# which turbulence model should I choose?

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

 March 17, 2013, 03:12 which turbulence model should I choose? #1 Member   jiaqi wang Join Date: Jan 2013 Posts: 36 Rep Power: 6 Sponsored Links Hi everyone, I try to simulate different velocity flow(turbulent flow) in a planar tube. Attachment 19909 However, no matter which turbulence model I choose, the results all seem as laminar. Can anyone tell me whats the problem? Thx. Regards, itsqi7

March 17, 2013, 03:17
#2
Member

jiaqi wang
Join Date: Jan 2013
Posts: 36
Rep Power: 6
This is the structure.structure.jpg
These are simulation results of k-e and SST[ATTACH]non_sst.jpg[/ATTACH]

However, after I defined the side walls as symmetry, both turbulent model can get turbulent flow. [ATTACH]symentry_sst.jpg[/ATTACH]

Is that because the planar tube is too thin?
Attached Images
 non_ke.jpg (43.7 KB, 12 views) symentry_ke.jpg (42.4 KB, 15 views)

 March 17, 2013, 03:19 #3 Member   jiaqi wang Join Date: Jan 2013 Posts: 36 Rep Power: 6 Sry, this is the result of symmetry wallsymentry_ke.jpg Really confused about this attachments...

 March 17, 2013, 05:50 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,725 Rep Power: 106 If the two bounding planes are walls then the effective Re number of this thing is much reduced and turbulence will dissipate very quickly - like you are seeing. What are you trying to model? A 2D diffuser? What have you used for boundary conditions on the top and bottom bounding planes?

March 17, 2013, 16:21
#5
Member

jiaqi wang
Join Date: Jan 2013
Posts: 36
Rep Power: 6
Quote:
 Originally Posted by ghorrocks If the two bounding planes are walls then the effective Re number of this thing is much reduced and turbulence will dissipate very quickly - like you are seeing. What are you trying to model? A 2D diffuser? What have you used for boundary conditions on the top and bottom bounding planes?
Hi Ghorrocks,

Thanks for ur reply. I want to simulate a 3D diffuser and by default I set all the boundaries except inlet, outlet as non-slip wall.

Regards,
itsqi7

 March 17, 2013, 18:19 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,725 Rep Power: 106 That is the problem then. You have reduced the Re number and increased turbulence dissipation by having lots of walls. If you want this to better represent a 3D diffuser either use symmetry planes for the top and bottom planes, or even better translational periodic boundaries.

March 18, 2013, 00:19
#7
Member

jiaqi wang
Join Date: Jan 2013
Posts: 36
Rep Power: 6
Quote:
 Originally Posted by ghorrocks That is the problem then. You have reduced the Re number and increased turbulence dissipation by having lots of walls. If you want this to better represent a 3D diffuser either use symmetry planes for the top and bottom planes, or even better translational periodic boundaries.
Thanks ghorrocks. I set the top and bottom planes as symmetry planes and get the reverse flow in the outlet.
Interestingly, the turbulence kinetic energy only changed in a tiny region near the inlet of diffuser, which can be seen in the picture.fullcontour.jpg
Detail of contour.detail.jpg
But I still don't understand what caused "the reduced Re number" and what is the meaning of using symmetry planes for top and bottom planes. Could you please briefly explain this? Thanks.

 March 18, 2013, 06:20 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,725 Rep Power: 106 Have a look at the hydraulic radius for your shape. Also, you will get less turbulence dissipation with translational periodic boudnaries rather than symmetry planes. It is all a matter of how many degrees of freedom you are constraining - if the FEA analogy makes sense to you. The reverse flow is probably due to a separation and is probably real. Then you will ned to extend your domain further downstream.

March 18, 2013, 11:57
#9
Senior Member

OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 13
Is the cross section of your diffuser circular or rectangular? If it is circular, you may want to use an axisymmetric wedge rather than 2D geometry you are currently using.

Quote:
 But I still don't understand what caused "the reduced Re number"...
If you have no-slip walls at the side walls, they will offer frictional resistance and there won't be a significant velocities in your geometry. Apparently, the hydraulic diameter of your geometry should be very small. All these will result in smaller Re and hence laminar flow as you are experiencing.

It makes perfect sense to use symmetry boundary condition at the side walls, as you showed in post #3. This way, the velocities will not be resisted by walls and Re would be higher, producing turbulent flow.

Although, I didn't understand why Glenn suggested using symmetry at top and bottom bounds. If I am not missing something, this doesn't sound right. They should be no-slip walls. But the big side walls should be symmetry.

If the cross section of your diffuser is rectangular, then it makes sense to use translational periodic condition at the two big parallel side walls.

OJ

March 19, 2013, 05:52
#10
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,725
Rep Power: 106
Quote:
 Although, I didn't understand why Glenn suggested using symmetry at top and bottom bounds.
Simply confusion over what is the "side" and what is the "top". To clarify - the diffuser section has to be no slip walls, and so does the duct leading into and out of it, but the two planar faces in close proximity should be either symmetry planes or translational periodic interfaces.

