to the first time and then continues.

Does anybody have the same experience?

ghorrocks · September 3, 2011, 21:20

Can you post an image of what you are seeing?

Mina_Shahi · September 4, 2011, 05:55

Unfortunately not

because every time it happened i reran it from the first time step.

Mina_Shahi · September 7, 2011, 17:32

this is the image you asked 1.jpg

Mina_Shahi · September 7, 2011, 19:39

I also got this note:

| The CFX results that are being used to initialise this |
| simulation were generated at a time value that is inconsistent |
| with the Coupling Initial Time value set in the CFX Input File. |
| Please review results carefully. |
| CFX results time : 5.2400E-02 |
| Coupling Initial Time : 0.0000E+00 |

i am solving a fluid structure interaction problem and after this notice i have jump in my result , can you please some body help me?

brunoc · September 7, 2011, 23:21

Hi Mina,

What's happening is that CFX is not restarting your simulation with the correct initial time. Start checking the 'Simulation Type' definition of your simulation. You probably have an error like that on the ANSYS side as well.

Restarting FSI simulations is not straighforward. You will need to set extra MFX commands on your ANSYS input file. Take a look at both ANSYS and CFX documentation. They have a section regarding what you'll need to do.

Cheers

Mina_Shahi · September 8, 2011, 05:32

Thanks for you reply

Yes when i restart the run apparently initial time in Ansys goes to Zero while in CFx it is Ok and sets according to previous simulation time, and i don't know how to manage it

lingdeer · December 21, 2011, 22:24

I have the exactly same problem as you Mina_Shahi. Happy and sad at the same time! :P
Anyone know the solution to this?
I tried to change the restart time step on ANSYS but it kept on restarting from 0.

Also, since the .rdb is written the beginning of the run and never get updated later, would that be a problem? (I have all the .Rnnn files though).

Thanks in advance!!!

Quote:

Originally Posted by Mina_Shahi

Thanks for you reply

Yes when i restart the run apparently initial time in Ansys goes to Zero while in CFx it is Ok and sets according to previous simulation time, and i don't know how to manage it

brunoc · December 22, 2011, 08:04

Elaine and Mina,

Restarting an FSI run that did not come to a clean stop is not straighforward and has its requirements, the most important (and obvious one) being that there needs to be a backup file from both CFX and ANSYS at the same timestep. You might also need to play with some APDL restart commands.

Just follow the instructions from the documentation (section 2.6.7 on the CFX help) and you should be good to go.

Cheers

lingdeer · December 22, 2011, 12:37

Thanks Brunoc.

I tried that but still the ANSYS restart from step 0.
Even though I added: (Let's say the timestep is stopped is at the middle of 188, my time step size is 0.01 so it's the 1.87s)

MFRSTART, 187, MULT

and

ANTYPE,4,RESTART,187,,CONTINUE

I have two rnnn files, that get overwritten every two time steps.
So I have .r001 and .r002
Which .r001 is the step which 187 is written
and .r002 is the step which 188 is written but this time step is not finished.

I tried to rename to .r187, but still, ANSYS still show an error that it cannot find the rnnn file of the time step specified.

If I use -1 in MFRSTART, it will start with the 0th coupling step.
Did I do anything wrong?

Also, the rdb is not updated everytime step and is only written at the beginning of the run. Would that be a problem?

September 1, 2011, 01:39	How to recover an unfinished solver run?	#1
altomos New Member Hoang Anh Dung Join Date: Jul 2010 Location: Korea Posts: 19 Rep Power: 16	Hello expertens, Does anyone how to recover an unfinished CFX solver run? When my transient simulation is running in Solver, it's suddenly stopped due to my computer's HDD free space. The I really one either: - To continue the run after freeing up more space, or - To generate a .res file with all finished trn results files. Here I attached an image, please help me, this is very important for me, Thank you a lot!

September 1, 2011, 03:01		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	It looks like you were saving full transient results files. You will have to go to the last successfully saved full transient results file. You will be able to recover all results up to that point from there, but anything after that will be lost. altomos likes this.

September 1, 2011, 13:37		#4
brunoc Senior Member Bruno Join Date: Mar 2009 Location: Brazil Posts: 277 Rep Power: 21	Hi altomos, The fact is you shouldn't be saving full transient files. That is equivalent of saving full result files everytime and is probably not what you're looking for. Besides it is both to disk space and time consuming. Instead, try changing you transient result file option to 'Selected Variables' and save only the variables you're interested in. You'll save plenty of space doing that. Cheers altomos likes this.

September 3, 2011, 16:07	problem in Transient simulation	#11
Mina_Shahi Member Mina Join Date: Apr 2011 Posts: 88 Rep Power: 15	Dear CFX users I am running a transient file in Workbench ansys. when i stop simulation and then continue that, it seems that in the time step that i stoped solving and then contine there is a jump in MONITOR FILES, which i don't know why it happens. it looks that just in this point it goes by a line to the first time and then continues. Does anybody have the same experience?

