Pipe U-Bend FLUENT Example

Jason Oakley, Spring 2007

Minor edits by Scott Sanders, Spring 2007

Problem statement:

Determine the force in the x-direction on a u-bend for pipe carrying water. The pipe has a square cross-section with sides of 75.5 mm. The horizontal inlet run is 300 mm as is the outlet run. There is a uniform velocity inlet of 10 m/s. From the control volume analysis of Ch.4 (Fluid Mechanics, Fox, McDonald, Pritchard, 6th Ed.) you could expect the force to be:

,

where U=10 m/s, r=998 kg/m3, A=0.0057 m2, which yields F=1,138 N. {it would be good practice to verify this on your own J}

The first step is to create the 2D geometry and mesh in Gambit (Windows or Unix) at CAE

  1. Choose menu>solver>fluent 5/6
  2. Right side buttons, choose geometry, vertex command button
  3. Choose create real vertex (under global), the default is origin, click apply (this will be the center of the arcs). Now create the rest of the vertices:

X / Y / Z
0 / -0.05 / 0
0 / -0.1255 / 0
-0.3 / -0.1255 / 0
-0.3 / -0.05 / 0
-0.3 / 0.05 / 0
-0.3 / 0.1255 / 0
0 / 0.1255 / 0
0 / .05 / 0
0.05 / 0 / 0
0.1255 / 0 / 0
  1. Click on the “fit to window” button in the lower right (there are two rows of five) which had two triangles on it to zoom in on the vertices.
  2. Click the edge command button and we will first create the straight edges. Hold down the shift button and click the upper-leftmost vertex and then the one just below it, and click apply. Continue the process for each of the other straight edges.
  3. Now create the bend which has an inside and outside for a total of four 90 degree sections. Right click on the create edge button and choose arc. Hold shift and choose the center, then click in the “end-points” box so it is yellow, then hold shift and click the endpoints for the first of the four 90 degree arcs. Continue for the next three arcs and the edges are finished.
  4. Choose the face command button. Click the “up arrow” to the right of the yellow box and click “All ->”, and close, and apply. This connects all the yellow edges and turns them into a blue wire-frame face.
  5. Choose the teal “zones command button” box under “operation” and choose “specify continuum types”.
  6. Shift-left click on any face edge and click apply and this will make the face filled with a fluid continuum.
  7. Choose “specify boundary types” box. We will make the upper left vertical edge a pressure outlet, shift-click it, and under “Type”, instead of wall, choose “Pressure_outlet” and apply.
  8. Shift click on each of the four horizontal walls, under “Type” select wall, and name it “horiz_walls”, and apply.
  9. Shift click on each of the four arcs, under “Type” select wall, and name it “bend_walls”, and apply.
  10. The lower left vertical edge will be a velocity inlet, shift-click it, and under “Type”, choose “Velocity_inlet”, and apply.
  11. Choose the yellow mesh command button.
  12. Choose the face command button.
  13. Shift click any edge on the face, change the spacing to 0.003 and apply.
  14. Menu, file, save as, browse, and choose your filename (you may just want to save it to the c:\temp directory and then copy it to your flash disk or home disk when you are done).
  15. Menu, file, export, mesh, browse, choose filename, click “export 2-D (x-y)mesh”, and accept

The second step is to open Fluent, choose 2ddp (two-dimensional, double precision) and run the simulation.

  1. On the menu, file>read>case and browse to your mesh file. Look at your grid by display>grid, display. When you are done with an option box (such as the open one) click the “close” button to close it- they don’t typically close automatically when you click “display” or “apply”.
  2. Define>models>viscous, choose inviscid.
  3. Define>materials, choose Fluent fluid materials database, scroll down to water-liquid (h20<l>), select and copy. Close. Close.
  4. Define>operating conditions, click gravity, in Y box enter -9.81, ok.
  5. Define>boundary conditions, select fluid (there might be a number after it, such as fluid.1), set, material name, water-liquid, ok.
  6. Still in boundary conditions, select velocity_inlet, set, in velocity magnitude box enter 10 m/s, ok, close.
  7. Solve>initialize>initialize, enter 1 m/s for x velocity, init, close.
  8. Solve>monitors>residual, under the options heading put a check mark in the plot box, and for the plotting window set to it 1. Set absolute criteria to 1e-5 for each of the three: continuity, x- and y- velocity. Click ok.
  9. Display>contours>density to verify that the fluid is water and not air.
  10. Solve>iterate, set number of iterations to a large number, e.g. 10000, and iterate. This took my computer 322 iterations and less than a minute.
  11. File>write>case and data, to save results.
  12. Report>forces, choose “bend_walls” and print, the answer will be output in the fluent window. The answer is about 16,900 Nt. Since this is a 2D simulation, the answer is in a per-meter format, therefore it needs to be multiplied by the side of the square duct, 75.5 mm, and the correct force in the x-direction is 1,275 Nt.
  13. Display>contours drop-down box>pressure>absolute pressure, under options put a check mark in the filled box, click display. Right click on the bar above the picture (title bar), choose page setup, and specify: color, DIB Bitmap, true color, vector, ok. Now you can copy this picture to the clipboard by right-clicking on bar above the picture and “copy to clipboard” for pasting into a word document if you wanted to write a report, etc. We note that the inlet pressure is higher than the outlet pressure (which is appropriately 101,325 Pa).

  1. There are a number of ways to find the pressure that the simulation calculated at the inlet. Choose plot>xy plot pressure, absolute pressure, plot direction x 0 and y 1, and specify the velocity_inlet and plot:

  1. We see that the inlet pressure is 1.19e5, therefore, to more accurately compare to the control volume calculation we need to subtract the pressure difference multiplied by the duct area: (119,000-101,325)*0.0057=101 Nt, therefore, the force on the bend, just from the linear momentum change is: 1,275-101=1,174 Nt. Much closer to the control volume calculation. This is an important point: we cannot specify both the velocity and the pressure at the inlet, the problem would be over specified, we need to go through the full solution procedure in order to determine the pressure, or conversely, determine the velocity if a pressure_inlet condition is specified.
  2. Now look at velocity vectors, display>vectors, set scale to 4 and skip to 10. You can play with these settings and create a zoom window (by holding down the middle button) and identify a small recirculation region just after the 180 degree bend.

  1. Finally, we will look at the velocity profile halfway through the bend. Surface>line/rake, specify endpoints, x0 0.05 y0 0, x1 0.1255 y1 0. For this new suface name, label it “halfway_bend”, create, close.
  2. Plot>xy plot, plot direction x 1, y 0, velocity, velocity magnitude (or y velocity) and surface halfway_bend (de-select any other surface that may have already been selected), click plot, close. Note the maximum velocity (14.5 m/s) at the inner radius and the minimum velocity (5 m/s) at the outer radius, how is this (in conjunction with the pressure contour plot) responsible for causing a river to meander?

  1. TO TURN IN: make a plot or picture of anything else you are interested in looking at, like the velocity profile at some other position, a picture of something other than pressure, etc.