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

Need insight into unexpected CFD results

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 24, 2018, 03:43
Default Need insight into unexpected CFD results
  #1
Member
 
Join Date: Jan 2018
Posts: 82
Rep Power: 5
Stroopwafelandcoffee is on a distinguished road
I'm currently doing a simulation of water flow in a microscopic channel due to a pressure differential. It's meant to simulate a physical lab setup which in turn simulates some biomedical aspect of the human body. The channel is 4mm long, 0.4mm wide and semi-circular like this:





The flow velocities are very low, in the order of 0.0xx m/s. According to my calculations for pipe flow this resulted in very low Reynolds numbers. Because of this I assumed laminar flow. I didn't assume fully developed flow so instead tThere's a velocity inlet, pressure outlet and no-slip stationary walls. I used an initial layer size for the BL of 1e-05mm, resulting in an initial layer size which is between 5e-03 and 1e-04 of the total BL thickness (growth rate 1.1). I had a hard time estimating what my BL should look like for laminar flows, so I'm wondering if this is appropriate. I can upload my mesh and cfx-pre setup if necessary.

I'm getting forces which seem to be of the right order:

Force X: 4.6384e-006 [N]
Force Y: -1.58845e-008 [N]
Force Z: -8.47918e-009 [N]

The wall shear in the X direction also shows expected results:



However, the wall shear in the Y- and Z- direction aren't quite what I expected:




There are some very local but very high spikes visible in the Y- and Z- shear stress, which I can not explain. So I'm wondering what I'm looking at and I'm hoping someone could help me get to the bottom of this. The shear stress vector plot also shows some strange results:




Stroopwafelandcoffee is offline   Reply With Quote

Old   July 24, 2018, 07:00
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,643
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I do a lot of MEMS simulations and am quite familiar with the issues involved. You are correct that your flow is going to be a very low Reynolds number. The implication of this is that there is no boundary layer. The flow will very quickly evolve into a parabolic laminar profile. There is no rapid velocity gradient at the boundary.

The implication of this is that mesh inflation layers and near-wall refinement are totally unnecessary. The gradients are evenly distributed around the flow field, which means the mesh size should be relatively even across the entire flow field.

A second implication of this is that you can be extremely sensitive to round off errors, and these can cause strange spikes and peaks in the results. Make sure you are using double precision numerics. The large change in mesh size from the boundary to the centre is also contributing to the round off error, so moving to a even mesh size will reduce these effects as well.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 24, 2018, 12:08
Default
  #3
Member
 
Join Date: Jan 2018
Posts: 82
Rep Power: 5
Stroopwafelandcoffee is on a distinguished road
That makes a lot of sense actually. What kind of element size would you recommend for the evenly distributed case? I'll do a refinement study on it anyway, but maybe you know a ballpark in which to start?
Stroopwafelandcoffee is offline   Reply With Quote

Old   July 24, 2018, 18:42
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,643
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
As micro fluidic flows are usually very laminar, have little in the way of separations and rarely have strong gradients you can often get away with much coarser grids that you can use for high Reynolds number flows. So I would start with something like 10 elements across the section, and the mesh set up to use that mesh size for the whole domain. That is just a starting point, do a mesh size sensitivity study to find your actual requirement.

As you only have a single mesh size parameter it will also be quite simple to do mesh sensitivity studies.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 25, 2018, 18:08
Default
  #5
Member
 
Join Date: Jan 2018
Posts: 82
Rep Power: 5
Stroopwafelandcoffee is on a distinguished road
Well, it worked. Thanks! I learned a lot from this, glad I picked up the little project
Stroopwafelandcoffee is offline   Reply With Quote

Reply

Tags
laminar, microscopic, shear stress

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
CFD Post. Multiple results comparison zombiaska Visualization & Post-Processing 1 December 23, 2014 16:06
how cfd results can be trusted in a very complex geometry garrison Main CFD Forum 1 November 8, 2014 04:13
Import external CFD results into Autodesk CFD for visualisation julien.decharentenay Autodesk Simulation CFD 0 May 31, 2014 20:16
Future CFD Research Jas Main CFD Forum 10 March 30, 2013 12:26
CFD vs Experimetal Results for Aerofoil owhelan FLUENT 0 March 25, 2010 07:03


All times are GMT -4. The time now is 04:37.