[Mohamed911]

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?

[ghorrocks]

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.

[Gert-Jan]

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

[Mohamed911]

Originally Posted by ghorrocks

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.

[Gert-Jan]

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.

[ghorrocks]

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.

[polakse]

Originally Posted by ghorrocks

...
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!