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

Filtering Blood Flow

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

Like Tree2Likes
  • 2 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 23, 2021, 23:59
Default Filtering Blood Flow
  #1
New Member
 
Join Date: Apr 2021
Posts: 2
Rep Power: 0
prashn is on a distinguished road
Hi everyone,

I am working on a multiphase filtration problem using ANSYS CFX. The model I have setup utilizes the quarter symmetry of my filter geometry. My main goals with the model is to obtain an axial pressure plot as well as to visualize particle paths/streamlines of the flow.

The CFD model consists of two domains: a fluid domain and a porous domain. The porous domain is our filter media- a .135 mm thick slice between the front and back parts of the filter body. A tetrahedral mesh size of 0.25 mm was used in this region with the mesh growing to 3 mm in the front and back parts of the filter geometry. As mentioned, the simulation is a multiphase one; however, only less that 0.01% of the fluid consists of 20 micron particles that need to be filtered out.

In terms of boundary conditions, an inlet mass flow rate (known as part of my design constraints) and an outlet average static pressure of 100 kPa (based on experimental testing) is specified. Because of the low Reynolds number of the flow, no turbulence model is utilized in this simulation (i.e. laminar flow).

The model runs successfully, however when I am post-processing the results, the streamline plot shows extreme recirculation regions, which is something that has not been observed in our experimental studies with this part.

I have refined the mesh in the region of the filter media as well as verified the boundary conditions with simple hand calculations. To establish a baseline model, I have also forced the outlet boundary condition as a mass flow rate outflow equal in magnitude to the inlet mass flow rate and I have removed the porous domain (i.e. a porosity of 1) but the recirculation still persists. Attached is a copy of the streamline plots and a copy of the out file.

I am unsure as to how else to resolve this seemingly inconsistent physics. Any help or insight is much appreciated! Please let me know if any additional details are necessary.
Attached Images
File Type: jpg No media_streamline.jpg (64.1 KB, 8 views)
File Type: jpg media_streamline.jpg (55.7 KB, 5 views)
Attached Files
File Type: pdf Fluid Flow CFX_001.pdf (138.0 KB, 4 views)
prashn is offline   Reply With Quote

Old   April 24, 2021, 03:46
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,840
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
You have set Minimum Volume Fraction = 0.999997. This means the volume fraction is clipped to this amount, so it can never go lower than that. Is this what you intended? It does not sound right. You probably want to leave this at default which is 1E-15 from memory.

How are you modelling the porous material? And how have you set it up to filter the particles?

Isn't the result you are looking for that the pressure drop occurs across the membrane and nothing much else happens? This does not sound like a very exciting CFD simulation. Why do you think this requires CFD? What are you trying to learn by doing a CFD model?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 24, 2021, 20:38
Default
  #3
New Member
 
Join Date: Apr 2021
Posts: 2
Rep Power: 0
prashn is on a distinguished road
Hello,

Thank you for the quick response. Your point regarding the volume fraction is correct- the 0.999997 figure is the initial volume fraction of the blood relative to the particles mixed within it. I didn't see anywhere else within CFX to specify a number of particles to be entrained in this flow. Is there a better way to introduce particles in my flow rather than defining the blood as a continuous fluid and the particles as a particle transport solid with a specified diameter?

The .135 mm thick disk within my geometry acts as my porous domain. Based on the filter media used in my experimental analysis, a volume porosity of 0.75 based on our media pore size of 20 microns was used (which is the same as the diameter of my particles); I assumed that the porosity of the porous domain was the setup to ensure particle filtration. All other metrics such as permeability, resistance loss coefficient, etc. were left default.

The reason I wanted to pursue CFD in this model was to demonstrate particle paths and the transient buildup of filter cake- two things that my experimental tests cannot show. The CFD will eventually be extended to a parametric analysis which will help inform a more refined design, which is much faster than building prototypes. The model is fairly simplistic in its current stage, but the results I am obtaining with regards to the streamline plot are questionable at best, and I hesitate to make the simulation more complex without addressing this error.

I appreciate your time. Thank you for your help.
prashn is offline   Reply With Quote

Old   April 24, 2021, 21:47
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,840
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Quote:
Your point regarding the volume fraction is correct- the 0.999997 figure is the initial volume fraction of the blood relative to the particles mixed within it. I didn't see anywhere else within CFX to specify a number of particles to be entrained in this flow. Is there a better way to introduce particles in my flow rather than defining the blood as a continuous fluid and the particles as a particle transport solid with a specified diameter?
Sorry to be blunt, but you have failed to understand the basics of multiphase modelling. There are so many red flags in that comment it is hard to list them. You really should do the CFX tutorials on multiphase modelling first so you understand the basics before starting your own work.

Quote:
I assumed that the porosity of the porous domain was the setup to ensure particle filtration.
Wrong, I am sorry. Porous domains do not work like that. They are not used to filter particles, the volume porosity is used to calculate the resistance to flow. The porous domain will have no effect on the particles in CFX (unless you add a custom model).

Quote:
The reason I wanted to pursue CFD in this model was to demonstrate particle paths and the transient buildup of filter cake
Particle paths - yes, CFX can do this. Buildup of stuff on filter - no, CFX cannot do this. Not with the default models anyway.

Quote:
The model is fairly simplistic in its current stage, but the results I am obtaining with regards to the streamline plot are questionable at best, and I hesitate to make the simulation more complex without addressing this error.
Excellent, good to see you are checking the simpler models are correct before going to more complex models. But as I explain, you have some fundamental problems with modelling this simulation in CFX as it lacks some fundamental physics you require (buildup of particles on the filter). Depending on exactly what you are trying to do this might be a show-stopper.
karachun and aero_head like this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 26, 2021, 23:17
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,840
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Regarding using porous domains to filter particles:

Subdomains have an option to set particle absorption properties. See the CFX-Pre Users Guide, section 17.5.1.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Reply

Tags
cfx, filter, multiphase

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
Will the results of steady state solver and transient solver be same? carye OpenFOAM Running, Solving & CFD 9 December 28, 2019 05:21
Blood flow under feverish condition kish CFX 4 April 23, 2013 10:00
Modeling blood flow - FloWorks mcneelyd FloEFD, FloWorks & FloTHERM 2 June 15, 2009 12:53
FLUENT BLOOD FLOW RATE Christoforos FLUENT 0 September 18, 2008 10:08
Inviscid Drag at subsonic, subcritical Mach # Axel Rohde Main CFD Forum 1 November 19, 2001 12:19


All times are GMT -4. The time now is 08:17.