[mahi007]

Hello

What is the best computational domain to perform analysis of flow around circular cylinders in FLUENT??

Thanks in advance.

[Far]

Originally Posted by mahi007

Hello

What is the best computational domain to perform analysis of flow around circular cylinders in FLUENT??

Thanks in advance.

Rectangle, Circular

[mahi007]

Originally Posted by Far

Rectangle, Circular

Thank you for reply. Can you suggest me how to construct geometry for circular domain?

Thanks in advance

[Far]

similar to your smaller circle with at least 60*diameter of smaller circle

[mahi007]

Originally Posted by Far

similar to your smaller circle with at least 60*diameter of smaller circle

Thank You. My problem is I am not able to mesh the annular space properly. I want to mesh the space by concentric circles and radial lines and I need more finer mesh near wall of cylinder.

Please elaborate bit on constructing. I will help me. I am new to CFD. Thanks in advance.

[Far]

Ok. Make a smaller circle (1D) and one larger circle (60D). Now use the edge split command and split by with parameter value of .5. Now you get the two curve for each circle. again apply edge split on all these four edges. Now join the corresponding vertices by making the straight edge. Now go to face command and select the four edges of each quarter circle and you get the four faces.

Now go to edge meshing panel and mesh the edges of circumference of both circles (8 edges in total) and then mesh the radial edges with ratio (1.15 or 1.2) and required spacing (0.001 or less depending on the requirements) and then go to face mesh command and now you are done.
At the end dont forget to specify the correct boundary conditions. make the half circle at front as pressure inlet/pressure farfield and at outlet as pressure outlet and smaller circle as wall.

[mahi007]

Originally Posted by Far

Ok. Make a smaller circle (1D) and one larger circle (60D). Now use the edge split command and split by with parameter value of .5. Now you get the two curve for each circle. again apply edge split on all these four edges. Now join the corresponding vertices by making the straight edge. Now go to face command and select the four edges of each quarter circle and you get the four faces.

Now go to edge meshing panel and mesh the edges of circumference of both circles (8 edges in total) and then mesh the radial edges with some ratio (1.15 or 1.2) and some spacing (0.001 or less depending on the requirements) and then go to face mesh command and now you are done.
At the end dont forget the specify the correct boundary conditions. make the half circle at front as pressure inlet/pressure farfield and at outlet as pressure outlet and smaller circle as wall.

Thank you for explanation. I did everything as you said. But the problem is I am getting weird results. I am using Velocity inlet boundary condition for front half of circle and Outflow condition for rear half. This is because I want the flow parameters for a particular reynolds number. When I see the stream lines, they are nothing but bunch of parallel lines in the annular space. Can you please tell me where I am going wrong.

Thanks in advance

[Far]

instead of outflow use pressure outlet. Whats Reynolds number? instead of streamlines plot vecotr and check the pressure and velocity contours. Could you post some pics? Are you interested in steady state or you think flow is steady?
Questions related to solution (Fluent or CFX) may please be posted in the relavant forum.

[mahi007]

Originally Posted by Far

instead of outflow use pressure outlet. Whats Reynolds number? instead of streamlines plot vecotr and check the pressure and velocity contours. Could you post some pics? Are you interested in steady state or you think flow is steady?
Questions related to solution (Fluent or CFX) may please be posted in the relavant forum.

I am simulating for velocity corresponding to reynolds number 30. I used pressure outlet instead of outflow. How to decide choosing between them? Also I did not get great results, may be I am doing some basic mistake if I am correct. I am attaching a figure below showing velocity vectors. Regarding operating conditions, how should I choose reference pressure location? By default it is keeping origin, but It did not make any sense in my case as point lies inside cylinder. So I change it to (0,1). Also I am using density and viscosity values of FLUENT which it provides by default: density=1.225, viscosity= 1.789e-05 for air. My pressure outlet conditions are guage pressure=0

Thanks in advance.

[Far]

Originally Posted by mahi007

I am simulating for velocity corresponding to reynolds number 30. I used pressure outlet instead of outflow. How to decide choosing between them? Also I did not get great results, may be I am doing some basic mistake if I am correct. I am attaching a figure below showing velocity vectors. Regarding operating conditions, how should I choose reference pressure location? By default it is keeping origin, but It did not make any sense in my case as point lies inside cylinder. So I change it to (0,1). Also I am using density and viscosity values of FLUENT which it provides by default: density=1.225, viscosity= 1.789e-05 for air. My pressure outlet conditions are guage pressure=0

Thanks in advance.

