which turbulence model should I choose?

itsqi7 · March 17, 2013, 02:12

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

itsqi7 · March 17, 2013, 02:17

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?

itsqi7 · March 17, 2013, 02:19

Sry, this is the result of symmetry wallsymentry_ke.jpg

Really confused about this attachments...

ghorrocks · March 17, 2013, 04:50

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?

itsqi7 · March 17, 2013, 15:21

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

ghorrocks · March 17, 2013, 17:19

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.

itsqi7 · March 17, 2013, 23:19

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.

ghorrocks · March 18, 2013, 05:20

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.

oj.bulmer · March 18, 2013, 10:57

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

ghorrocks · March 19, 2013, 04:52

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.

oj.bulmer · March 19, 2013, 04:55

Well, I realize that you were referring to the top most image, and I was referring to the bottom images. Two are oriented differently

itsqi7 · March 19, 2013, 18:04

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

ghorrocks · March 19, 2013, 18:13

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.

itsqi7 · March 19, 2013, 20:06

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

ghorrocks · March 20, 2013, 06:10

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.

oj.bulmer · March 20, 2013, 07:52

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

itsqi7 · March 20, 2013, 15:44

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

itsqi7 · March 20, 2013, 15:46

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

itsqi7 · March 20, 2013, 15:51

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.

ghorrocks · March 20, 2013, 16:29

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.

March 17, 2013, 02:12	which turbulence model should I choose?	#1
itsqi7 Member jiaqi wang Join Date: Jan 2013 Posts: 36 Rep Power: 13	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

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Use of k-epsilon and k-omega Models	Jade M	Main CFD Forum	40	January 27, 2023 07:18
Fluent :- turbulence Model	prince_pahariaa	FLUENT	9	May 20, 2016 03:41
What model of turbulence choose to study an external aerodynamics case	raffale	OpenFOAM	0	August 23, 2012 05:45
question about turbulence model selection and sensitivity	karananand	Main CFD Forum	1	February 26, 2010 04:41
Centrifugal Pump and Turbulence Model	Michiel	CFX	12	January 25, 2010 03:20

March 17, 2013, 02:19		#3
itsqi7 Member jiaqi wang Join Date: Jan 2013 Posts: 36 Rep Power: 13	Sry, this is the result of symmetry wallsymentry_ke.jpg Really confused about this attachments...

March 17, 2013, 04:50		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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, 17:19		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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, 05:20		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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 19, 2013, 04:55		#11
oj.bulmer Senior Member OJ Join Date: Apr 2012 Location: United Kindom Posts: 473 Rep Power: 20	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, 18:13		#13
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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 20, 2013, 06:10		#15
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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, 16:29		#20
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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.