[cesarcg]

Harshal,

Try using dropbox to upload your file. Then share the link here with us.

Regards.

[Harshal]

Hello, all. I have shared the drop box link for the .tin file.

I have generated the mesh using Robust Octree method and this is the best result I have got so far as compared to other methods (like generating mesh with Octree, then deleting volume elements, laplace smoothing surface mesh, generating volume mesh with Delauney etc.)

Please have a look at the mesh and let me know how I can improve it.


https://www.dropbox.com/s/vw4xv29w8p...t_2%5B1%5D.tin

Thanks,

Harshal

[siw]

I've just opened your file and some quick points to note:

1. You could delete the front axel and remove the holes on the car and front wheels that it made. Minor point.
2. Reduce the triangulation tolerance by one order of magnitude.
3. Make OFRN bodies inside the car if using octree method.
4. Copy some points downstream of the car rear wheels and spoiler and make a Density Region.
5. Set all surface sizings to e.g. 0.25,0.5,1,2,4,8,16,32 etc as per octree power of 2 rule.
6. Lower the edge criterion to 0.01 because of the spoiler's sharp trailing edge.
7. Apply prisms on the road. But this will need to be looked at where it interfaces with the wheels. Would help if the wheels flattened on the road a bit.
8. Change some prism settings: float the prism layers (num of layers and total height = 0), min prism qual = 0.00001. Also
switch on Auto Reduction in the advanced prism options. Then split and re-distribute the prisms as per your y+ requirement.
9. The domain is still too small (except for the upstream extent).
10. If this is for a RANS simulation then a plane of symmetry would make it more efficient.

[Harshal]

Originally Posted by siw

I've just opened your file and some quick points to note:

1. You could delete the front axel and remove the holes on the car and front wheels that it made. Minor point.
2. Reduce the triangulation tolerance by one order of magnitude.
3. Make OFRN bodies inside the car if using octree method.
4. Copy some points downstream of the car rear wheels and spoiler and make a Density Region.
5. Set all surface sizings to e.g. 0.25,0.5,1,2,4,8,16,32 etc as per octree power of 2 rule.
6. Lower the edge criterion to 0.01 because of the spoiler's sharp trailing edge.
7. Apply prisms on the road. But this will need to be looked at where it interfaces with the wheels. Would help if the wheels flattened on the road a bit.
8. Change some prism settings: float the prism layers (num of layers and total height = 0), min prism qual = 0.00001. Also
switch on Auto Reduction in the advanced prism options. Then split and re-distribute the prisms as per your y+ requirement.
9. The domain is still too small (except for the upstream extent).
10. If this is for a RANS simulation then a plane of symmetry would make it more efficient.

Hi, siw,
thanks for your reply. I have followed most of your suggestion. However, I wanted to ask you why I need to create a prism layer on the road ? I want to only study the drag and downforce generated by the vehicle. At the moment, I 'm trying to generate volume mesh with perfectly round tyres. If that dosen't work, I'll have to 'flatten' the tyres.

Also, when I use 'auto reduction' option in Prism, it takes a LOT of time, to generate the prism layers. Is there any way around this ?
About the prism settings, you suggest that I should keep the no. of layers and total height as 0. Should I give initial height as the height required to get y+ of 1 (0.0000089) in my case ? And then should I split the prism into 12 layers ? I'm a bit confused. If I give the initial height and keep the no. of layers and total height as 0, will it even generate any prism layer ?

Also, I don't know if this will be a RANS simulation. Currently, I'm trying to generate a good mesh. After that, I'll simulate it in Fluent.

Thanks,

Harshal

[siw]

I don't know the requirements of your simulation so I simply was thinking that the road would be a no-slip surface and the correct boundary layer profile there would better represent a real surface (neglecting the roughness a real road has) and then that influence on to the flowfield around the lower and underside parts of the car. Since under the car the flowfield is being channeled between the road and car underside. Drag is difficult enough to predict so if it was me I would want to account (as best as possible considering the limitations of the chosen modelling method) the carry over effects of the road to the car. But if that may not be important to you forget it.

Check out these car/lorry mesh images from the Pointwise blog (http://blog.pointwise.com), they bunch cells at the road:

http://afinemesh.files.wordpress.com...-1920x1200.png
http://afinemesh.files.wordpress.com...volumemesh.png
http://afinemesh.files.wordpress.com...facemesh21.png

Refer to the presentations I hyperlinked in the posts above. Set initial height and total height = 0. Set a few layers (e.g. 7). Then split those layers (e.g so you get a total 30 layers) then redistribute them based on your desired first layer height which you stated above. You'll need to play about with this until you are happy.

