
[Sponsors] 
[GAMBIT] Meshing in Gambit for analysis of flow past cylinders 

LinkBack  Thread Tools  Search this Thread  Display Modes 
January 16, 2012, 04:25 
Meshing in Gambit for analysis of flow past cylinders

#1 
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 11 
Hello
What is the best computational domain to perform analysis of flow around circular cylinders in FLUENT?? Thanks in advance. 

January 16, 2012, 05:14 

#2 
Super Moderator


January 16, 2012, 05:28 

#3 
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 11 

January 16, 2012, 11:18 

#5  
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 11 
Quote:
Please elaborate bit on constructing. I will help me. I am new to CFD. Thanks in advance. 

January 16, 2012, 12:02 

#6 
Super Moderator

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. Last edited by Far; January 17, 2012 at 03:38. 

January 17, 2012, 02:40 

#7  
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 11 
Quote:
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 

January 17, 2012, 03:34 

#8 
Super Moderator

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. 

January 17, 2012, 11:25 

#9  
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 11 
Quote:
Thanks in advance. 

January 17, 2012, 11:40 

#10  
Super Moderator

Quote:
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 cfdonline users) Also check these linkes : https://confluence.cornell.edu/displ...+Specification https://confluence.cornell.edu/displ...+Specification 

January 18, 2012, 12:43 

#11  
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 11 
Quote:
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 58 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? 

January 18, 2012, 13:47 

#12 
Super Moderator

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.cfdonline.com/Forums/flu...oureward.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. 

January 18, 2012, 13:49 

#13  
Super Moderator

Quote:


January 19, 2012, 23:05 

#14  
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 11 
Quote:
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. 

January 21, 2012, 02:49 
Mesh is important factor

#15  
Super Moderator

Quote:
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) Quote:
Quote:
Quote:
Quote:
Use double precision solver. Last edited by Far; January 21, 2012 at 07:12. 

January 21, 2012, 07:45 

#16 
Super Moderator

I found some problem in mesh file. try new files upload here http://www.cfdonline.com/Forums/flu...tml#post340413
According to this reference (http://www.hitechprojects.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. Last edited by Far; January 21, 2012 at 13:44. 

January 23, 2012, 07:55 

#17  
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 11 
Quote:


January 23, 2012, 09:38 

#19 
Member
Mahindra
Join Date: Jan 2012
Posts: 59
Rep Power: 11 
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. 

January 23, 2012, 13:15 

#20  
Super Moderator

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.
Quote:
Last edited by Far; January 23, 2012 at 13:42. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
[ANSYS Meshing] Migrating from GAMBIT to ANSYS Meshing  DavidCFD  ANSYS Meshing & Geometry  1  April 1, 2011 06:22 
Flow past a sphere  Fabio  FLUENT  23  December 18, 2009 16:32 
Supersonic flow past a wedge with counter flow  Mahesh Bailakanavar  FLUENT  0  February 14, 2008 01:21 
incompressible free surface flow past cylinder  vineet  FLUENT  2  April 1, 2002 06:56 
beginning  Flow past a square cylinders  Odenir de Almeida  Main CFD Forum  4  February 10, 1999 10:38 