CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLOW-3D (http://www.cfd-online.com/Forums/flow-3d/)
-   -   simulating flow (http://www.cfd-online.com/Forums/flow-3d/108241-simulating-flow.html)

pyxbird October 17, 2012 20:39

simulating flow
 
Dear all,
Hi, I am simulating flow in a water channel, my input velocity is 26.67cm/s, the inlet boundary is "specified velocity", the outlet is "continuative", the initial speed of the fluid is zero, when I run the simulation it doesn't work? However, when I change the initial velocity into 26.67cm/s, the simulation runs normally and 6 seconds later the flow became steady, but the output turns out to be unreasonable. Along z direction most of the velocity is 26.67cm/s, so anyone can help me find out where is wrong?

JBurnham October 22, 2012 12:41

Probably you are either using inviscid flow, not specifying a wall boundary at z-min (symmetry is free-slip condition), or do not have gravity activated. Unless there is a wall-boundary or solid no-slip component at the bottom of the channel, and unless at least laminar viscous flow is activated, then there is no zero-slip and thus no velocity profile. Also try to use at least 8 - 12 cells in z-direction to resolve the profile.

pyxbird October 22, 2012 19:48

2 Attachment(s)
Quote:

Originally Posted by JBurnham (Post 387935)
Probably you are either using inviscid flow, not specifying a wall boundary at z-min (symmetry is free-slip condition), or do not have gravity activated. Unless there is a wall-boundary or solid no-slip component at the bottom of the channel, and unless at least laminar viscous flow is activated, then there is no zero-slip and thus no velocity profile. Also try to use at least 8 - 12 cells in z-direction to resolve the profile.

Sorry for my poor introduction of my flow model but I am very glad that you can send me your advice, here I provide a more detailed information about my model: the computating time is 50s, gravity is activated, newton viscosity, wall boundary at z-min, no free-slip, RNG turbulence, x-direction 3500cells for 7 meters, z-direction 50 cells for 10cm, the velocity of the inlet boundary is 26.67cm/s, the outlet "continuative", the depth of the water is 7.5cm, I try many times, but the velocity profile is bad, and I will show the picture by the attachment. This time the flow just can not become steady. All the two pictures shows the velocity profie at x=6.5 meter, Picture 1 is for the t=30seconds, and picture 2 is for t=50s, both of the outcome is weird, but I just can not figure out where is wrong.

JBurnham October 23, 2012 10:55

The velocity profile appears to be similar to a logarithmic velocity profile. I guess I don't see the problem. It starts low, near the wall (although the cells are not small enough to see it go close to zero), and increases as depth increases, with a characteristic curve. Then at the free surface it goes to zero again, which is to be expected. How is it not accurate? Do you have data to compare it to, or an expected solution (like a logarithmic profile)?

pyxbird October 23, 2012 19:45

1 Attachment(s)
Quote:

Originally Posted by JBurnham (Post 388133)
The velocity profile appears to be similar to a logarithmic velocity profile. I guess I don't see the problem. It starts low, near the wall (although the cells are not small enough to see it go close to zero), and increases as depth increases, with a characteristic curve. Then at the free surface it goes to zero again, which is to be expected. How is it not accurate? Do you have data to compare it to, or an expected solution (like a logarithmic profile)?

Hi, Jburnham, I am not satisfied with the outcome for two main reason:
1.running 50seconds, the flow is still unsteady(the profile still chages) at last
2.it differs greatly from the data given by the experiment, at the top of the profile the velocity is the max velocity which can reach nearly 36cm/s
And I will show the velocity profile from the experiment

pyxbird October 23, 2012 23:33

1 Attachment(s)
Quote:

Originally Posted by JBurnham (Post 388133)
The velocity profile appears to be similar to a logarithmic velocity profile. I guess I don't see the problem. It starts low, near the wall (although the cells are not small enough to see it go close to zero), and increases as depth increases, with a characteristic curve. Then at the free surface it goes to zero again, which is to be expected. How is it not accurate? Do you have data to compare it to, or an expected solution (like a logarithmic profile)?

Dear JBurnham,
this time I use another computer(better one) to simulate the flow,and I find that:1.the flow is steady now 2.the problem still exist:the max velocity(at the surface of the water) is about 27cm/s, can not reach about 39cm/s which is given by the experiment
And I will add the velocity profile below.

pyxbird October 23, 2012 23:57

2 Attachment(s)
Quote:

Originally Posted by JBurnham (Post 388133)
The velocity profile appears to be similar to a logarithmic velocity profile. I guess I don't see the problem. It starts low, near the wall (although the cells are not small enough to see it go close to zero), and increases as depth increases, with a characteristic curve. Then at the free surface it goes to zero again, which is to be expected. How is it not accurate? Do you have data to compare it to, or an expected solution (like a logarithmic profile)?

Dear JBurnham,
Sorry for my carelessness, I find another problem: the water level exceeds 8cm( experiment 7.5cm) most of the time ,especially at the beginning of the simulation, at the inlet boundary the water level even reaches 9cm, I check the velocity boundary, the fluid height I input is 7.5cm, the oulet boundary is also 7.5cm, but why it turns out to be like this, and how shall I solve this problem? In other words, does it influence the velocity profile directly? Or is it the reason the max velocity can not reach 39cm/s? I will show the surface pictures below.

JBurnham October 24, 2012 11:30

You should be running this as a one-fluid, free-surface type problem. You should also initialize the fluid depth and velocity at t = 0, to match the boundaries. Upstream boundary should be velocity-type, downstream boundary should be pressure-type if the flow is sub-critical Fr < 1, or Outflow type if the flow is super-critical Fr > 1. It looks like you're modeling 2-fluids simulataneously, and this will diffuse the free surface and result in incorrect velocity profiles.


All times are GMT -4. The time now is 03:53.