# Turorials on pipe flow

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

 January 12, 2012, 12:24 Turorials on pipe flow #1 New Member   Join Date: Dec 2011 Posts: 17 Rep Power: 6 Hi everybody, I was just wondering if any of you guys know of a tutorial that will guide one in gambit/fluent in making a simple pipe so that I can show the fluid going to fully developed and see the pressure drop as flow goes along the pipe. I thought it was simple to do geometry as in just have a top line and bottom line, however I have been told that I had to do a slice of the circle. I am confused. Does anyone know what he means?

 January 13, 2012, 03:02 #2 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 3,160 Rep Power: 32 2d? 3d? is your pipe straight? http://202.118.250.111:8080/fluent/G...guide/tg03.htm __________________ In memory of my friend Hervé: CFD engineer & freerider

 January 13, 2012, 10:45 pipe flow #3 New Member   Join Date: Dec 2011 Posts: 17 Rep Power: 6 Thank you Max for a reply. I have done that tutorial you posted. The pipe I am doing is straight. My supervisor told me that since the pipe is asymmetric I have to do a slice of the pipe. He said if its difficult to do I can do planar and lose considerable marks so am assuming its in 3D. Below is the diagram of what he said I had to do. He said since its asymmetric I just have to consider the slice as there is no need to consider the whole pipe?

 January 13, 2012, 12:36 #4 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 993 Rep Power: 17 well, you can draw and simulate: 1- a 2d axisymmetric tube, by drawing 4 points (2 for the axis and 2 for the upper part of the tube), create edges and the surface, mesh it and apply boundary conditions for inlet, outlet, wall and axis; this means drawing half of the tube you have attached and simulate a 2d axisymmetric problem. 2- you can draw and simulate the 3d tube, by drawing a cilinder and assigning boundary conditions, inlet, outlet and wall. 3- you can draw and simulate a slice, for example 1/4 of the tube (3d), by drawing 1/4 of cilinder and assigning boundary conditions, inlet, outlet, wall and periodic (for the 2 rectangular faces); when you mesh the reactangular faces you have to link them. Then in fluent you will set periodic conditions. 4- you can draw and simulate 3d half pipe, by drawing half cilinder and assigning boundary conditions, inlet, outlet, wall and simmetry (to the rectangular face). The simplest one is the 2d axisymmetric problem. Hope that helps Daniele mrenergy likes this. Last edited by ghost82; January 13, 2012 at 14:08.

January 13, 2012, 16:10
#5
New Member

Join Date: Dec 2011
Posts: 17
Rep Power: 6
Quote:
 Originally Posted by ghost82 3- you can draw and simulate a slice, for example 1/4 of the tube (3d), by drawing 1/4 of cilinder and assigning boundary conditions, inlet, outlet, wall and periodic (for the 2 rectangular faces); when you mesh the reactangular faces you have to link them. Then in fluent you will set periodic conditions.
I think point 3 sounds like what I meant to be doing. What is the reason for simulating just a slice as opposed to half the pipe or a full pipe, is there advantages?

Is there a guide on how to simulate a slice? If not do you mean draw a cylinder first. Then take away some volume, say 3/4 of it. Then add two rectangles to close the cylinder. Then do boundary conditions.

Thank you

January 13, 2012, 23:59
#6
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,372
Rep Power: 20
Quote:
 Originally Posted by Gamb1t I think point 3 sounds like what I meant to be doing. What is the reason for simulating just a slice as opposed to half the pipe or a full pipe, is there advantages? Is there a guide on how to simulate a slice? If not do you mean draw a cylinder first. Then take away some volume, say 3/4 of it. Then add two rectangles to close the cylinder. Then do boundary conditions. Thank you
There is the most obvious advantage of reducing the overall computation cost by simulating the smallest representative domain of the whole problem. From symmetry and periodicity arguments, the solution to the quarter pipe simulation should be exactly the same as the full pipe problem. The same argument goes for the half-pipe. Half-pipe is smaller than a full-pipe. A quarter-pipe is even smaller than a half-pipe. So solve the quarter-pipe.

Your outline is correct. Create a 3D representation of the 1/4 cylinder (however you are most comfortable with) by closing the two faces (which will be rectangles). Then Mesh it. Then import into fluent and start setting up the problem.

January 14, 2012, 04:41
#7
Senior Member

Daniele
Join Date: Oct 2010
Location: Italy
Posts: 993
Rep Power: 17
Quote:
 Originally Posted by Gamb1t I think point 3 sounds like what I meant to be doing. What is the reason for simulating just a slice as opposed to half the pipe or a full pipe, is there advantages? Is there a guide on how to simulate a slice? If not do you mean draw a cylinder first. Then take away some volume, say 3/4 of it. Then add two rectangles to close the cylinder. Then do boundary conditions. Thank you
You should obtain the same results with all simulations.
The less expensive in termes of computational cost is the 2d axisymmetric.
If you want to draw 1/4 pipe, in gambit you can draw the full cilinder, then draw a square base prism with one vertex of the base with the same coordinate of the center of one base of the cilinder, with side of the base equal or greater than the radius of the circle, and with prism height equal or greater than the height of the cilinder.
After that you can intersect the two volumes and you will obtain the 1/4 cilinder, you don't have to create any further face..
In the mesh tab, link the two rectangular faces, premesh other edges/faces and mesh the volume.
Set boundary conditions, export the 3d mesh, start fluent and set your problem.

Daniele
Attached Images
 Immagine.jpeg (7.5 KB, 24 views)

 January 14, 2012, 16:59 #8 New Member   Join Date: Dec 2011 Posts: 17 Rep Power: 6 Thank you for replies. I think I now know how its meant to be done. I will try on Monday to get this pipe out of the way. Danielle, that attached thumbnail really helped my understanding. Last edited by Gamb1t; January 14, 2012 at 17:15.

