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

Two Separate flow regions with Dynamic Meshing

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 26, 2019, 14:04
Default Two Separate flow regions with Dynamic Meshing
  #1
New Member
 
Minnesota
Join Date: Apr 2019
Posts: 10
Rep Power: 7
zjuv9021 is on a distinguished road
All,

I am performing a transient FSI with system coupling that is bending and displacing a tubing with an inner lumen fluid region to the point where the lumen is completely occluded and becomes essentially two separate flow regions, separated by the occluded lumen.

Is this possible to replicate with dynamic meshing? What options would I consider, if this can work?

Attached is a diagram of how far I've gotten with the deformed fluid region, with the red horizontal line indicating where the full occlusion is happening as I further compress this tubing
Attached Images
File Type: jpg Capture.jpg (91.9 KB, 32 views)
zjuv9021 is offline   Reply With Quote

Old   May 1, 2019, 13:36
Default
  #2
Senior Member
 
Join Date: Dec 2016
Posts: 152
Rep Power: 10
RaiderDoctor is on a distinguished road
Hey zjuv9021,


I'm assuming you are using ALE here, and not overset or a fictitious grid method. Unfortunately, you can't split a fluid domain into two parts. This will create a negative cell volume, and crash your sim. What you can do in Mechanical is set up a contact region, and add an offset so that the domain will never be split in two. I would then try playing around with "Contact Detection" in Fluent.
RaiderDoctor is offline   Reply With Quote

Old   May 1, 2019, 13:59
Default
  #3
New Member
 
Minnesota
Join Date: Apr 2019
Posts: 10
Rep Power: 7
zjuv9021 is on a distinguished road
Quote:
Originally Posted by RaiderDoctor View Post
Hey zjuv9021,


I'm assuming you are using ALE here, and not overset or a fictitious grid method. Unfortunately, you can't split a fluid domain into two parts. This will create a negative cell volume, and crash your sim. What you can do in Mechanical is set up a contact region, and add an offset so that the domain will never be split in two. I would then try playing around with "Contact Detection" in Fluent.
Thank you. I am utilizing FLUENT's dynamic meshing (Does this utilize ALE?).
Can you speak more to the specifics of setting up contact regions in Mechanical, as opposed to my fluid region geometry? I currently have a mechanical tubing with an inner lumen that has an inner lumen face, and outer lumen face, and 2 faces at the end of the tubing structure.

Within my fluid, I simply have an inlet, outlet, and wall face.

Does contact detection in fluent look for when the distance between the structural components are in a defined proximity, or the fluid region?

Kind regards,
Zach
zjuv9021 is offline   Reply With Quote

Old   May 1, 2019, 17:35
Default
  #4
Senior Member
 
Join Date: Dec 2016
Posts: 152
Rep Power: 10
RaiderDoctor is on a distinguished road
ALE stands for the arbitrary Lagragian-Eulerian method. This is basically a method in which the mesh is allowed to move and deform, and that motion is then accounted for in the governing equations. I tried finding a good resource for you, but this was the best I could find.

http://www.me.sc.edu/research/jzuo/C.../ALE/ALE_1.htm

Yes, the dynamic meshing tab does make use of the ALE method. If you are using this, though, it would be a good idea to understand how it works, and what it does to the governing equations. This isn't important in its function, though, but it's critical that you have a good understanding of the theory.

Oh man, talking about contact deserves its own forum. The basics are this, though; Mechanical doesn't automatically "see" the walls of solid domain (i.e., there's no collision detection there). If you want, imagine two boxes modeled in Mechanical. Now, slowly move one box towards the other. In the physical world, the boxes would come in contact with one another, and then stop moving due to the normal force acting on it. In Mechanical, however, the box would just keep moving straight through the stationary one like it wasn't even there. You have to tell it that contacting walls will actually touch, and then you have to tell it how they touch. For instance, is the surface fricitonal? Frictionless? Bonded? etc.? Check out the PPT I pulled from the internet.

https://www.dropbox.com/s/mkjudosrpf...ntact.ppt?dl=0

As I said before, when two walls in Mechanical touch, this means that fluid domain in Fluent is split in two. This is very bad, and will cause crashing to occur. To circumvent this issue, you can specify something known as a "contact offset" in Mechanical. This is basically where Mechanical will institute the contact you have selected, but it will be offset from the surface at a distance you select. This allows your fluid domain to remain in one piece.

Contact detection in Fluent is a tricky bugger. On one hand, it works perfectly. When two walls (that you say will eventually "touch") get close enough (you specify how close), Fluent will automatically change the cells in that region over to a new zone. Basically, there's still only one fluid domain, but now you have two zones; one with your original working fluid, and one with a very porous media in it. This media will not allow any fluid to pass through it, so you can essentially say that that region is simulating contact.

The problem with this is that CFD Post cannot post-process anything with contact detection. For some reason, it can't handle zones randomly appearing and disappearing. So, you have three choices; either post-process in Fluent (which is a bloody nightmare), Tecplot (if you have access/know how to use it), or don't use contact detection in Fluent.
RaiderDoctor is offline   Reply With Quote

Old   May 2, 2019, 13:52
Default
  #5
New Member
 
Minnesota
Join Date: Apr 2019
Posts: 10
Rep Power: 7
zjuv9021 is on a distinguished road
This really helps put this into lamens terms, thank you!

Say I want to see this mechanically buckle in two positions (see image), can I also do this? With now two separate "porous" regions.

Thank you,
Zach
Attached Images
File Type: jpg Capture.JPG (30.4 KB, 19 views)
zjuv9021 is offline   Reply With Quote

Reply

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
About Some Concepts:Laminar flow, turbulent flow, steady flow and time-dependent flow Jing Main CFD Forum 8 October 5, 2018 17:02
[ANSYS Meshing] Blocking and Meshing Strategy for an open flow domain over backward facing ramp Crank-Shaft ANSYS Meshing & Geometry 0 January 11, 2013 05:48
[ANSYS Meshing] Turbulent Flow meshing sherazi21st ANSYS Meshing & Geometry 0 December 22, 2011 12:25
[GAMBIT] Dynamic Meshing of a combustion chamber donarundas ANSYS Meshing & Geometry 1 December 2, 2009 07:13
Can 'shock waves' occur in viscous fluid flows? diaw Main CFD Forum 104 February 16, 2006 05:44


All times are GMT -4. The time now is 23:00.