[Harshal]

Hello all,
I have recently undertaken a project in vehicle aerodynamics. I have already generated a mesh in ICEM and have simulated the flow in Fluent. Unfortunately, the 'scaled residuals' in Fluent are never steady and vary even after a large number of iterations. When I searched for a solution for this problem, I came across a post stating that for vehicle aerodynamics, a Y+ value of 40-50 while meshing is advisable, to get correct results.

My question is :
How can I implement the Y+ value in ICEM ? There are options in 'Prism' command like 'Height', 'Height ratio' etc. What should I input to get Y+ of 40 or 50 ?

Also, I tried to calculate the wall distance using the Y+ estimation calculator. I have given the velocity of car as 'Free stream velocity'. However, I am not sure about the 'Boundary Layer Length' option. What should I input there ? The car length ?

Thanks and Regards,

Harshal

[blazejpop]

I don't know if you can do this in ICEM, but definitely you can in Fluent.

[siw]

Yes, you need to calculate a suitable first prism height outside of ICEM, based on your target y+ (and a few other parameters) which can be done with the calculator here at CFD-Online.

If you are not sure on the length to use then just use the car length as you say and run the simulation as see what you get. If it's not what you want then try something else.

Also the use of a y+ from 40-50 will use a wall-function approach. If you want to accurately predict the boundary layer for, say the drag, you'll want a y+ of about 1.

You'll find these Tips-n-Tricks from LEAP Australia useful for these types of questions: (http://www.computationalfluiddynamic...ps-and-tricks/).

[Harshal]

Originally Posted by siw

Yes, you need to calculate a suitable first prism height outside of ICEM, based on your target y+ (and a few other parameters) which can be done with the calculator here at CFD-Online.

If you are not sure on the length to use then just use the car length as you say and run the simulation as see what you get. If it's not what you want then try something else.

Also the use of a y+ from 40-50 will use a wall-function approach. If you want to accurately predict the boundary layer for, say the drag, you'll want a y+ of about 1.

You'll find these Tips-n-Tricks from LEAP Australia useful for these types of questions: (http://www.computationalfluiddynamic...ps-and-tricks/).

Hello Siw,
thank you for your reply. I have calculated the wall distance using th Y+ Estimator available here, and have got a distance of 2.7e^-4.
So, my question is, where do I enter this value in the 'Prism' option in ICEM ? Should I give this value for 'maximum size', 'height' or 'height ratio' ?

Also, can I generate an inflation in the mesh ? I mean I have defined a global mesh size which is quite coarse. Now, I'll generate a prism layer, which will produce a fine mesh of 3-4 layers. Can I adjust the transition between the mesh size so that after the prism layer (fine mesh), there will be a less fine mesh and finally a coarse mesh defined by the global size ?
Or does giving the Y+ means that we are adjusting the transition from fine prism mesh to global mesh size ?

Also, thanks for the link. It looks very useful and I'll certainly go through it.

Thanks, again,

Harshal

[siw]

Your distance of 2.7e^4 will be the initial height in ICEM. Then you can enter a number of layers (e.g. 12) and a height ratio (e.g. 1.2) and ICEM will calculate the total height.

On your point about 3-4 layers. It's widely written in the ANSYS Help Guides that you want a minimum of 10-15 prism layers in the boundary layer.

Read the thread http://www.cfd-online.com/Forums/ans...h-quality.html to get an idea about floating/splitting/re-distributing prism layers to get a smooth prism to tetra volume transition and get your required initial prism height (i.e. y+).

Also read PSYMN's presentation, I've linked to it in http://www.cfd-online.com/Forums/ans...eat-sheet.html. That's the best source for ICEM info.

[Harshal]

Originally Posted by siw

Your distance of 2.7e^4 will be the initial height in ICEM. Then you can enter a number of layers (e.g. 12) and a height ratio (e.g. 1.2) and ICEM will calculate the total height.

On your point about 3-4 layers. It's widely written in the ANSYS Help Guides that you want a minimum of 10-15 prism layers in the boundary layer.

Read the thread http://www.cfd-online.com/Forums/ans...h-quality.html to get an idea about floating/splitting/re-distributing prism layers to get a smooth prism to tetra volume transition and get your required initial prism height (i.e. y+).

