CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Errors occur in CFX

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 3, 2020, 07:56
Default Errors occur in CFX
  #1
M29
New Member
 
Sumin Park
Join Date: Jul 2019
Posts: 18
Rep Power: 2
M29 is on a distinguished road
Hello, I encountered some problems in CFX.

I actually simulate spent fuel dry storage by using CFX. I want to see how to occur heat transfer at the heat transfer fin attached outer of dry cask.

So, I made an full model and added outer fin into the dry cask.

In the dry cask, the fluid domain set to helium(ideal) and atmos set to air(ideal). For that, I used Beta Features->turn off "Constant domain Physics".

And I also made "air-exposure space"(now i named it to atmos). Atmos surround dry cask.
So, for atmos boundary conditions, I set "wall" and "no-slip condition" at all faces except for interface face. And used temperature condition for heat transfer option.

Finally I started solver and error ouccurs...

Error and geometry are attached.

For error about isolated fluid regions, I checked geometry and interface but there is no problem..

For error about IO module, I don't know what it's about.

Please give me some advise..
Attached Images
File Type: png whole geometry1.png (6.8 KB, 6 views)
File Type: png whole geometry2.png (6.1 KB, 5 views)
File Type: png whole geometry.png (64.3 KB, 5 views)
File Type: png dry cask.png (72.4 KB, 5 views)
File Type: jpg boundary conditions for atmos.jpg (88.3 KB, 7 views)
M29 is offline   Reply With Quote

Old   February 3, 2020, 07:57
Default
  #2
M29
New Member
 
Sumin Park
Join Date: Jul 2019
Posts: 18
Rep Power: 2
M29 is on a distinguished road
add pictures about errors
Attached Images
File Type: png error1.png (20.2 KB, 7 views)
File Type: png error2.png (21.4 KB, 6 views)
File Type: png error3.png (17.0 KB, 6 views)
File Type: png error4.png (10.9 KB, 6 views)
File Type: png Beta features.png (15.5 KB, 4 views)
M29 is offline   Reply With Quote

Old   February 3, 2020, 17:32
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,061
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Beta features are designed to be used by experienced users who can debug the sometimes strange ans misleading error messages you get when using beta software. So it would probably be better to model this as a multicomponent fluid and then you won't have to use any beta features - and this is a simple model which won't add much to your simulation time.

The errors about setting pressure levels are saying you have to define a somewhere pressure in each fluid region.

The errors about reading the file suggest some files have been corrupted or deleted. I would regenerate the input files and run it again.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 3, 2020, 21:14
Default
  #4
M29
New Member
 
Sumin Park
Join Date: Jul 2019
Posts: 18
Rep Power: 2
M29 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Beta features are designed to be used by experienced users who can debug the sometimes strange ans misleading error messages you get when using beta software. So it would probably be better to model this as a multicomponent fluid and then you won't have to use any beta features - and this is a simple model which won't add much to your simulation time.

The errors about setting pressure levels are saying you have to define a somewhere pressure in each fluid region.

The errors about reading the file suggest some files have been corrupted or deleted. I would regenerate the input files and run it again.
Then,,how can i set the pressure in each fluid region?? Is it differ to set the reference pressure in fluid domain?

And what's means input files?

Thank you for your help!
M29 is offline   Reply With Quote

Old   February 4, 2020, 00:50
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,061
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
The reference pressure just sets the offset to the pressure variable. By setting the pressure level you have to define a pressure somewhere in the domain. Using a pressure inlet or outlet is the most common way, or it could be by setting the pressure in an initial condition for a transient simulation.

The input files means the def file.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 4, 2020, 01:07
Default
  #6
M29
New Member
 
Sumin Park
Join Date: Jul 2019
Posts: 18
Rep Power: 2
M29 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
The reference pressure just sets the offset to the pressure variable. By setting the pressure level you have to define a pressure somewhere in the domain. Using a pressure inlet or outlet is the most common way, or it could be by setting the pressure in an initial condition for a transient simulation.

The input files means the def file.
I realized that the wall boundary conditions at atmos side and top face is wrong.
So, I will set the "opening boundary conditions" at atmos side and top face. (At atmos bottom face, I will set the wall boundary condition.)

And how can i regenerate the def file for my case???
M29 is offline   Reply With Quote

Old   February 4, 2020, 03:14
Default
  #7
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 1,025
Rep Power: 16
Gert-Jan is on a distinguished road
If you don't have a boundary with a pressure level set (relative to the reference pressure), then you can set the pressure level at a specific position in closed volumes. Look for Solver Control>Advanced Options> Pressure level information
Gert-Jan is offline   Reply With Quote

Old   February 4, 2020, 04:20
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,061
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
You regenerate the def file by updating the simulation setup in CFX-Pre and writing a def file.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 4, 2020, 10:58
Default
  #9
M29
New Member
 
Sumin Park
Join Date: Jul 2019
Posts: 18
Rep Power: 2
M29 is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
If you don't have a boundary with a pressure level set (relative to the reference pressure), then you can set the pressure level at a specific position in closed volumes. Look for Solver Control>Advanced Options> Pressure level information
Thank you for your answer!! but i set the opening conditions instead of wall condition.
After that i solve my problem!
M29 is offline   Reply With Quote

Old   February 4, 2020, 11:00
Default
  #10
M29
New Member
 
Sumin Park
Join Date: Jul 2019
Posts: 18
Rep Power: 2
M29 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
You regenerate the def file by updating the simulation setup in CFX-Pre and writing a def file.
Really thank you!! I clear my problems because of your answers.
M29 is offline   Reply With Quote

Reply

Tags
ansys, cfx & fluent

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[solidMechanics] Support thread for "Solid Mechanics Solvers added to OpenFOAM Extend" bigphil OpenFOAM CC Toolkits for Fluid-Structure Interaction 514 February 27, 2020 06:47
Transient simulation not converging skabilan OpenFOAM Running, Solving & CFD 14 December 17, 2019 00:12
Floating point exception error lpz_michele OpenFOAM Running, Solving & CFD 53 October 19, 2015 03:50
dynamic Mesh is faster than MRF???? sharonyue OpenFOAM Running, Solving & CFD 14 August 26, 2013 08:47
Building OpenFOAM1.7.0 from source ata OpenFOAM Installation 42 May 14, 2012 21:48


All times are GMT -4. The time now is 10:05.