 January 15, 2012, 09:57 #9 New Member   Join Date: Dec 2011 Posts: 17 Rep Power: 6 Hi, I have another point: Since I am trying to find when the flow becomes fully developed and when a pressure drop occurs, does it mean I have to make a really long pipe or is there another way to do it. Thanks.

January 15, 2012, 10:40
#10
Senior Member

Daniele
Join Date: Oct 2010
Location: Italy
Posts: 993
Rep Power: 17
Quote:
 Originally Posted by Gamb1t Hi, I have another point: Since I am trying to find when the flow becomes fully developed and when a pressure drop occurs, does it mean I have to make a really long pipe or is there another way to do it. Thanks.
You can estimate the length for fully developed flow in pipe:
for laminar flows:
El=0.06*Re
le=El*d

for turbulent flows:
El=4.4*Re^(1/6)
le=El*d

Where:
El=Entrance Length Number (dimensionless)
Re=Reynolds number
le=length to fully developed velocity profile
d=pipe diameter

Make sure to draw a pipe longer than the length to fully developed velocity profile.

PS: pressure drop occur all along the pipe, even after the flow is fully developed..

Daniele

January 15, 2012, 12:18
#11
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,372
Rep Power: 20
Quote:
 Originally Posted by Gamb1t Hi, I have another point: Since I am trying to find when the flow becomes fully developed and when a pressure drop occurs, does it mean I have to make a really long pipe or is there another way to do it. Thanks.
I am a little confused.

If you are studying the developing length, then of course you would need a really long pipe. Or is that not the problem?

You can simulate only the fully developed portion and not use any entrance length if all you care about is flow after it has become fully developed, is that your problem?

January 15, 2012, 13:55
#12
New Member

Join Date: Dec 2011
Posts: 17
Rep Power: 6
Quote:
 Originally Posted by LuckyTran I am a little confused. If you are studying the developing length, then of course you would need a really long pipe. Or is that not the problem? You can simulate only the fully developed portion and not use any entrance length if all you care about is flow after it has become fully developed, is that your problem?
I am studying incompressible pipe flow. I don't have to particularly study the developing length but thought it would be something good to do since its the only thing I can think of. After the straight pipe I would need to do a pipe with orifice plate inside it. I think for that I would need to simulate flow after it becomes fully developed.

Daniele, thanks for those equations. Really appreciate it.

February 11, 2013, 18:37
#13
New Member

Jing Shi
Join Date: Feb 2013
Posts: 20
Rep Power: 5
Quote:
 Originally Posted by ghost82 well, you can draw and simulate: 1- a 2d axisymmetric tube, by drawing 4 points (2 for the axis and 2 for the upper part of the tube), create edges and the surface, mesh it and apply boundary conditions for inlet, outlet, wall and axis; this means drawing half of the tube you have attached and simulate a 2d axisymmetric problem. 2- you can draw and simulate the 3d tube, by drawing a cilinder and assigning boundary conditions, inlet, outlet and wall. 3- you can draw and simulate a slice, for example 1/4 of the tube (3d), by drawing 1/4 of cilinder and assigning boundary conditions, inlet, outlet, wall and periodic (for the 2 rectangular faces); when you mesh the reactangular faces you have to link them. Then in fluent you will set periodic conditions. 4- you can draw and simulate 3d half pipe, by drawing half cilinder and assigning boundary conditions, inlet, outlet, wall and simmetry (to the rectangular face). The simplest one is the 2d axisymmetric problem. Hope that helps Daniele
I have a question, if I use a 2d pipe tube by drawing 4 points (2 for the upper parter and two for the bottom), create edges and the surface, mesh it and apply bounday conditions for inlet, outlet, wall and simulate a 2d planar problem, it is not right, is it? The results are not in agreement with 3d tube.

February 12, 2013, 05:52
#14
Senior Member

Daniele
Join Date: Oct 2010
Location: Italy
Posts: 993
Rep Power: 17
Quote:
 Originally Posted by Jing Hi, see your good answer to that question. I have a question, if I use a 2d pipe tube by drawing 4 points (2 for the upper parter and two for the bottom), create edges and the surface, mesh it and apply bounday conditions for inlet, outlet, wall and simulate a 2d planar problem, it is not right, is it? The results are not in agreement with 3d tube.
Hi!
it is not correct if you simulate it as a 2d planar problem; in 2d planar you are simulating a squared-rectangular base conduct with a depth equal to the value you set in the reference values panel.
To compare results with 3d simulation you have to simulate it as 2d axisymmetric.

Daniele

 February 12, 2013, 05:55 #15 New Member   Jing Shi Join Date: Feb 2013 Posts: 20 Rep Power: 5 Thank you very much! Regards, Jing

February 17, 2013, 08:57
#16
Super Moderator

Sijal
Join Date: Mar 2009
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Quote:
 Originally Posted by ghost82 3- you can draw and simulate a slice, for example 1/4 of the tube (3d), by drawing 1/4 of cylinder and assigning boundary conditions, inlet, outlet, wall and periodic (for the 2 rectangular faces); when you mesh the rectangular faces you have to link them. Then in fluent you will set periodic conditions.
Shouldn't we apply symmetry on both sides?

 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 hasanduz Main CFD Forum 2 October 11, 2013 17:59 subsemitonium CFX 6 May 6, 2013 22:00 mazhar1613 ANSYS Meshing & Geometry 1 January 12, 2012 00:18 Primadhani FLUENT 1 May 11, 2011 20:41 Saima CFX 1 January 10, 2011 17:41

All times are GMT -4. The time now is 00:02.