Also read PSYMN's presentation, I've linked to it in http://www.cfd-online.com/Forums/ans...eat-sheet.html. That's the best source for ICEM info.

Hello Siw,
thanks for your reply. I followed the ppt you linked, the one which deals with generating the prism layers. I tried first generating the surface mesh. However, there were some surfaces of the car which could not be meshed. So, I tried meshing them individually using surface mesh option. However, this was also not successfull and there was an error 'Surface Mesh Failed'. Therefore, I tried to generate a volume mesh directly, using the Robust Octree Method. There I gave the minimum height, the number of layers and so on. However, when the mesh was generated I could not see the prism layers (12 layers; I also reduced the acceptable prism quality so as to prevent low quality prisms in to being converted to pyramids). When I then changed the number of layers to 5 and generated the mesh, I could see the layers. So, this method works for 3-5 layers but not for 10 or 12 layers. Can you tell me where I am going wrong ?

Thanks,

Harshal

[siw]

Can you post a few images, that will help with fixing things regarding your comment about success with only a few prism layers.

I assume you made the octree volume mesh first, don't forget to first build topology. Give that a try then delete the volume elements so that you are left with a surface mesh. Check and smooth it. Then make a new volume mesh with the Delaunay method, that will work from your surface mesh. Lastly, make the prism as per PSYMN's presentation.

[Harshal]

Originally Posted by siw

Can you post a few images, that will help with fixing things regarding your comment about success with only a few prism layers.

I assume you made the octree volume mesh first, don't forget to first build topology. Give that a try then delete the volume elements so that you are left with a surface mesh. Check and smooth it. Then make a new volume mesh with the Delaunay method, that will work from your surface mesh. Lastly, make the prism as per PSYMN's presentation.

Thanks for your reply. Yes, you are right. I generated directly a volume mesh with Robust Octree method. However, before generating the volume mesh, I did Build Topology in the Geometry option and made sure that the geometry was alright. You suggested that I should generate the volume mesh by robust Octree method, then delete the volume elements, check and smoothen the surface mesh and then use Delauney method. The querstion is, how can delete the volume element after generating the mesh with Robust Octree ?

Regarding my earlier message, about generating a surface mesh, I realised that the surface mesh was infact generated. However, for some parts, it's not visible. I then switched off the 'Surfaces' from the Tree and could see the mesh for all parts. I don't know why this happened.

Thanks,

Harshal

[Andrea1984]

Hi Harshal,

for deleting the volume elements:
Edit mesh -> Delete elements -> Select all volume elements (last option on the right)

Andrea

[Harshal]

Originally Posted by Andrea1984

Hi Harshal,

for deleting the volume elements:
Edit mesh -> Delete elements -> Select all volume elements (last option on the right)

Andrea

Thanks, Andrea1984, for the quick reply.

[Harshal]

Hello all,
as you know, I am trying to simulate a sports car for aerodynamic analysis. So far, I have generated a mesh and prism as per the document created by Mr.Simon. I am trying to work with Fluent. However, I am getting very low mesh orthogonality (in the range of 10^-7). I tried various thing in ICEM mesh generation like changing the orthogonal weight fro 0.5 to 1.0 to 0.1, changing the prism quality, refines the mesh w.r.t aspect ratio etc. However, the mesh orthogonality in Fluent is still very low. In Fluent I tried to fix this problem with TUI. However, it only considers 0.1% of the worst cells and not all the worst cells.
Can someone kindly advise me how to fix this problem either in ICEM or in Fluent ? It would be really helpful.

Thanks,

Harshal

[siw]

Can you post some images of mesh with the poor cells.

[Harshal]

Thanks, siw, for your reply.
I have uploaded some images from my work. Please advice me on how to improve the mesh, so that I can have better mesh orthogonality.

Thanks,

Harshal

[siw]

Some general points as I don't know the specific requirements for your mesh and simulation (e.g. are you repeating wind tunnels, is drag accuracy very important, which RANS (assumed) turbulence model are you using). Post the *tin file and I'll have a quick attempt.