First of all, the results are correct from qualitative point of view. Keep the default values in operating pressure panel.
What is value of velocity you are setting in velocity inlet panel. I recommend to use density 1 kg/m3, velocity 1 m/sec and dia = 1 m (already from geometry, so no need to worry) and then calculate the value of viscosity from the Re no.
What type of flow is there at this very low Reynolds number? Is there any vortex shedding (transient flow) at Re= 30 and whats the strouhal no. in literature for this Re? Try to compare your values to literature. Check the mesh sensitivity, time step dependency, domain extent sensitivity. You need to run the case for long enough time. You also need to apply the FFT to extract the frequency.
Post a pic of mesh with and without zooming of small cylinder. How many no of nodes are there?

I have very good quality mesh created in ICEM and may share the tin and topology files (Search the forum, I did it already for cfd-online users)

Also check these linkes :
https://confluence.cornell.edu/displ...+Specification
https://confluence.cornell.edu/displ...+Specification

[mahi007]

Originally Posted by Far

First of all, the results are correct from qualitative point of view. Keep the default values in operating pressure panel.
What is value of velocity you are setting in velocity inlet panel. I recommend to use density 1 kg/m3, velocity 1 m/sec and dia = 1 m (already from geometry, so no need to worry) and then calculate the value of viscosity from the Re no.
What type of flow is there at this very low Reynolds number? Is there any vortex shedding (transient flow) at Re= 30 and whats the strouhal no. in literature for this Re? Try to compare your values to literature. Check the mesh sensitivity, time step dependency, domain extent sensitivity. You need to run the case for long enough time. You also need to apply the FFT to extract the frequency.
Post a pic of mesh with and without zooming of small cylinder. How many no of nodes are there?

I have very good quality mesh created in ICEM and may share the tin and topology files (Search the forum, I did it already for cfd-online users)

Also check these linkes :
https://confluence.cornell.edu/displ...+Specification
https://confluence.cornell.edu/displ...+Specification

Hello

Thanks a lot. It worked. I do not have experimental results right now. But I got some reasonable values. I got pressure force value of 0.483 at reynolds number of 30. At this reynolds number there wont be any vortex shedding. it is steady laminar flow. I meshed cylinder with 120 points on circumference of circle along with 144 radial circles with first length 0.0002.

While plotting pressure cf with direction vector, I am getting only values at 5-8 points. Is mesh too coarse to get many points?
Also in reference values, should I use projected area(like 1 m2 for cylinder of diameter 1) or cylinder area?

[Far]

Mesh seems to be fine enough, however, I would recommend to increase the no of nodes in radial direction by factor of 1.5 and also reduce the near wall distance by factor of 2 initially. Make these changes in two steps so that you can get the flavour of any change. Also try the mesh created for cylinder of dia 1 m in this post http://www.cfd-online.com/Forums/flu...ou-reward.html
Reference value of 1 m2 is OK. What I am thinking (I am not clear about this) is the ideal gas law which states P=rho*R* Temperature. I shall discuss this aspect in detail in next post.

[Far]

While plotting pressure cf with direction vector, I am getting only values at 5-8 points. Is mesh too coarse to get many points?

I suggest you to plot the pressure coefficient w.r.t angle, in this way you will get values on all 120 nodes along circumference.

[mahi007]

Originally Posted by Far

Mesh seems to be fine enough, however, I would recommend to increase the no of nodes in radial direction by factor of 1.5 and also reduce the near wall distance by factor of 2 initially. Make these changes in two steps so that you can get the flavour of any change. Also try the mesh created for cylinder of dia 1 m in this post http://www.cfd-online.com/Forums/flu...ou-reward.html
Reference value of 1 m2 is OK. What I am thinking (I am not clear about this) is the ideal gas law which states P=rho*R* Temperature. I shall discuss this aspect in detail in next post.

I refined mesh a bit with 200 radial points and 244 concentric circles. Also in previous posts you suggested me to check the mesh sensitivity, time step dependency, domain extent sensitivity. How to do these tests?

Also when I change the density and viscosity values for a particular Reynolds number as you have suggested, Should I also change values in Reference values panel?

Also I am not getting an option including angle while plotting XY plot for pressure cf along cylinder surface.

How to obtain strouhal frequency once vortex shedding starts?

The domain I am using converging at only 200 iterations. Is that alright? or any problem? Because when I ran with the mesh you created, the residuals are oscillating and they are not converging even after 2500 iterations.

Help me. Thank you.

[Far]

I refined mesh a bit with 200 radial points and 244 concentric circles. Also in previous posts you suggested me to check the mesh sensitivity, time step dependency, domain extent sensitivity. How to do these tests?

