CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Error exporting results (http://www.cfd-online.com/Forums/cfx/77796-error-exporting-results.html)

pawan1989 July 4, 2010 14:08

Error exporting results
 
Hey guys, just recently started using CFX after a couple years of using fluent.

I am having a few "minor" problems, and I say minor because I think as far as the physics goes, my results look ok. I am able to run a transient analysis for however-many time-steps I want. However here are some of the problems I am running into, some important, some just annoying:


1) The solution always ends in an error. Always. For one it says something about my Reynolds number being outside the range expected based blah blah blah - this I read up was only a warning because I am trying to model a real turbulent flow as a laminar model. But you know the residuals converge, the mass flow converges and its all good.
After that it just says error has occurred in cfxsolve: The ANSYS CFX solver has terminated without writing results file.

2) I have backed up .trn files and .bak files at appropriate intervals. Now I go to export results and it fails, tells me "unable to initialize API: file has invalid topology

This is a problem because I need it exported to post-process later.

3) When I try to start another run using the results of my .trn file from the succcessful run as an initial condition, it doesn't work, tells me it cannot impose mesh (or something similar, i don't have the exact words as of the moment).

So.. yeah, I Feel like I am missing something small and stupid but I am stuck regardless.
I am not doing any mesh adaptation or anything like that. Just a simple transient analysis of a globally hypersonic flow problem.

Any help appreciated. Thank you :)

ghorrocks July 4, 2010 18:49

1) The Reynolds number warning is simply saying you are using a laminar model for a flow which is probably turbulent. It is a warning only so can be ignored (at your own risk! Make sure you know you can ignore it before doing so!)

The failing to write the results file is a problem heard often in the forum. I am not totally sure where it comes from, but I suspect running CFX in workbench is part of it. Have you tried running CFX outside of workbench?

2) Sounds like a workbench problem.

3) Sounds like the trn file does not include the mesh. You can't use that trn file as a restart file then. Make sure files you want to restart from include the mesh (in the output tab on CFX-Pre)

pawan1989 July 4, 2010 19:17

Thanks ghorrocks :) Appreciate your response.

I am not running cfx as part of the ansys workbench. I am running it independently, just the cfx5 solver which has the options to turbogrid, cfx-pre, cfx solver manager, and cfx post.

The "write geometry" might be what's missing, I might just have to run it with that. I shall try that, thank you :)

Another thing, just out of curiosity. My mesh, half a million cells, 128 time steps transient, took around 6-8 hours on fluent. My mesh, a million cells, 80 time steps takes 36 hours on cfx. Only reason I am using cfx is because there's no grid-size limitation like fluent (with the new license, fluent is limited to 512000 cells).
I think its absurd. Anything I am doing particulary wrong? I used explicit time stepping on fluent but I don't think cfx has an explicit time stepping method does it?

I am just trying to ignore it and just wait out 36 hours for 80 time steps. And its annoying when at the end of 36 hours i realize i forgot to do smoething silly or it won't write my results.

ghorrocks July 4, 2010 20:05

CFX is fully implicit, and has no explicit options. For some classes of flows this is not a good thing - you may have found one. To make use of the implicit nature of the solver you should run second order time differencing and as large timesteps as allowable temporal discretisation error allows. Don't use the same timesteps as fluent.

pawan1989 July 5, 2010 12:42

exporting the mesh fixes all my problems. well, it fixes being able to export a cgns file :)

my run hasn't terminated yet so I don't know if it comes to a good end or still gives me an error when ending.

As far as finding the largest allowable time step.. hmm I don't exactly know what to do for that. Right now I have it set such a way that there are 40 measurements from the fluid particle's start at the inlet to the finish at the outlet. Won't increasing the timestep have a bad impact on my solution?

Thanks for all the help :)

ghorrocks July 5, 2010 19:03

Quote:

As far as finding the largest allowable time step.. hmm I don't exactly know what to do for that.
Simply do a sensitivity study. Vary the timestep size and find which time step size gives you an acceptable compromise between solution accuracy and run time time. This is basic stuff which you should do for every new simulation.


All times are GMT -4. The time now is 14:44.