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

questions about the pathlines generated by Fluent

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

Like Tree5Likes
  • 1 Post By xiang
  • 1 Post By Harrison
  • 1 Post By stuart23
  • 1 Post By kike
  • 1 Post By mmohaqeqf

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 1, 2003, 20:04
Default questions about the pathlines generated by Fluent
  #1
Harrison
Guest
 
Posts: n/a
Dear Sir,

I have a question about the pathline generated by the Fluent. Would you please help me to figure it out?

I am simulating the ventilation system in an animal house. I have two inlets (top ceiling inlet and floor inlet) and one outlet. I assume the flow is incompressible idea gas. No chemical reactions. I use Standard k-e model first and change to RNG model after it begin to converge. The model gives me good results including temperature gradient, ammonia gradient, and air velocity vectors profiles. However, when I use the pathline to show the airflow pattern in the house, I find that all pathlines entering the top ceiling inlet stay at the ceiling and end at the corner. They do not flow down and to the outlet. I check the total mass balance of all inlets and outlet. It is good.

So, I am wondering if this pathline pattern means something special. Or do you have the same situation as me? Does anybody know how fluent define the pathline? How does fluent calculate it? Based on our regular knowledge, the particles entering the inlet should leave through the outlet if there is no sink in the domain. Am I right?

Thank you very much! Harrison
  Reply With Quote

Old   July 1, 2003, 22:58
Default re: questions about the pathlines generated by Fluent
  #2
Alex Munoz
Guest
 
Posts: n/a
Hi

I don't know too much about pathline, I have never used it. However, i sugguest that you use DPM model

See the tutorial for particle tracking basically, create the injections one for each inlet, then the material (your material could be the default antracite). finally, request particle tracking under under display>particle tracking.

Use all the default parameters of DPM except the maximum number of step, which are determined by the distance between the inlet and the outlet and the lenght step that you assing the default 0.01m if you select specify length scale.

For the injection properties just provide a velocity normal to the inlet surface equal to the average velocity of the flow at that surface and the particle diameter 1e-03 or 1e-04m.

Good luck

Alex Munoz

  Reply With Quote

Old   July 2, 2003, 01:38
Default re: questions about the pathlines generated by Fluent
  #3
xiang
Guest
 
Posts: n/a
Dear Harrison,

Are you sure that your setting for the max. number of steps is sufficient so that the calculation of the path lines can be completed? If not, the pathline will terminate somewhere in your domain without reaching the outlet. In this case, the number of incomplete pathlines will be reported in the console window. Of course, since your solution was converged, the mass balance was kept for all your outlet and inlets.

Another way to check the pathline is that your enable "reverse" option in the pathline panel and set the outlet as release surface, then FLUENT will track back the pathline from the outlet to inlet. Hope I am giving you some help without wasting your time. regards, Xiang rongbiao
nhendre likes this.
  Reply With Quote

Old   July 3, 2003, 01:31
Default re: questions about the pathlines generated by Fluent
  #4
Harrison
Guest
 
Posts: n/a
Hi, Alex and Xiang,

Thank you so much.

I believe that I set to the max number of steps. I will try the DMP and reverse model. Thanks again!

Harrison
nhendre likes this.
  Reply With Quote

Old   September 1, 2011, 12:05
Default
  #5
New Member
 
Join Date: Jul 2011
Location: Boston, MA
Posts: 15
Rep Power: 14
kike is on a distinguished road
I think that I have a similar situation to what Harrison had. I have a simulation with one inlet and one outlet and after convergence of all equations to 1e-6 the pathlines are incomplete. The path the particles take though seem to make good sense until they stop without escaping. Thus I think that the problem is merely that more time is needed to finish calculating the pathlines, I decided to continue to iterate disregarding the convergence criteria but it seems it will take a long time before all the pathlines are calculated. If there is a way to reduce the time step for the pathline calculation that would be great, is this only available in unsteady? my simulation is steady.
kike is offline   Reply With Quote

Old   September 1, 2011, 13:22
Default
  #6
Senior Member
 
Stuart Buckingham
Join Date: May 2010
Location: United Kingdom
Posts: 267
Rep Power: 25
stuart23 will become famous soon enoughstuart23 will become famous soon enough
Kike,
You should not need to iterate the solver any more. Try inceasing the step size and number of steps options in the pathline dialogue. Your pathlines are probably just not traced far enough

Stu
nhendre likes this.
stuart23 is offline   Reply With Quote

Old   September 1, 2011, 14:23
Default
  #7
New Member
 
Join Date: Jul 2011
Location: Boston, MA
Posts: 15
Rep Power: 14
kike is on a distinguished road
Stuart, thanks for your response. You are right, after a long time of iterations, the results do not seem to be different. I tried to increase the stepsize as you said (by deactivating the accuracy control) and although this brought more detail, the path lines seem to remain trapped within my geometry. When I Click reverse on the outflow some pathlines are completed and the particles escape, unfortunately not all the particles escape in this option either.
kike is offline   Reply With Quote

Old   September 1, 2011, 15:14
Default
  #8
New Member
 
Join Date: Jul 2011
Location: Boston, MA
Posts: 15
Rep Power: 14
kike is on a distinguished road
As an update, I took the results into CFD-post and the streamlines are displayed through a more complete path, almost half or more go from inlet to outlet, however, there are some still that (although taking the path that seems to make sense) they end up suspended in between.. any suggestions?
nhendre likes this.
kike is offline   Reply With Quote

Old   August 18, 2018, 12:11
Default
  #9
Member
 
Mohammad M F
Join Date: Jan 2016
Location: Washington DC, USA
Posts: 43
Rep Power: 10
mmohaqeqf is on a distinguished road
I know the last post on this thread is like a couple of years old, I just want to mention that I have been dealing with pathline function in Fluent for the last couple of months and it seems that even for a simple geometry like a bend or a gradual expansion, it is super difficult to complete all pathline and you always have some terminated (incomplete) pathline there.
I had no luck so far, and personally think that's the limitation of Fluent pathline generation.
nhendre likes this.
mmohaqeqf is offline   Reply With Quote

Reply

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
looking for a smart interface matlab fluent chary FLUENT 24 June 18, 2021 10:07
The fluent stopped and errors with "Emergency: received SIGHUP signal" yuyuxuan FLUENT 0 December 3, 2013 23:56
few quesions on ANSYS ICEMCFD and FLUENT Prakash.Paudel ANSYS 0 August 12, 2010 13:07
beginner's questions about fluent paralle processing Renold FLUENT 1 May 18, 2009 01:53
Simple fluent questions temp3733@gmail.com FLUENT 0 May 18, 2005 13:50


All times are GMT -4. The time now is 00:02.