First domain extend: Either take these values from good paper or try: 10 dia upstream and 20 dia downstream, 15 dia up and 30 down and 20 dia up and 40 down. or may be 25 up and 35 down as taken in this post http://www.cfd-online.com/Forums/flu...ou-reward.html. You should understand the basic idea, which is to avoid the reflections from the boundaries.

Mesh Sensitivity This can done by refining the mesh size by factor of 1.44 in each direction (that is equivalent to doubling the overall mesh size). Create at least three meshes and then compare the important parameters and if you see that values between two meshes are not changing then you have achieved the mesh Independence and you can use the mesh with less no of nodes from these two grids.

Time step This depends upon the frequency of vortex shedding. The frequency of vortex shedding can be determined from the Strouhal no for that particular Reynolds no. See this Fig. and this one http://en.wikipedia.org/wiki/File:Srrrpd.png

Strouhal no. is defined as
where St is the dimensionless Strouhal number, f is the frequency of vortex shedding, L is the characteristic length (for example hydraulic diameter) and V is the velocity of the fluid [Ref :http://en.wikipedia.org/wiki/Strouhal_number

From this formula you can get the idea of the shedding frequency (be careful: You need to calculate the Strouhal no. from the shedding frequency found from the FFT (see below) and compare to experimental St no. For all three meshes to see what is happoing while refining the meshes with this important parameter) For example if St no. is 0.18 and velocity is 1 m/s and L = 1 m. Therefor shedding frequency is 0.18 and time to pass one frequency is

Now you decide in how many time steps you want the reach this time. For example if you take 25 steps then your time step would be 0.22. This imply you are resolving one cycle in 25 steps ( 25*.22 = 5.5 seconds).
You may start with 25 steps and double for each time step sensitivity analysis. This look like time step = .22 (25 time steps) , 0.11 (50 time steps) and 0.055 (100 time steps)

Also when I change the density and viscosity values for a particular Reynolds number as you have suggested, Should I also change values in Reference values panel?

Yes.

Also I am not getting an option including angle while plotting XY plot for pressure cf along cylinder surface.

Create points along the periphery of circle with the interval of 5 deg (or less depending upon the resolution requirements) and then get the values on these points. For this use surface integral and apply vertex averaging.

How to obtain strouhal frequency once vortex shedding starts?

Use the lift coefficient graph and then take the FFT available in Fluent. From that graph the dominate frequency is the shedding frequency and strouhal no. can be found from the above formula. OR create the point at some downstream point (may be at x= 1.5 and Y = 0.5) and create surface monitor (Choose velocity as variable and apply vertex averaging) and apply FFT on these values. Caution: Do not change any parameter when recording these files other wise data may not valid for FFT analysis.

The domain I am using converging at only 200 iterations. Is that alright? or any problem? Because when I ran with the mesh you created, the residuals are oscillating and they are not converging even after 2500 iterations.

This may be due to the fact that your mesh is not capturing the vortex shedding and therefore you are getting the converged steady state solution, while other mesh is capturing the vortex shedding and hence giving you the oscillating steady solution, which clearly shows that you need to run this case as transient.

Use double precision solver.

[Far]

I found some problem in mesh file. try new files upload here http://www.cfd-online.com/Forums/flu...tml#post340413

According to this reference (http://www.hitech-projects.com/eupro...er%20flows.pdf) the flow for Reynolds number 30 is steady with two sysmetrical vortices, therefore both steady and transient simulations should give you the same answer.

[mahi007]

Originally Posted by Far

I found some problem in mesh file. try new files upload here http://www.cfd-online.com/Forums/flu...tml#post340413

According to this reference (http://www.hitech-projects.com/eupro...er%20flows.pdf) the flow for Reynolds number 30 is steady with two sysmetrical vortices, therefore both steady and transient simulations should give you the same answer.

I never go any vortices in the wake region using my circular domain. Also the flow was smooth without any separation. Can you tell me where I am going wrong?

[Far]

did you get any vortices in the another mesh I have just uploaded?

[mahi007]

Originally Posted by Far

did you get any vortices in the another mesh I have just uploaded?

No I did not get any vortices with your mesh. The flow is smooth rejoining at back of cylinder. Also I got drag coefficient of 6.9 which is more than experimental value.

Between do you have any experimental data regarding this flow around circular cylinder? If you know, kindly pass it to me, as I am finding it difficult to get data.

[Far]

Well the literature I have, mostly deals with Reynolds number higher than 100. In reference, attached above, just describe the flow for different regimes without giving much details.

No I did not get any vortices with your mesh. The flow is smooth rejoining at back of cylinder. Also I got drag coefficient of 6.9 which is more than experimental value.

http://www.princeton.edu/~asmits/Bicycle_web/blunt.html