1. The mesh looks very coarse, decrease the surface element size on the car and either use the curvature features or set specific sizings on local parts for refinement.
2. Refine the mesh in the proximity of the car (wake, ground) a density region or two will sort that out. Allowing the mesh to gradually grow (<20%) will help mesh quality (and accuracy) rather than having large growth.
3. I cannot see any inflated prism layers on the car and the ground (perhaps you don't want the latter).
4. The car surface has many patches. Are you using a patch independent method (octree)?
5. Is the top of your fluid domain really supposed to be that close to the car? It is too close and will influence the flow around the car. Even if it is a wind tunnel roof it's too close. Also if it's a tunnel roof you'll want inflation layers there as well.

Now you've posted some images you can wait for the comments to say you'd be better off using ICEM Hexa blocking and that the topology is straight forward (plus more accurate aero results and better computational efficiency).

[Harshal]

Originally Posted by siw

Some general points as I don't know the specific requirements for your mesh and simulation (e.g. are you repeating wind tunnels, is drag accuracy very important, which RANS (assumed) turbulence model are you using). Post the *tin file and I'll have a quick attempt.

1. The mesh looks very coarse, decrease the surface element size on the car and either use the curvature features or set specific sizings on local parts for refinement.
2. Refine the mesh in the proximity of the car (wake, ground) a density region or two will sort that out. Allowing the mesh to gradually grow (<20%) will help mesh quality (and accuracy) rather than having large growth.
3. I cannot see any inflated prism layers on the car and the ground (perhaps you don't want the latter).
4. The car surface has many patches. Are you using a patch independent method (octree)?
5. Is the top of your fluid domain really supposed to be that close to the car? It is too close and will influence the flow around the car. Even if it is a wind tunnel roof it's too close. Also if it's a tunnel roof you'll want inflation layers there as well.

Now you've posted some images you can wait for the comments to say you'd be better off using ICEM Hexa blocking and that the topology is straight forward (plus more accurate aero results and better computational efficiency).

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

[cesarcg]

Dear Harshal,

As suggested by @Siw, I'd give a try to hexa meshing and see if it works better. I think that you could come up with a mesh with better orthogonality among cells. If your computational domain is the size you are showing in your captions, it may be a good idea to use C-Grid.

Let's wait for you to post the *.tin file.

Regards,
César

[Harshal]

Originally Posted by cesarcg

Dear Harshal,

As suggested by @Siw, I'd give a try to hexa meshing and see if it works better. I think that you could come up with a mesh with better orthogonality among cells. If your computational domain is the size you are showing in your captions, it may be a good idea to use C-Grid.

Let's wait for you to post the *.tin file.

Regards,
César

Hello, Cesar,
thanks for your reply. Unfortunately, I don't know how to upload the .tin file here. The .tin format is not supported here, in the attachment key (I get the 'Invalie File' error). I tried to upload the zip file. However, its size exceeds the permitable size. (2.94 MB instead of 97.7 KB).

[siw]

*.tin files are usually very small, I don't recall any of my files being bigger than the hundreds of KB.

[Harshal]

Hello siw,
thanks for your reply. Can I post the .tin file directly, or do I have to convert it into some other format ? I'll try again to post it.

Also, following your advice, I have increased the height of the box and generated a mesh with prism. I have attached a photo here. Can you tell me how I can smoothen the prism mesh ?

Thanks,

Harshal

[siw]

Just zip the *tin file and post it here.

Prism smoothing is tricky. I suggest reading PSYMN's presentation on ICEM tetra/prism, a quick search will find it. Basically, make sure you start with a checked and smoothed surface and volume mesh i.e. the quality should be as high as possible (> 0.3). When you smooth the prisms keep the quality metric < 0.05 with the PENTA_6 elements and smooth to a higher quality with PENTA_6 frozen. Again, the presentation explains it better than me.

It's difficult to see from that image but it looks like a rapid cell transition from the last prism to the first tetra, ideally the transition should not be greater than about 20%.

One other thing. How are you treating the interface of the wheels and the ground? If the wheels are perfect circles then that can force tight regions for the elements at the ground. In reality inflated wheels will bulge a little and that'll help with the mesh locally.