# Setting the height of the stream in the free channel

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

 July 9, 2015, 11:23 Setting the height of the stream in the free channel #1 New Member   kevin Join Date: Sep 2014 Posts: 13 Rep Power: 10 hello again, I am doing a project on flow around a surface piercing cylinder. I carried out an experiment to measure the height of the water in the channel, the height of the flow when it rises up at the front of the cylinder and dips down around the sides and back of the cylinder. The results were: free stream height=80mm wave height at front of cylinder=81mm side(90 degrees)=76mm back=75mm The velocity of the flume was 0.21m and the width of the flume was 120mm. I used the CFX tutorial on flow over a bump to try and learn how to carry out this problem. I got all the basic steps in and used the expressions: Name Definition UpH 0.08[m]DownH 0.08 [m] DenWater 997 [kg m^-3] DenRef 1.185 [kg m^-3] DenH (DenWater - DenRef ) UpVFAir step((y-UpH)/1[m]) UpVFWater 1-UpVFAir UpPres DenH*g*UpVFWater*(UpH-y) DownVFAir step((y-DownH)/1[m]) DownVFWater 1-DownVFAirDownPres DenH*g*DownVFWater*(DownH-y) The only things I changed from the tutorial were the upstream and downstream heights. The domain I'm using is 1m long and 120mm wide. I was wondering why when I run the results the flow seems to come in to the inlet boundary at the correct height of 80mm but then dips down dramatically before it develops up to the cylinder were the action happens. The results I was looking to achieve were the pressure profile of the cylinder, the height of the isosurface around the cylinder and the Cd of the cylinder. Any help or guidance would be much appreciated. Thanks for your time. Regards, Kevin McCartin Undergraduate Mech Engineering, Institute of technology Tallaght PS: I have my file saved as an ANSYS workbench file but it will not allow me to attach it?

 July 9, 2015, 18:58 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,372 Rep Power: 139 Please post your CCL (that's just a small text file) and an image of what you are modelling.

 July 9, 2015, 20:34 #3 New Member   kevin Join Date: Sep 2014 Posts: 13 Rep Power: 10 Ghorrocks, Thanks for your help and time it is much appreciated. I am not sure how to access the ccl file.I am presuming it is the .out file on ANSYS workbench 15 as it is a text file. I have attached 3 photos in a word document also to try show the situation a little better. As you will see from the photo at the inlet boundary the flow suddenly drops. Maybe there is a problem with the expressions used further upstream. Thanks again. Kevin McCartin Mechanical engineering undergraduate, Institute of technology, Tallaght, Ireland Last edited by kevinmccartin; July 9, 2015 at 20:35. Reason: no attachments

 July 9, 2015, 20:42 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,372 Rep Power: 139 In CFX-Pre go file export CCL. When the free surface rapidly changes like this it is usually because the free surface you have specified is incompatible with the flow conditions (velocity or fluid motion or whatever) and this causes the fluid motion to rapidly drop. The problem is usually a incorrectly defined boundary condition.

July 9, 2015, 20:49
Attachments
#5
New Member

kevin
Join Date: Sep 2014
Posts: 13
Rep Power: 10
Ghorrocks,
attached are 2 pictures. I am unable to find the .ccl file in the directory at the moment im not too sure how to access it from workbench.
Thanks.
Regards,
Kevin
Attached Images
 picture 1.JPG (44.2 KB, 61 views) picture 2.JPG (34.4 KB, 60 views)

 July 9, 2015, 21:01 #6 New Member   kevin Join Date: Sep 2014 Posts: 13 Rep Power: 10 Apolagies only saw your last message there. I tried to export but I keep getting a warning message saying "nothing to export" in the cfx pre. It is probably because I am using a virtual machine to access ANSYS. Thanks Kevin

 July 9, 2015, 21:03 #7 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,372 Rep Power: 139 CFX-Pre is the setup block in workbench. You can only access the CCL via the GUI from CFX-Pre. Your images confirm what I suspected, you almost certainly have not specified the inlet BC correctly. The CCL will contain the information about what you have done. kevinmccartin and karachun like this.

 July 9, 2015, 21:11 #9 New Member   kevin Join Date: Sep 2014 Posts: 13 Rep Power: 10 Ghorrocks, Above is the CCL file. I am not sure how to set boundaries any other way. Set an inlet velocity and an outlet static pressure. I used the 2 walls as non slip walls along with cylinder surfaces. The top was used as an opening with entrainment. Thanks Kevin

 July 9, 2015, 21:22 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,372 Rep Power: 139 The boundaries you have defined are inconsistent. You have set a flow rate and free surface height at the inlet (which is it applying), but the exit boundary condition requires the free surface to be much lower than you specify and this lower height propagates back up the domain. You need to be a bit more clever with your exit boundary. I would consider replacing the exit boundary with a chamber where you keep the free surface height at the desired level. Or you might use a momentum source term to do it. Whatever you do, have a careful think about exactly what your BCs are specifying. The way this tutorial sets up the boundary conditions might not be the best way for you to do it in your case.

 July 9, 2015, 21:36 #11 New Member   kevin Join Date: Sep 2014 Posts: 13 Rep Power: 10 Ghorrocks, Thanks for your time and recommendations. I will do some additional research on this tomorrow and see how I do. Thanks for your time, you sir are a gent. Regards Kevin

October 13, 2022, 18:01
#12
Member

Ashkan Kashani
Join Date: Apr 2016
Posts: 34
Rep Power: 9
I understand it's been quite a while since this discussion was made but I was hoping to see your comment on my problem here as it's relevant.
Quote:
 Originally Posted by ghorrocks The boundaries you have defined are inconsistent. You have set a flow rate and free surface height at the inlet (which is it applying), but the exit boundary condition requires the free surface to be much lower than you specify and this lower height propagates back up the domain.
I agree with you because using the same inlet and outlet boundary conditions, I'm having the same problem of water surface dropping along the channel length.
Quote:
 Originally Posted by ghorrocks I would consider replacing the exit boundary with a chamber where you keep the free surface height at the desired level.
I'm not sure exactly what you meant by a "chamber" but I set a part of the outlet, as high as the water surface elevation at the inlet, as a no-slip wall in order to force the water surface to rise. However, by doing so, long-lasting unsteadiness appears in the form of travelling waves along the channel length. I'm thinking of artificially increasing the viscosity close to the domain boundaries in the hope of accelerating the attenuation of these waves. However, I'm not sure if this trick is physically/numerically appropriate.

 October 13, 2022, 21:43 #13 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,372 Rep Power: 139 The chamber I was referring to is to artificially put a chamber on the exit boundary, designed to keep the water level at the correct level. You could do this with a weir arrangement. Transient waves in free surface simulations are normal. I do not generally recommend applying non-physical effects to remove them - they are real, so you should model them. You probably have to use a transient model anyway, so modelling the waves should not be too much of a problem. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 Tags coefficient drag, cylinder, free surface, surface piercing

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post maximus FLUENT 1 September 10, 2014 16:20 ms.jafarinik FLUENT 0 April 18, 2010 14:38 pkgupta FLUENT 0 April 2, 2010 05:56 AB Siemens 6 November 15, 2004 04:41 R Amini Main CFD Forum 1 May 2, 2002 05:16

All times are GMT -4. The time now is 13:40.