 March 19, 2013, 05:55 #11 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 13 Well, I realize that you were referring to the top most image, and I was referring to the bottom images. Two are oriented differently

March 19, 2013, 19:04
#12
Member

jiaqi wang
Join Date: Jan 2013
Posts: 36
Rep Power: 6
Quote:
 Originally Posted by ghorrocks That is the problem then. You have reduced the Re number and increased turbulence dissipation by having lots of walls. If you want this to better represent a 3D diffuser either use symmetry planes for the top and bottom planes, or even better translational periodic boundaries.
Hi Glenn,

I think I misunderstand your point about top side either. The pic in post#3 is the result of setting big side walls as symmetry boundaries, and the pics in post#7 are the results of setting small side walls as symmetry boundaries(Although I don't know why you suggested that then...).
Your suggestion is to set big side walls as either symmetry or translational periodic boundaries, right? But doesn't this simulate an infinite thick diffuser? What I want to simulate is the flow in a rectangular cross section as in the pics rather than a thick one.
Thanks a lot for ur and OJ's help.

jiaqi

 March 19, 2013, 19:13 #13 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,725 Rep Power: 106 Yes, both the symmetry plane and translational periodicity approaches are simulating infinitly ducts. But if the geometry you show is what the true 3D shape of this thing is then you should expect it to have a lot of turbulence dissipation in it. Have you worked out the Re number of the flow? I would use the thin dimension of the thickness for the length scale, not the larger cross dimension. That will tell you how turbulent the flow is going to be.

March 19, 2013, 21:06
#14
Member

jiaqi wang
Join Date: Jan 2013
Posts: 36
Rep Power: 6
Quote:
 Originally Posted by ghorrocks Yes, both the symmetry plane and translational periodicity approaches are simulating infinitly ducts. But if the geometry you show is what the true 3D shape of this thing is then you should expect it to have a lot of turbulence dissipation in it. Have you worked out the Re number of the flow? I would use the thin dimension of the thickness for the length scale, not the larger cross dimension. That will tell you how turbulent the flow is going to be.
Hi Glenn,

I set the inlet flow rate as 1m/s, and the narrowest cross section is 2mm*10mm. So Re should be 3.3e3. I think this Re should have turbulent flow. Anyway, even I set the inlet flow rate as 100m/s, there is still no turbulent flow. I don't know whether it's the right answer. But when I use the result to calculate the pressure recovery coefficient, it seems that it does not confirm with the real situation.

Regards,
itsqi7

 March 20, 2013, 07:10 #15 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,725 Rep Power: 106 Re=3300 is a very low turbulence flow. You will not get much turbulence in it at the best of times. Also, many turbulence models (k-e especially) are designed for high Re flow and do not function well at low Re like this. You are going to carefully choose a turbulence model to be appropriate for this flow. When you say "these is still no turbulent flow", how are you reaching that conclusion? Anywhere the k value is more than zero you have turbulent flow.

March 20, 2013, 08:52
#16
Senior Member

OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 13
Quote:
 Anyway, even I set the inlet flow rate as 100m/s, there is still no turbulent flow. I
Reynolds number with 100 m/s would be 330000, which should definitely be a turbulent flow. Can you attach snap of results?

Also, for Re 3300, have you tried low Re models or transitional models?

OJ

March 20, 2013, 16:44
#17
Member

jiaqi wang
Join Date: Jan 2013
Posts: 36
Rep Power: 6
Quote:
 Originally Posted by ghorrocks Re=3300 is a very low turbulence flow. You will not get much turbulence in it at the best of times. Also, many turbulence models (k-e especially) are designed for high Re flow and do not function well at low Re like this. You are going to carefully choose a turbulence model to be appropriate for this flow. When you say "these is still no turbulent flow", how are you reaching that conclusion? Anywhere the k value is more than zero you have turbulent flow.
Hi Glenn,

I used SST model to simulate this low Re flow.
You are right. I misunderstood the 'turbulent flow'. I thought there should be back flow. Actually for even low Re there is k value more than zero near the side but no back flow shown in the contour. This phenomenon is what I want to get, just not obvious
Thanks a lot for your help.

Regards,
itsqi7

March 20, 2013, 16:46
#18
Member

jiaqi wang
Join Date: Jan 2013
Posts: 36
Rep Power: 6
Quote:
 Originally Posted by oj.bulmer Reynolds number with 100 m/s would be 330000, which should definitely be a turbulent flow. Can you attach snap of results? Also, for Re 3300, have you tried low Re models or transitional models? OJ
Hi OJ,

I think I got the result but thought it was wrong... Please see the above post.
Thanks very much for your help.

Regards,
itsqi7

March 20, 2013, 16:51
#19
Member

jiaqi wang
Join Date: Jan 2013
Posts: 36
Rep Power: 6
Quote:
 Originally Posted by itsqi7 Hi Glenn, I used SST model to simulate this low Re flow. You are right. I misunderstood the 'turbulent flow'. I thought there should be back flow. Actually for even low Re there is k value more than zero near the side but no back flow shown in the contour. This phenomenon is what I want to get, just not obvious Thanks a lot for your help. Regards, itsqi7
By the way, I think meshing also mattered because I changed the inflation of viscous boundary layer before I got the right answer.

 March 20, 2013, 17:29 #20 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,725 Rep Power: 106 It sounds like you are still misunderstanding turbulent flow. Turbulence is NOT recirculations, back flow and/or transient flow. Turbulence IS 3D transient flow which has a wide range of time and length scales, right down to the microscopic level (the turbulent energy cascade) - see any turbulence textbook for more discussion on this definition. So separations, flow instability, recirculations and transient flow can still occur in laminar flows - but they will not have time and length scales down to the microscopic levels.

 Thread Tools Display Modes Linear Mode

 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 On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Jade M Main CFD Forum 27 August 11, 2017 15:41 prince_pahariaa FLUENT 9 May 20, 2016 03:41 raffale OpenFOAM 0 August 23, 2012 05:45 karananand Main CFD Forum 1 February 26, 2010 05:41 Michiel CFX 12 January 25, 2010 04:20