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

Streamlines issue

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 18, 2022, 04:59
Question Streamlines issue
  #1
Member
 
Join Date: Dec 2019
Posts: 31
Rep Power: 4
Mohamed911 is on a distinguished road
Hello to all,

I am currently studying an axial pump.
In my studies, I use streamlines as references to calculate the exposure times of the fluid particles. However, out of the total number of streamlines that I have chosen (2000 streamline), only a small amount of them reach the pump outlet (less than 1000 streamlines in some cases less than 30 streamlines).

Do you have any idea how to solve this problem?
Mohamed911 is offline   Reply With Quote

Old   March 18, 2022, 17:56
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,234
Rep Power: 135
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Have a look at the streamline integration parameters in CFD-Post. There are settings for maximum length, maximum time, minimum integration step and other settings which are probably terminating the streamlines early.
__________________
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 20, 2022, 19:30
Default
  #3
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,643
Rep Power: 25
Gert-Jan will become famous soon enough
No matter what streamline I use (based on Velocity or Velocity in Stn Frame), in a pump they hardly ever reach an outlet because they end on a blade or stator.
If you want to evaluate the pump in the way you like, you better add massless particles in your simulation setup (CFX-Pre) and let them bounce off the wall, so you are have a much higher change they'll reach the outlets.

P.S. don't turn on turbulent dispersion
Gert-Jan is offline   Reply With Quote

Old   March 21, 2022, 12:05
Default
  #4
Member
 
Join Date: Dec 2019
Posts: 31
Rep Power: 4
Mohamed911 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Have a look at the streamline integration parameters in CFD-Post. There are settings for maximum length, maximum time, minimum integration step and other settings which are probably terminating the streamlines early.
I tried changing all those limits, but nothing, I always get less than 50 streamlines at the inlet.
Mohamed911 is offline   Reply With Quote

Old   March 21, 2022, 12:17
Default
  #5
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,643
Rep Power: 25
Gert-Jan will become famous soon enough
Did you try "Preview Seed Points"?
In sampling you define how your streamlines should start. If you select equally spaced and give in 100, you should get 100 points equally distributed over the surface, not?

It might help if you choose "Forward and Backward" in Direction.
If you are still unsatisfied, then you could try the mass less particles.
Gert-Jan is offline   Reply With Quote

Old   March 21, 2022, 17:55
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,234
Rep Power: 135
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
If this is an important property for your analysis then you should think about doing it a better way. The massless particle approach suggested by Gert-Jan is one way, but that is also affected by similar integration issues as streamlines (although you can get particles far more accurate than streamlines, so the errors can be reduced to a much larger extent).

But an alternative approach is to use a convecting scalar. Set up a additional variable as a convecting scalar, units of [s], define inlets as having a scalar value of zero, and put a source term on the entire domain of 1 [s^-1]. This will generate a new variable which will have the "age" of the fluid in every point of the flow. This approach does not require its own integration step and so avoids all those errors and is calculated on the same mesh as the CFD, so is as accurate as your simulation. It also gives you the fluid age in all locations in the flow - even locations it is very hard to get particles into.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   August 23, 2022, 16:32
Default
  #7
New Member
 
Scott
Join Date: Aug 2011
Posts: 4
Rep Power: 13
polakse is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
...
But an alternative approach is to use a convecting scalar. Set up a additional variable as a convecting scalar, units of [s], define inlets as having a scalar value of zero, and put a source term on the entire domain of 1 [s^-1]. This will generate a new variable which will have the "age" of the fluid in every point of the flow...
Sorry to revive this older thread, but I'm working on something similar and I have a couple questions...
  1. shouldn't the units for the source term be [s s^-1] since the source term in a transport equation is equivalent to the time derivative of the scalar quantity?
  2. I added an additional variable, scalar quantity tR, units [s], with the option "transport equation" in the Fluid Models tab of the domain. Then, I added a subdomain to the fluid domain so I can assign a source term to this variable. In the subdomain, Sources tab, I select the variable tR and the "Source" units default to [kg m^-3]. I tried clicking the expression button and entering 1 [s s^-1]. CFX accepted this without error or warning. However, when I come back into the model setup, it has reverted back to 1 [kg m^-3].
  3. Using this method, I solve the model (SS) and achieve reasonable convergence, but when I plot the results of tR, the value is in the 10^3 range. A simple calculation reveals that tR should be in the 10^-1 range. Indeed, if I plot "time on streamline," the values all look appropriate (~10^-1). The velocities and temperatures solve for by the model all seem reasonable and match calculations and experiment data. Such a huge disparity in residence time is strange. Could this be an issue with the source term units?
  4. For what it's worth, I'm eventually looking to calculate a distribution of residence time for the fluid leaving the domain (i.e. plotted on the outlet face)
Thanks in advance!
polakse is offline   Reply With Quote

Reply

Tags
cfx, pumps, streamlines break

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
[General] Streamlines from VTK files Zerleccoia ParaView 0 May 5, 2016 13:16
Streamlines and AMI patches johannesk OpenFOAM Post-Processing 5 March 24, 2016 05:13
Streamlines from a surface in fluent KrishnaSandeep FLUENT 0 January 25, 2015 20:37
Interpreting streamlines of a rotating fan. danbence Visualization & Post-Processing 1 April 8, 2014 11:13
[General] Problems with streamlines for 2D porous media flow simulations twophaseflow ParaView 4 February 11, 2014 15:32


All times are GMT -4. The time now is 01:54.