Understanding particle injection and influence of geometry position

  • 87 Views
  • Last Post 24 October 2018
keishlaortiz posted this 22 October 2018

I'm currently using ANSYS to simulate the large arteries of the cardiovascular system, specifically injecting nanoparticles in certain areas to see how many nanoparticles reach a certain area of the cardiovascular system.    However, I'm getting results I don't fully understand. Before running simulations with my model, I created some simplest models to observe the behavior of the nanoparticles. I realized that having 3 pipes (like in a dumbbell topology) with same dimensions (same length and radius), the results of the simulation (i.e., where nanoparticles goes) are different if the pipes are placed at different angles (i.e. horizontal, vertical and/or diagonal).  

 

For example, the dumbbell topology has 3 pipes as I explained above, with 1 inlet and 3 outlets. The pipe of outlet 1 is placed vertically (along -y axis), pipe of outlet 2 is placed diagonally (along -x and -y axis) and pipe of outlet 3 is placed horizontally (along -x axis). I injected 1000 gold nanoparticles with 1e-08m in diameter using the Stokes-Cunningham with Brownian motion model randomly distributed at the inlet surface, assuming laminar flow model. The results for this simulation is that 37.5% of nanoparticles escape through outlet 1, 58.2% through outlet 2 and 0% through outlet 3.     I ran a second simulation, but this time, placing pipe of outlet 2 diagonally along the +x and -y axis and I got these results: 31.9% of nanoparticles escape through outlet 1, 28% escape through outlet 2 and 31.9% escape through outlet 3. My question is why now do I have some nanoparticles escaping from outlet 3 by only changing the angle of pipe of outlet 2? Can someone help me to understand this? Thanks!    

Order By: Standard | Newest | Votes
Kremella posted this 23 October 2018

Hello,

Couple of questions about your model set-up:

  • Are you suggesting that your inlet branches into three different pipes? A picture of your geometry would help greatly here. I picture sometimes conveys what 1000 words cannot.
  • Are the flow rates the same in all your outlets?
  • What type of model are you solving (Unsteady DPM)? Is your geometry 2D or 3D?
  • Do you have any additional physics in your flow (gravity)?
  • What are your boundary conditions? 

Please provide some images to help us understand your question better.

Thank you.

Best Regards,

Karthik

keishlaortiz posted this 23 October 2018

Hi, Karthik

1. Yes, the inlet branches into three different pipes, the images of both geometry are below:

Geometry 1

Geometry 2

2. The outlets are set as pressure outlet with a gauge pressure of 13332 each one.

3. I'm using unsteady DPM and the model is in 3D. I used a time step size of 0.01s and number of time steps is 1000 (i.e., 10s simulation time).

4. I didn't use gravity force for the results I posted above, however, I ran some simulations with same geometries with gravity force towards different directions and the results don't change drastically.

5. For the inlet, I assume a velocity inlet of 0.4 m/s and pressure outlets of 13332 gauge pressure as I mentioned in 2. The wall boundary condition is reflect.

If you need more information let me know.

Thanks!!

abenhadj posted this 23 October 2018

Another flow configuration leads to another flow regime: separation, recirculation bubble and reattachements are affecting your flow. It is more interesting if you report the mass flow rates at inlet and outlets for both configuration by using the Report Functions. 

Best regards,

Amine

  • Liked by
  • keishlaortiz
Kremella posted this 23 October 2018

Hi,

I think Amine is right on the money. I think because of the way your geometry is - you might have different flow rates in your problem. The two geometries have different flow physics. Please confirm if this is the case using the instructions provided by Amine.

Thank you.

Best Regards,

Karthik

keishlaortiz posted this 23 October 2018

Indeed, below are the flow rates for both geometries after simulation. So, for geometry 1 the flow at outlet 3 is positive, while the flow rate of outlet 3 in geometry 2 is negative. So this explains why for geometry 1 there are no particles flowing through outlet 3? Right? Why does this happens then? Thanks!

Geometry 1 flow rates

Geometry 2 flow rates

Kremella posted this 24 October 2018

Hello,

I am not very sure as to which of your three outlet face zones correspond in your geometry. If I were to guess on what is happening in your geometry - either because of flow separation or recirculation zones in geometry 1, the upstream end of your outlet 3 pipe has a slightly lower pressure than the downstream. There is a backflow being generated in that section because of this lowering of upstream pressure. Please plot velocity vector plot and pressure contour plots to understand your results better.

Thank you.

Best Regards,

Karthik

keishlaortiz posted this 24 October 2018

Hi Karthik,

 

Outlet 1 corresponds to the pipe that is placed vertically, outlet 2 corresponds to the pipe placed diagonally and outlet 3 corresponds to the pipe that is placed horizontally. Note that I only changed the position of the pipe placed diagonally (i.e., pipe for outlet 2). Below are the velocity vector and pressure (Dynamic pressure) contour plots for both geometries.

Geometry 1 plots

Geometry 2 plots

Close