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

The stream line passes through the part set as the wall

Register Blogs Community New Posts Updated Threads Search

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 27, 2022, 22:26
Red face The stream line passes through the part set as the wall
  #1
New Member
 
Junyeol
Join Date: Mar 2022
Posts: 18
Rep Power: 4
dhehdxhdaus is on a distinguished road
Hi for all, Sorry in advance for my poor English

I set the shape as shown in the attached image.

Like the attached image shape, I want to see a stream line that deflects when there is an object placed in the flow of the fluid.
Based on the image above, the lower and left parts are inlet and outlet, respectively, and the spherical shape is given as a solid wall, and the flow part is given as fluid water.

At this time, when the output stream line is animated, the dots penetrate the wall and pass as it is.
All connectivity tabs have been deleted.
I'm curious as to what is the universal cause of this situation.
The inlet and outlet are 6mmHg and 0mmHg as total pressure, respectively. Thanks for your help.
Attached Images
File Type: png capture.PNG (62.2 KB, 26 views)
dhehdxhdaus is offline   Reply With Quote

Old   March 28, 2022, 02:12
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Does the object move? Is it in a rotating frame of reference? Is the model transient? All of these things can cause streamlines to terminate at walls.

If not, please upload your output file and an image of the full geometry.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   March 28, 2022, 05:33
Default
  #3
New Member
 
Junyeol
Join Date: Mar 2022
Posts: 18
Rep Power: 4
dhehdxhdaus is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Does the object move? Is it in a rotating frame of reference? Is the model transient? All of these things can cause streamlines to terminate at walls.

If not, please upload your output file and an image of the full geometry.

Thank you for your response. ghorrocks

Object is stationary. The analysis was conducted once as steady and then again as transient.
It seems difficult to disclose all models for company security. I'm sorry I couldn't reveal the model despite you helping me.
dhehdxhdaus is offline   Reply With Quote

Old   March 28, 2022, 06:26
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
If the simulation is transient then streamlines can go into walls.

Also inadequately converged solutions can also have streamlines going into walls.

But unless you give us me specific details about what you have done we will not be able to help you further.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   March 28, 2022, 09:17
Default
  #5
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,903
Rep Power: 28
Gert-Jan will become famous soon enough
You can try to reduce the Step Tolerance.

Btw, is the object an Immersed Solid? Then it might be very hard to get correct streamlines.

Also, better use different postprocessing objects. Streamlines only give a general indication the flow. Better look at contours, vectors, etc.
Gert-Jan is offline   Reply With Quote

Old   March 28, 2022, 21:58
Default thanks for your help, ghorrocks
  #6
New Member
 
Junyeol
Join Date: Mar 2022
Posts: 18
Rep Power: 4
dhehdxhdaus is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
If the simulation is transient then streamlines can go into walls.

Also inadequately converged solutions can also have streamlines going into walls.

But unless you give us me specific details about what you have done we will not be able to help you further.
Not the interpretation attached to the main post, but I made a model with almost the same conditions.

Even in the case of a newly created model, after creating a stream line, when animation is activated, dots pass through the solid.

I think I made a basic mistake, but I don't know why.

I'll attach the second test interpretation I made.
The mesh is extremely large due to capacity issues. If I make the mesh a little tighter, it will look like the shape I tried.


Thanks again for your help
Attached Files
File Type: zip test.zip (181.6 KB, 3 views)
dhehdxhdaus is offline   Reply With Quote

Old   March 28, 2022, 22:10
Default
  #7
New Member
 
Junyeol
Join Date: Mar 2022
Posts: 18
Rep Power: 4
dhehdxhdaus is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
You can try to reduce the Step Tolerance.

Btw, is the object an Immersed Solid? Then it might be very hard to get correct streamlines.

Also, better use different postprocessing objects. Streamlines only give a general indication the flow. Better look at contours, vectors, etc.
yes It immersed. I'll try to reduce the Step Tolerance. thanks for your help.
I left an analysis file similar to the simulation I conducted in the reply above, so if you are okay with it, please check it once.
dhehdxhdaus is offline   Reply With Quote

Old   March 28, 2022, 23:00
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
It is an immersed solid? Then why didn't you say so.....

In that case look at the immersed solid parameter momentum source scaling factor. It will need to be increased to stop significant flow from going through the body. The default is 10, try 100 and see how that works. For a small body you might need to increase it quite a bit.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   March 29, 2022, 00:29
Default
  #9
New Member
 
Junyeol
Join Date: Mar 2022
Posts: 18
Rep Power: 4
dhehdxhdaus is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
It is an immersed solid? Then why didn't you say so.....

In that case look at the immersed solid parameter momentum source scaling factor. It will need to be increased to stop significant flow from going through the body. The default is 10, try 100 and see how that works. For a small body you might need to increase it quite a bit.
I'm sorry if I did something stupid. I just wanted to say that the solid shape is sinking into the liquid.

https://www.youtube.com/watch?v=1H1UlQ-ebmY&t=561s

I watched the video above and followed it, but in the video above, it went well with the solid domain. I don't know what the difference is between immersed solid and solid domain.

I followed what you said and the result was much closer to what I was hoping for.

It's been a really big help. Thank you again!
dhehdxhdaus is offline   Reply With Quote

Old   March 29, 2022, 00:48
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I recommend you read the documentation so you understand immersed solids. They are treated fundamentally differently to solid domains, and have their own issues you need to be aware of. The momentum source factor is the most fundamental and important factor in an immersed solids simulation, so you need to know what it means and how to control it.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Reply


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
decomposePar problem: Cell 0contains face labels out of range vaina74 OpenFOAM Pre-Processing 37 July 20, 2020 06:38
Natural convection in a closed domain STILL NEEDING help! Yr0gErG FLUENT 4 December 2, 2019 01:04
problem during mpi in server: expected Scalar, found on line 0 the word 'nan' muth OpenFOAM Running, Solving & CFD 3 August 27, 2018 05:18
Ansys Licence Serve on Ubuntu 16.04 LTS david.pasquale ANSYS 2 January 20, 2017 12:52
error while compiling the USER Sub routine CFD user CFX 3 November 25, 2002 16:16


All times are GMT -4. The time now is 19:06.