[mahi007]

Originally Posted by 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.

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

Hello

Thank you for your concern. I did not work on it for past 4 days, as I had examinations. Today I tried again with your mesh. But it did not work.

In your mesh what is the cylinder wall? The innermost circle should be cylinder, right?
But the outermost concentric circles are taken as wall by FLUENT as your boundary conditions states that. You named them as "geom". Please clarify on that.

Also I have very limited experimental data with me at reynolds number 30, 40 etc. I am comparing drag coefficient to validate my results. Experimental value of cd at Re=40 is 1.8, but I am getting 6.5.

I am going terribly wrong with my circular domain (244X200). Any suggestions on how to get out this situation. I am using all default settings in solver while simulating this. Also, I never got vortices behind cylinder.

Regards
Mahindra

[Far]

That mesh has problems, you have just highlighted. Use the latest mesh http://www.4shared.com/rar/R7dSz2kw/...21_2012_2.htmlthere are no such walls in interior.

[mahi007]

Originally Posted by Far

That mesh has problems, you have just highlighted. Use the latest mesh http://www.4shared.com/rar/R7dSz2kw/...21_2012_2.htmlthere are no such walls in interior.

Your mesh working now after you have changed the interior wall. I got pair of vortices at Re=40, which I supposed to get. I got cd value of 1.54 which is within 10% of experimental value.

But the problem I am facing is on convergence criteria. When I ran FLUENT with default value of 0.0001 as criteria, I did not get vortices. Then I changed it to 0.00001 to all residuals, which have me some encouraging results with vortices in wake region. When I disabled check convergence criteria, solution never converged even after 8000 iterations. But cd value got converged to 1.5329.

Can you tell me how to approach this convergence criteria, I mean how to arrive at correct value??

Thank you

[Far]

For laminar flows I set the convergence criteria as (just out of habit)

1. If using absolute convergence criteria then 1e-18
2. Relative convergence (for transient flows) 1e-5

But the problem I am facing is on convergence criteria. When I ran FLUENT with default value of 0.0001 as criteria, I did not get vortices. Then I changed it to 0.00001 to all residuals, which have me some encouraging results with vortices in wake region. When I disabled check convergence criteria, solution never converged even after 8000 iterations. But cd value got converged to 1.5329.

This shows that you are studying the convergence sensitivity and you should mention this in your report as well. Normally in compressible and high mach number flows (Type of flows I usually deal with), convergence criteria of 1e-5 is good enough to get the solution independent of convergence criteria.

My advise would be to study the convergence behavior and plot Cd as function of this criteria (make a graph in excel) so that you get idea what should be convergence criteria in your case.


You are getting Cd as 1.5329 and experimental value is 1.8 (14% error), you need to refine the mesh further (in addition to above discussion) or some other parameters e.g. extent of domain on downstream side.


PS. In Fluent 13 I usually setup the case for similar problems as :

1. Coupled pressure solver with Courant number 1e5 to 1e06
2. All schemes with 2nd order accuracy
3. Hybrid initialization or some times patch initialization (for transient case)

[mahi007]

Originally Posted by Far

For laminar flows I set the convergence criteria as (just out of habit)

1. If using absolute convergence criteria then 1e-18
2. Relative convergence (for transient flows) 1e-5



This shows that you are studying the convergence sensitivity and you should mention this in your report as well. Normally in compressible and high mach number flows (Type of flows I usually deal with), convergence criteria of 1e-5 is good enough to get the solution independent of convergence criteria.

My advise would to study the convergence behavior and plot and Cd as function of this criteria (make a graph in excel) so that you get idea what should be convergence criteria in your case.


You are getting Cd as 1.5329 and experimental value is 1.8, you need to refine the mesh further (in addition to above discussion) or some other parameters e.g. extent of domain on downstream side.

PS. In Fluent 13 I usually setup the case for similar problems as :

1. Coupled pressure solver with Courant number 1e5 to 1e06
2. All schemes with 2nd order accuracy
3. Hybrid initialization or some times patch initialization (for transient case)

Thank you for your quick reply. I did all these simulations using your mesh and I think you made it in ICEM. Also I would like to know whether I can open that mesh in Gambit to make necessary changes.

[Far]

No. You can not edit this in gambit, you need ICEM for this.

But I can guide you to build similar mesh in gambit. Or if you need I can further refine this mesh and extend the domain and upload again.

[mahi007]

Originally Posted by Far

No. You can not edit this in gambit, you need ICEM for this.

But I can guide you to build similar mesh in gambit. Or if you need I can further refine this mesh and extend the domain and upload again.

Ok. Then give me guidelines to build mesh in gambit. As I am starter, it will help me learn better.

Thanks

[mahi007]

Originally Posted by Far

No. You can not edit this in gambit, you need ICEM for this.

But I can guide you to build similar mesh in gambit. Or if you need I can further refine this mesh and extend the domain and upload again.

One of my friends working with ANSYS. ICEM is working on his system. I can refine your mesh in that. I dont have much experience in ICEM. To refine mesh, I have to go to edit mesh--> Adjust mesh density--> Refine/Coarse mesh option, right?

Also I can refine in steps of 1. Is it necessary to refine whole mesh or only selected elements?

Thank You

[mahi007]

Originally Posted by Far

No. You can not edit this in gambit, you need ICEM for this.

But I can guide you to build similar mesh in gambit. Or if you need I can further refine this mesh and extend the domain and upload again.