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
different results between serial solver and parallel solver	wlt_1985	FLUENT	11	October 12, 2018 09:23
OpenCL linear solver for OpenFoam 1.7 (alpha) will come out very soon	qinmaple	OpenFOAM Announcements from Other Sources	4	August 10, 2012 12:00
Symmetry plane error in solver	Santiago Orrego.	CFX	6	January 31, 2007 08:09
Help, can't stop solver run...Windows OS	ben akih	CFX	2	November 13, 2006 11:05
Convergence with coupled implicit solver	Henrik Ström	FLUENT	1	October 29, 2005 04:57

September 1, 2011, 23:20		#7
brunoc Senior Member Bruno Join Date: Mar 2009 Location: Brazil Posts: 277 Rep Power: 21	Hi Glenn, Sorry, but it's not a blanket statement. A CFX results file is filled with dozens (sometimes hundreds) of different 3D fields that are important during the solver calculation. But I find it hard to believe that an engineer will need to analyze every single one of these fields in order to draw conclusions. Saving only the variables you're interested in do save time and disk space. In my opinion, even for debugging saving the full results is a bad procedure, since CFX will save some (or lots of?) complete 3D fields of unneeded stuff. For instance, saving the mesh every timestep on a fixed domain simulation is a true waste of space. Same goes for material properties for fluids with constant properties. The list could go on. Last, it's amazing how many people run long simulations without a clue of what to look for (not your case, of course). Saving only some variable forces the user into thinking what he wants from the simulation from the beginning. So yes, I maintain my idea that users shouldn't generally save full transient files. Cheers.

September 1, 2011, 23:52		#9
brunoc Senior Member Bruno Join Date: Mar 2009 Location: Brazil Posts: 277 Rep Power: 21	I think we're talking about different things. I was talking about transient intermediate files, which I don't believe should be saved with full results settings. I agree you might need complete results for restarts, but that's why CFX has backup files (and different tabs and settings for transient, backup and results files). Saving full backup files is obviously a good practice, and full result files needs no comments.

September 2, 2011, 02:20		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	No, we are talking about the same thing. Previous releases of CFX had problems with backup results files in transient runs. I think it was fixed way back in V5, but since then I had never used backup files in transient runs. I understand that bug is fixed now and they work fine, but I am set in my ways I commonly setup two sets of results files in a transient run, a minimum set of results files with the variables I always use (velocity, pressure, temperature) at a time interal suitable for later animations, and a second set of results files which are a full results file simply to act as a backup in case the run crashes or the computer goes down.

September 3, 2011, 21:20		#12
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	Can you post an image of what you are seeing?

September 4, 2011, 05:55		#13
Mina_Shahi Member Mina Join Date: Apr 2011 Posts: 88 Rep Power: 15	Unfortunately not because every time it happened i reran it from the first time step.

September 7, 2011, 17:32		#14
Mina_Shahi Member Mina Join Date: Apr 2011 Posts: 88 Rep Power: 15	this is the image you asked 1.jpg

September 7, 2011, 19:39		#15
Mina_Shahi Member Mina Join Date: Apr 2011 Posts: 88 Rep Power: 15	I also got this note: \| The CFX results that are being used to initialise this \| \| simulation were generated at a time value that is inconsistent \| \| with the Coupling Initial Time value set in the CFX Input File. \| \| Please review results carefully. \| \| CFX results time : 5.2400E-02 \| \| Coupling Initial Time : 0.0000E+00 \| i am solving a fluid structure interaction problem and after this notice i have jump in my result , can you please some body help me?

September 7, 2011, 23:21		#16
brunoc Senior Member Bruno Join Date: Mar 2009 Location: Brazil Posts: 277 Rep Power: 21	Hi Mina, What's happening is that CFX is not restarting your simulation with the correct initial time. Start checking the 'Simulation Type' definition of your simulation. You probably have an error like that on the ANSYS side as well. Restarting FSI simulations is not straighforward. You will need to set extra MFX commands on your ANSYS input file. Take a look at both ANSYS and CFX documentation. They have a section regarding what you'll need to do. Cheers

September 8, 2011, 05:32		#17
Mina_Shahi Member Mina Join Date: Apr 2011 Posts: 88 Rep Power: 15	Thanks for you reply Yes when i restart the run apparently initial time in Ansys goes to Zero while in CFx it is Ok and sets according to previous simulation time, and i don't know how to manage it

December 22, 2011, 08:04		#19
brunoc Senior Member Bruno Join Date: Mar 2009 Location: Brazil Posts: 277 Rep Power: 21	Elaine and Mina, Restarting an FSI run that did not come to a clean stop is not straighforward and has its requirements, the most important (and obvious one) being that there needs to be a backup file from both CFX and ANSYS at the same timestep. You might also need to play with some APDL restart commands. Just follow the instructions from the documentation (section 2.6.7 on the CFX help) and you should be good to go. Cheers

December 22, 2011, 12:37		#20
lingdeer Member Lingdeer Join Date: Jul 2011 Posts: 49 Rep Power: 15	Thanks Brunoc. I tried that but still the ANSYS restart from step 0. Even though I added: (Let's say the timestep is stopped is at the middle of 188, my time step size is 0.01 so it's the 1.87s) MFRSTART, 187, MULT and ANTYPE,4,RESTART,187,,CONTINUE I have two rnnn files, that get overwritten every two time steps. So I have .r001 and .r002 Which .r001 is the step which 187 is written and .r002 is the step which 188 is written but this time step is not finished. I tried to rename to .r187, but still, ANSYS still show an error that it cannot find the rnnn file of the time step specified. If I use -1 in MFRSTART, it will start with the 0th coupling step. Did I do anything wrong? Also, the rdb is not updated everytime step and is only written at the beginning of the run. Would that be a problem?