[vhcongtltd]

Hello,

I try to calculate the drag force coefficient on cylinder in case with oscillating flow at inlet boundary. i.e U=Uosin(2pi*f*t)

How to set velocity in Reference values?
any ideas ?

Thank you

[Maimouna]

Hi,

I'm also looking for the same question. Could you find the answer?

Thanks and regards.

Maimouna

[vhcongtltd]

Sorry, I did not figure out yet. How about you?

[Maimouna]

Sorry, not yet too. Which type of oscillating are you doing: forced or natural?

[vhcongtltd]

Originally Posted by Maimouna

Sorry, not yet too. Which type of oscillating are you doing: forced or natural?

I put oscillating flow at inlet boundary. i.e U=Uosin(2pi*f*t). I plan to use a wave at inlet boundary. Do you have any idea?
Thank

[Maimouna]

Unfortunately, I don't know what you exactly mean, if you are interested you case google ''how to accurately flow around cylinder'' there are some attached folders might help.

All the best.

[Rayder]

Hello everyone
If anyone can help me to simulate the problem attached using Ansys, and if you can explain how I can treat with the roughness parameter, please I need it in my project, and that will be so helpful. I have been working on it too may time but it gave me a different results than the analytic solution especially with the friction part. Please if you can contact me with my E-mail that will be so nice of you.
Haider_skran@yahoo.com
2.jpg

[ghost82]

Originally Posted by Rayder

Hello everyone
If anyone can help me to simulate the problem attached using Ansys, and if you can explain how I can treat with the roughness parameter, please I need it in my project, and that will be so helpful. I have been working on it too may time but it gave me a different results than the analytic solution especially with the friction part. Please if you can contact me with my E-mail that will be so nice of you.
Haider_skran@yahoo.com
Attachment 33980

Hi, this is off topic, however...
I think you need to take care on 2 things in this problem:

1- you have a developed flow: this means the fluid is fully developed, so in fluent you need to write an udf to have a fully developed flow at the inlet (there is an example in udf manual, velocity inlet + k + epsilon (<--turbulent dissipation)); otherwise, you can make the pipe longer, monitor the velocity profile in the axial direction, identify where the fluid fully develops, and start your calculations (pressure drop, etc.) from that point.
Outlet boundary should be set to outflow, because the fluid is fully developed.

2- Roughness parameter: the Moody's chart was obtained by coating the internal surfaces of tested pipes with a monolayer of sand, and the pipe wall roughness was defined as the average diameter of the sand grains (epsilon); the sentence "the roughness of stainless steel is 0,002 mm" is quite ambiguous: which roughness? I think this refers to that of the Moody's chart, so you can input directly this value into the fluent "roughness heigh" box (take care to units). Roughness constant is a parameter of the uniformity of sand grains: a value of 0,5 means all the grains are of equal diameter, so I think you should set this value to 0,5.

Several algorithms were developed to link various roughness to the sand grain roughness, I usually use the followings:

epsilon=Ra*5,863
epsilon=Rrms*3,100
epsilon=Rzd*0,978

epsilon=sand grain roughness
Ra=average roughness (this is the average value of the heights, + or -, measured from a mean line of a profile)
Rrms=root mean squared roughness
Rzd=peak to valley roughness

Daniele

[ghost82]

Originally Posted by vhcongtltd

Hello,

I try to calculate the drag force coefficient on cylinder in case with oscillating flow at inlet boundary. i.e U=Uosin(2pi*f*t)

How to set velocity in Reference values?
any ideas ?

Thank you

I think you should create an udf to calculate the drag coefficent with variable velocity inlet.
You should investigate about how to calculate the drag force;
Maybe you could use:
- for pressure forces: F_P(f,t1) * A[0]
where F_P is the face pressure and A[0] is the projected area in x direction;
- for viscous forces: F_STORAGE_R_N3V(f,t1,SV_WALL_SHEAR)[0]
this is not documented in udf manual;

Then you should add:
Domain *d = Get_Domain(1); to get domain pointer, which should be 1, as you have only 1 phase;
Thread *t1 = Lookup_Thread(d,xxx); where xxx is the id of the wall of the cylinder (you read it in the fluent gui)

Once you have the total force (pressure+viscous), you can easily compute the drag coefficient with time varying velocity.

Daniele

[Rayder]

First of all I would like to thank you Daniele
I have done what you said , but I did not get the results that I looking for , If you can simulate the problem that will be so helpful

[ghost82]

Rayder,
you have 2 posts on cfd-online, I will not simulate your problem and nobody on this forum will do it for you.
Describe what you have done, you didn't describe anything about your setup, and I will help you with suggestions.