Better give me directions to refining mesh and extending domain in ICEM. It will be easy and helpful

Thanks

[Far]

One of my friends working with ANSYS. ICEM is working on his system. I can refine your mesh in that. I dont have much experience in ICEM. To refine mesh, I have to go to edit mesh--> Adjust mesh density--> Refine/Coarse mesh option, right?

Also I can refine in steps of 1. Is it necessary to refine whole mesh or only selected elements?

You can refine in this way as well. No it is not necessary to do so, you just need to refine the mesh in important areas e.g. wake. Another method is from blocking tab. You can go to pre mesh settings and select the edge and increase no. of nodes.
After making these chagnes,
1. go to pre mesh (left pan)
2. right click and update
3. Convert to unstructured mesh
4. Output mesh.

[mahi007]

Originally Posted by Far

You can refine in this way as well. No it is not necessary to do so, you just need to refine the mesh in important areas e.g. wake. Another method is from blocking tab. You can go to pre mesh settings and select the edge and increase no. of nodes.
After making these chagnes,
1. go to pre mesh (left pan)
2. right click and update
3. Convert to unstructured mesh
4. Output mesh.

I am finding it difficult to refine from blocking tab. I am doing it in following way. Let me know if I am doing anything wrong.

First going to blocking tab--> Pre Mesh Parameters--> Refinement

There I am selecting the 8 blocks you have made around cylinder wall. Selecting refinement directions all. Still mesh is not getting refined, but I am getting result refinement done.

Help me.

Also while writing .msh file, what are options I have to choose, I mean Scaling factors, Write binary file etc

Thanks

[Far]

since pre mesh is not visible in left pan, therefore you can not see the effect of refinmnet command. Turn on pre mesh and turb off shells in mesh. After refining the mesh, right click on premesh and update and convert to unstructured mesh. After that you can out put the mesh.

[mahi007]

Originally Posted by Far

since pre mesh is not visible in left pan, therefore you can not see the effect of refinmnet command. Turn on pre mesh and turb off shells in mesh. After refining the mesh, right click on premesh and update and convert to unstructured mesh. After that you can out put the mesh.

I am sorry, I am not able to refine it properly. I am selecting pre mesh option which I can see under blocking in left pan. When I select it, it is saying that mesh is outdated and need to recompute. When I clicked yes, something is going wrong and whole mesh is getting weird. As you only made it, can you kindly step by step procedure to refine mesh in whatever places I want.

Also I am selecting the blocks around cylinder for refinement. Is it correct to do?

Thanks

[mahi007]

Originally Posted by Far

since pre mesh is not visible in left pan, therefore you can not see the effect of refinmnet command. Turn on pre mesh and turb off shells in mesh. After refining the mesh, right click on premesh and update and convert to unstructured mesh. After that you can out put the mesh.

Also I refined whole mesh using adjust mesh density command and then used in FLUENT. Cd value converged to 1.5845. Convergence as if it never changed after reaching to this value. Earlier when I used mesh without any refinement it converged to 1.5329. Experimental value is 1.8. Does it means I have to refine further more?

[Far]

http://www.4shared.com/rar/dwx89ip_/...an29_2012.html

Download above files.

I am facing this problem in icem:

1. I created two additional circles of dia 3 and 7 in order to make the blocking in the boundary layer and important flow regions (got highly orthogonal mesh) and associate two o-block edges to these circles and got pretty good mesh. But I got the walls in interior. Is there any method so that the temporary circles (wall) do not include in the final mesh?

2. When removed these circles, the above problem was resolved but when edited by mahi007 (later checked by myself) the pre-mesh is distorted. This is logical since there is no geometry where edges can be projected.

3. Again I have recreated the circles to associate two O-blocks and this time I set the boundary condition for these circles (walls) as interior in ICEM and did not get any wall in Fluent. But this time I got two interior zones. Is there any method so that I neither get the walls nor two interior zones.

[Far]

yeah this shows that results are still sensitive to mesh. Refine mesh further.

[mahi007]

Originally Posted by Far

http://www.4shared.com/rar/dwx89ip_/...an29_2012.html

Download above files.

I am facing this problem in icem:

1. I created two additional circles of dia 3 and 7 in order to make the blocking in the boundary layer and important flow regions (got highly orthogonal mesh) and associate two o-block edges to these circles and got pretty good mesh. But I got the walls in interior. Is there any method so that the temporary circles (wall) do not include in the final mesh?

2. When removed these circles, the above problem was resolved but when edited by mahi007 (later checked by myself) the pre-mesh is distorted. This is logical since there is no geometry where edges can be projected.

3. Again I have recreated the circles to associate two O-blocks and this time I set the boundary condition for these circles (walls) as interior in ICEM and did not get any wall in Fluent. But this time I got two interior zones. Is there any method so that I neither get the walls nor two interior zones.

What is problem having two interior zones instead of one?
Will it make any difference to results?
Can you provide me with the mesh with above correction made?

Thanks

[Far]

What is problem having two interior zones instead of one?
No problem, but this should not happen
Will it make any difference to results?
No
Can you provide me with the mesh with above correction made?
It is already uploaded in my previous post

[Far]

Mesh file is here. Same as previous one, no refinement.
http://www.4shared.com/rar/7Q6zQBgQ/fluent.html

[mahi007]

Originally Posted by Far

Mesh file is here. Same as previous one, no refinement.
http://www.4shared.com/rar/7Q6zQBgQ/fluent.html

Hello

Sorry, I mean I want entire project files, not only mesh. In previous post you attached does not have .uns files and most others. It has only 3 files which has all edges. I mean when I opened that in ICEM, I can only see edges you made.

I want entire package after you made correction (Pre mesh distortion).

Thanks