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

new variable defination

Register Blogs Community New Posts Updated Threads Search

Like Tree4Likes
  • 2 Post By ghorrocks
  • 1 Post By Gert-Jan
  • 1 Post By Gert-Jan

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 4, 2018, 06:47
Default new variable defination
  #1
New Member
 
Reza
Join Date: Jun 2018
Posts: 5
Rep Power: 8
Reza.sbi is on a distinguished road
I want to define a new variable in cfx , that's Eq is:
HI(%)=(ct^a)(shear stress )^b
this is hemolysis index
c,a,b is constant
t is time
The solution method is steady state
I want to get an hemolysis countor in cfx post .

Can someone help me?
Reza.sbi is offline   Reply With Quote

Old   June 4, 2018, 07:32
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,871
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
This is easy to do, but the only trick is you will need to make the expressions (ct) and (shear stress) unitless before you raise them to a power. You can do this by just dividing by one, with a unit of the inverse of their units.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   June 4, 2018, 08:02
Default
  #3
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,928
Rep Power: 28
Gert-Jan will become famous soon enough
Quote:
Originally Posted by Reza.sbi View Post
I want to define a new variable in cfx , that's Eq is:
HI(%)=(ct^a)(shear stress )^b
this is hemolysis index
c,a,b is constant
t is time
The solution method is steady state
I want to get an hemolysis countor in cfx post .

Can someone help me?



If I read it correctly, your equation is: c*t^a*ShearStress^b.
So you have time to the power of a.
But you mention it is steady state, i.e. time is not a variable. So, that doesn't match. Please clarify.........
Reza.sbi likes this.
Gert-Jan is offline   Reply With Quote

Old   June 5, 2018, 05:17
Default
  #4
New Member
 
Reza
Join Date: Jun 2018
Posts: 5
Rep Power: 8
Reza.sbi is on a distinguished road
Hi
In Navier Stokes
In steady state
iteration step are used instead of time steps.
I would use
*length of time each particle is placed under stress
as time in this equation:
HI(%)=(ct^a)(shear stress )^b
my project is hemolysis estimtion in ventricular assist device( centrifugal pump).
I have obtained the pressure and shear stress counter from cfx
I want to get a hemolysis counter
I think
This equation must be solved simultaneously with the contunity equationbut I do not know what to do?
Reza.sbi is offline   Reply With Quote

Old   June 5, 2018, 05:43
Default
  #5
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,928
Rep Power: 28
Gert-Jan will become famous soon enough
If you open your case in CFD-Post, you can create streamlines. Then you obtain a new variable "Time on Streamline". Since you only want to postprocess this equation, I guess this variable is sufficient for what you need, not?
Reza.sbi likes this.
Gert-Jan is offline   Reply With Quote

Old   June 5, 2018, 12:28
Default
  #6
New Member
 
Reza
Join Date: Jun 2018
Posts: 5
Rep Power: 8
Reza.sbi is on a distinguished road
Yes
Thank you
I have done this
This method is Lagrangian
But I want to run Eulerian
And in this way it is necessary to define the variable before it is run.
in Lagrangian method, We can not get hemolysis counter. we can get Discrete data.
I want to compare two Lagrangian and Eulerian methods.
Reza.sbi is offline   Reply With Quote

Old   June 5, 2018, 19:06
Default
  #7
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,928
Rep Power: 28
Gert-Jan will become famous soon enough
I can't follow your comment completely. Please read it over and rearrange your sentences.

You mentioned: "This equation must be solved simultaneously with the contunity equation". Why? Is the equation used somewhere else?

Nevertheless, streamlines are some kind of Lagrangian, as it ignores Turbulent dispersion. But it is done in the postprocessing, so, you can do everything after the run is done. What's wrong with it? Again: Why must the equation be solved simultaneously with the continuity equation?

To run Eulerian, you have to define a scalar that describes the residence time. This is doable.:
1) define a Additional Variable (volumetric)
2) Create a subdomain that covers your whole domain and set a source for your additional variable equal to 1.
3) Set 0 at the inlet.
4) run the calculation
If you are sure this variable is solved completely (Check the overall balances!!!), you obtain a variable representing time that you can use for your equation. A problem/challenge can be that this scalar is subject to mixing.

A better way could be the use of Lagrangian particles with turbulent dispersion in the solver. Then you get discrete data, where mixing doesn't interfere, and have the possibility to create a residence time distribution. But evaluating your equation can only be done in the postprocessing. Also, there is no guarantee that in every cell a particle will be present, so yous time will be undefined at these locations.

In other words, every method has its pros and cons........
Gert-Jan 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
OpenFoam-1.6-ext Allwmake compilation error - one last barrier Pat84 OpenFOAM Installation 15 July 25, 2012 22:49
emag beta feature: charge density charlotte CFX 4 March 22, 2011 10:14
error in COMSOL:'ERROR:6164 Duplicate Variable' bhushas COMSOL 1 May 30, 2008 05:35
Env variable not set gruber2 OpenFOAM Installation 5 December 30, 2005 05:27
Replace periodic by inlet-outlet pair lego CFX 3 November 5, 2002 21:09


All times are GMT -4. The time now is 03:42.