You should know what modelling method you are going to use (RANS, SAS, DES, LES) before you start mesh generation because that will dictate how you go about making your mesh.

[Harshal]

Hello, all,
I am still trying to generate a volume mesh with prism layers and I'm having a LOT of troubles doing this. These are the following things that I tried:

1) Generate volume mesh with Robust octree, delete volume, Laplace smooth shell mesh, generate Delaunay mesh.
Problem: The Delaunay mesh generated is completely different to what I expect. (Image attached)
While generating prism there is a message 'attempting to use drawlib without opening window' and then 'prism terminated prematurely'

2) Generate Volume mesh by Robust Octree and then prism layers by giving the initial height, no. of layers and height ratio.

Problem: It takes a lot of time to generate. Also, on doing Check Mesh, there are various problems like Uncovered Faces, Non-Manifold Vertices, multiple edges etc which even after fixing do not seem to be solved.
By the way, how can one fix the Non-Manifold vertices problem ?

3) Generate volume mesh by Robust Octree, generate prism layers by giving initial height and total height as zero and number of layers as 2 or 3.
Then, splitting the no. of layers into 12 and redistributing w.r.t initial height.

Problem: Problem occurs in Fluent. It says Segmentation Violation
(This problem occurs always when using this approach i.e. splitting the prism layers and redistributing them)

It would be extremely helpful if anyone can help me in generating a volume mesh with prism layers.

Thanks,

Harshal

[Far]

Originally Posted by Harshal

Hi, siw, thanks for your reply.
1) How do I decrease the surface element size on the car? Do you mean that I should select every car surface, give an element size and then generate surface mesh ? Or should I give small element size in the 'Global mesh settings'? For the curvature feature I have turned on the 'curvature based proximity' option. Is there any other way ?

2) Could you please explain how to I can generate a mesh that grows gradually ? I also tried the 'Mesh density' option , but was unable to select the right points in 3D (For instance it is difficult to know where one point is w.r.t to car like is is above the car or below it). Is there any way around that ?

3) I tried a Y+ value of 1 with 12 layers. So, the prism layer is very thin. Do you think it would be better to use a higher Y+ value ? I don't know what range of Y+ values is acceptable in this case.

4) I tried both, patch dependent and path independent method. The patch independent method generates better surface mesh than patch dependent.

5) I'm not sure about the height of the box.

Currently, I am using the k-e standard model. Yes, I will upload the .tin file. But I can do that only tomorrow, not today.

Thanks, again,

Harshal

Hi Harshal
I have used all these steps with the patch independent along with size functions and density box. Keep in mind denaulay does not respect the surface density...

[Far]

You have to be careful to choose the part for the prism and please check all surfaces are in good connectivity and delete the unnecessary curves and merge surfaces to avoid sharp angles.

The the pic shown in your post suggest that you are using the denaulay algorithm on surface mesh either you got from patch dependent or from octree and mesh is leaking... I would different approach to mesh the outer boundaries...

just a teaser here...

[Harshal]

Originally Posted by Far

You have to be careful to choose the part for the prism and please check all surfaces are in good connectivity and delete the unnecessary curves and merge surfaces to avoid sharp angles.

The the pic shown in your post suggest that you are using the denaulay algorithm on surface mesh either you got from patch dependent or from octree and mesh is leaking... I would different approach to mesh the outer boundaries...

just a teaser here...

Hello Far,
Thanks a lot for your reply. Can you please explain in brief your approach (for the pictures you posted) ? As far as possible, I want to use automatic mesh generation tools since I have almost zero experience with blocking.

Also, I wanted to ask if there is any relation between the total prism height and the maximum size in Global Settings. A friend of mine told me that Total Prism Height = 0.1* Maximum size given in Global Settings. Is this true?

Thanks,

Harshal

[Far]

the surface mesh made from the surface blocking, converted into tris and smoothened and volume meshing was generated using denaulay. I dont think that prism hieght is calculated in this way...

[Harshal]

Originally Posted by Far

the surface mesh made from the surface blocking, converted into tris and smoothened and volume meshing was generated using denaulay. I dont think that prism hieght is calculated in this way...

Hello,
thanks for the quick reply. By the way, did you generate the above mesh in my file, that I shared here via drop box ? If yes, can you share it with me ? However, I cannot see the spoiler here.

