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

Wrong direction of flow!!!

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

Like Tree2Likes
  • 1 Post By ghorrocks
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   July 18, 2013, 01:26
Question Wrong direction of flow!!!
  #1
New Member
 
Hung
Join Date: Jul 2013
Location: Seoul
Posts: 7
Rep Power: 4
hungnguyen1908 is on a distinguished road
hi all,
I was simulating the flow of Vane tidal turbine. After running in CFX-Solver, I analysed the result in CFX-Post, the direction of flow made me surprised and confused. I mean the direction of flow tends to run from the outlet to the inlet. Physically, the flow must direct from inlet to the outlet.
I divided the inlet and outlet into 2 parts for each (Part no.1 for water, and part no.2 for Air). In term of outlet boundary condition, I setup part no.1 (Water) as "outlet"; meanwhile, part no.2 (Air) is setup as "opening".
If I change part no.2 into "outlet", it will immediately appear the error "Overflow". But if I keep setting up part no.2 as "opening", that'll run well. however, the direction of flow is still wrong in this case.
Are there anyone able to give me some explainations and useful advices for this??? If u really care about my problems, I can send several images of my model and my set-up parameters to u.
Many thanks!
hungnguyen1908 is offline   Reply With Quote

Old   July 18, 2013, 09:02
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,807
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You obvious have something very wrong in your setup. Please post an image and your CCL on the forum.
ghorrocks is offline   Reply With Quote

Old   July 18, 2013, 22:28
Default Dear Mr.Ghorrocks
  #3
New Member
 
Hung
Join Date: Jul 2013
Location: Seoul
Posts: 7
Rep Power: 4
hungnguyen1908 is on a distinguished road
https://www.dropbox.com/s/b091nwtrpi...CFD-online.rar

This is a link of my document, including one powerpoint file and some pictures of my calculation domain in CFX-Pre.
Please check carefully the informations of my calculation. I'm so confused about this. I over and over re-designed and changed many parameters, but it was still wrong. (

Best regard!
hungnguyen1908 is offline   Reply With Quote

Old   July 19, 2013, 06:32
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,807
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Some comments:

For this model you should use the alternate rotation model. This is because the fluid is still really travelling in the stationary frame and not rotating in the rotating frame. This will improve convergence a small amount. Look in the documentation for more details on this.

Remove the specified pitch angles, make that "none". You are modelling the whoel rotor so you do not need pitch correction.

This model would be MUCH simpler if the inlet is purely water. You appear to have half water and half air. Is that what you really want to model? Wouldn't the water fill the whole inlet runner, at least at the inlet?

Unless you know what you are doing and have done a sensitivity analysis do not define the time step size yourself. Use adaptive time stepping, homing in on 3-5 coeff loops per time step. The most common mistake by newbies in transient simulation is by setting a time step size that is far too big.

Remove the minimum coeff loops in the convergence tolerance, and make the maximum 10.

Obviously this is a transient simulation. There is no way this was ever going to work steady state.
hungnguyen1908 likes this.
ghorrocks is offline   Reply With Quote

Old   July 19, 2013, 06:34
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,807
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Oh yes - and your mesh quality at the bottom of the rotor where the blades almost touch the bottom is likely to be horrible. It might be worth your while to distort the geometry slightly in this region to improve mesh quality.
hungnguyen1908 likes this.
ghorrocks is offline   Reply With Quote

Old   July 19, 2013, 08:25
Default Many thanks for your advice, Mr.Ghorrocks
  #6
New Member
 
Hung
Join Date: Jul 2013
Location: Seoul
Posts: 7
Rep Power: 4
hungnguyen1908 is on a distinguished road
https://www.dropbox.com/s/p42vvinzdj...2013.07.10.rar

I'm reading about "alternate rotation model" to understand clearly before I set up. the link above is my "*.def" file that I setup before to simulate.

As u know, the inlet must include water and air because that's my professor's project. And I'm an assistant for him. I have a mission of modeling it.

I'm new user of Ansys CFX. Then I have a little experience. And I have to learn about this so much!

Again, many thanks to your comments.
Best regard!
hungnguyen1908 is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Accelerate flow in one direction JanR FLUENT 2 January 19, 2011 16:52
Can 'shock waves' occur in viscous fluid flows? diaw Main CFD Forum 105 November 20, 2009 05:19
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07
udf error srihari FLUENT 0 February 9, 2009 10:00
component flow direction fieldnames for boundary profiles required. Ricky Wong FLUENT 1 May 12, 2000 10:36


All times are GMT -4. The time now is 03:43.