Also, I tried to generate prism mesh by entering prism parameters (keeping the initial and total height zero) but there was an error- prism ended prematurely. Then I gave some value for total prism height and kept initial height zero. In this case, the software apparently generated the prism layers. However, I could not see the any mesh (shell or volume mesh). The volume mesh was also not listed in the tree. So, I did the whole mesh disappeared. Do you know the reason behind this and how I can solve it ?

Thanks again,

Harshal

[Harshal]

Hello all,
I have some doubts regarding mesh check and mesh quality.

1)Could someone please tell me how to fix errors like Surface Orientation and Non Manifold vertices. I usually create subsets for each and then delete them. However, this leads to other errors like Uncovered Faces and Single Edges. If I fix them, then again I get errors namely Surface Orientation and Non Manifold Vertices. So, I am stuck in a loop.
Is there anyway to fix the above errors without deleting the problematic elements ?

2) Is there anyway to delete particular elements (low quality elements) from the mesh ? When I check the mesh quality, and I get the bar chart displaying mesh quality, I would like to delete the cells which have low quality, witthout actually selecting each element individually from the mesh. Is there any way to do this ?

3) Also, is there any way to delete the prism layer. I mean just the prism layer, and not the entire volume mesh.

Thanks and Regards,

Harshal

[Harshal]

Hello all,
I need your help.
1) I have been trying to generate volume mesh with prism for quite some time now. Unfortunately, whenever I generate the prism layers, the mesh quality decreses drastically and I cannot use it in Fluent for simulations.

I have attached here a picture with bad quality volume cells. Can anyone, please, tell me how to smoothen these cells ? I have used the usual smoothing option but it's unable to improve mesh quality.

I used Robust Octree method. Then I created a few prism layers (around 8) keeping the initial height and total height zero. I had selected the 'auto reduction' option and reduced the acceptable prism quality to 0.000001.

The I splitted these prism layers into 30 layers w.r.t prism ratio of 1.5 and then, finally, redistributed these layers with initial height of 0.0000091 (coressponds to Y+ 1).

2) Also, in one of my other versions of the same model, I am getting an error that my Geometry has a Hole. I tried fixing it by selecting some curves, but the problem could nt be fixed. I have attached some images here and hope that someone can guide me through it.


I hope that someone here can help me to solve this problem since I have been stuck here for a while now.

Thanks and Regards,

Harshal

[Harshal]

Hello all,
I am simulating a car in wind tunnel. I have defined all the wind tunnel walls as stationary walls with no slip condition. I wanted to ask what should I defined for the car ? Should I defined it as stationary wall with no slip condition or with specified shear stress ? And what value should I give for shear stress (X component) ?

Thanks,

Harshal

[Far]

Thats great the you have generated the mesh successfully.

For wind tunnel you should define wall with zero shear stress (slip) and for car with no slip condition.

[Harshal]

Originally Posted by Far

Thats great the you have generated the mesh successfully.

For wind tunnel you should define wall with zero shear stress (slip) and for car with no slip condition.

Hi Far,
thanks for your reply. Actually. I haven't generated the prism layers as of now. I am trying to figure out whether the problems, which I mentioned above, are caused by prism layers or not. So, currently, I am simulating without prisms.

Thanks for your reply,

Harshal

[Harshal]

Hey Far,
I have a question. Is it possible to generate a part of mesh with unstructured method like Octree or Delauney and the other part with blocking ?
For instance can I try to generate a mesh by blocking the car but for difficult parts like the mirrors can I use Octree method ? Could you please give some suggestions in this approach ?

I have found out that my Tetras have very low quality, lower than the prism layers.

Awaiting your reply,

Thanks,

Harshal

[Harshal]

Hello all,
I have some questions regarding Fluent simulations for car aerodynamics.
I am using Fluent for studying drag and downforce on a car. I have to use two algorithms: k-omega and k-epsilon and compare the results.

I am right now following my friend's advice. He said first I need to do steady state simulations. When the first order solutions converge, then I should use nd order (Pressure, Turbulent energy, Momentum etc). When the second order converges, I should use this value as intial value for transient simulation.

However, the steady state converges only for 1st Order (I have tried only k-epsilon till now). For the 2nd order, the solution does not converge (even after 5000 iterations).

So, I wanted to ask:

1) Should I expect the 2nd degree to converge at all ? If not, how can I know when to switch to transient simulation ?

2) Also, when I do transient simulation, how can I decide the step size, no. of time steps and no. of iterations per time step ?

Thank You,

Harshal

[Harshal]

Hello all,
I recently completed my project work. This was my first experience with CFD and I thank you all for your help and guidance. Without your support, it would not have been possible for me to complete this project.

Thank You all, for your support !

Regards,

Harshal