[Sergi]

Hi All,

I've been reading posts for a while, but now I've decided to become a member of this forum to try to gain even more knowledge in the cfd simulations world.

So, here's my case. I've imported a parasolid geometry from SolidWorks, which is a race car, and when it comes to the volume mesh, I get horrible results for the leading edge and trailing edge of the front wing main plane and flap, and I have no idea about what more I can try to find a solution to this to obtain a better mesh.

The meshing models that I use are the surface remesher (with the automatic surface repair option deactivated because I don't find any improvement if it's activated), the trimmer mesher and prism layer mesher.

For the phyics, they are a llitle more, so that you'll find attached and image of all the models at the end of this post.

The reference values for the mesh and the specific values that I set for the front wing are also attached some images with all the parameters.

So, any ideas in how this problem with the geometry/mesh could be solved would be very welcomed. If you require some extra info that I missed to add, please let me know it.

Thanks in advanced to all of you!

FW trailing edge.jpg Mesh and physics models.jpg Reference values.jpg
FW region parameters.jpg

[fluid23]

To control volume mesh size at a surface, you must first control the surface mesh size at the surface. Have you ever meshed a 2D airfoil before and noticed that you have a much higher node density at the leading and trailing edges? You need to do the same thing here.

Probably your easiest option is to go back into Solidworks and modify your geometry so that you can have separate surfaces at the LE and TE. Use the split line command and either a sketch, surface or plane to make the surface 'cuts'.

Then go back and remesh, but be sure to assign custom controls to the LE and TE surfaces under operations > mesh ... etc.

Originally Posted by Sergi

Hi All,

I've been reading posts for a while, but now I've decided to become a member of this forum to try to gain even more knowledge in the cfd simulations world.

So, here's my case. I've imported a parasolid geometry from SolidWorks, which is a race car, and when it comes to the volume mesh, I get horrible results for the leading edge and trailing edge of the front wing main plane and flap, and I have no idea about what more I can try to find a solution to this to obtain a better mesh.

The meshing models that I use are the surface remesher (with the automatic surface repair option deactivated because I don't find any improvement if it's activated), the trimmer mesher and prism layer mesher.

For the phyics, they are a llitle more, so that you'll find attached and image of all the models at the end of this post.

The reference values for the mesh and the specific values that I set for the front wing are also attached some images with all the parameters.

So, any ideas in how this problem with the geometry/mesh could be solved would be very welcomed. If you require some extra info that I missed to add, please let me know it.

Thanks in advanced to all of you!

Attachment 48239 Attachment 48240 Attachment 48241
Attachment 48242

[Sergi]

Originally Posted by MBdonCFD

To control volume mesh size at a surface, you must first control the surface mesh size at the surface. Have you ever meshed a 2D airfoil before and noticed that you have a much higher node density at the leading and trailing edges? You need to do the same thing here.

Probably your easiest option is to go back into Solidworks and modify your geometry so that you can have separate surfaces at the LE and TE. Use the split line command and either a sketch, surface or plane to make the surface 'cuts'.

Then go back and remesh, but be sure to assign custom controls to the LE and TE surfaces under operations > mesh ... etc.

Thanks for your answer Matt. I'll try to do that and see if it works. At least I've already prepared the airfoil in SolidWorks (to make it easier for me, now I'm only testing the FW instead of the whole car).

In the meantime, could you give me some more details about the configuration for the volumetric control feature under the operations menu that I need to use for this? I'm quite newbie on this and some extra guidance would be very welcomed.

[fluid23]

You don't need a volumetric control, at least not yet. I typically add those to refine areas with high pressure/velocity gradients later on (if at all).

All you need to do is go into your mesh operation and right click custom controls then select new > surface control. Now name it something like LE or TE, assign a part surface to it and open the controls drop down. Here you will see a list of different mesh settings that you can control on that surface. You will want to highlight Target Surface Size and Minimum Surface Size then change the property to Custom.

Now you can expand the values drop down menu and define a new target and minimum surface size for this one surface, or multiple surfaces if you have several that you want to have meshed similarly. Then just remesh and view the results. You may have to play around a bit to figure out what works best for your application.

I would also recommend changing default controls > surface curvature > basic curvature to at least 60 if you haven't done so.

[Sergi]

Originally Posted by MBdonCFD

You don't need a volumetric control, at least not yet. I typically add those to refine areas with high pressure/velocity gradients later on (if at all).

All you need to do is go into your mesh operation and right click custom controls then select new > surface control. Now name it something like LE or TE, assign a part surface to it and open the controls drop down. Here you will see a list of different mesh settings that you can control on that surface. You will want to highlight Target Surface Size and Minimum Surface Size then change the property to Custom.

Now you can expand the values drop down menu and define a new target and minimum surface size for this one surface, or multiple surfaces if you have several that you want to have meshed similarly. Then just remesh and view the results. You may have to play around a bit to figure out what works best for your application.

I would also recommend changing default controls > surface curvature > basic curvature to at least 60 if you haven't done so.

Thanks Matt! Definitely, by using the split line command in SW to separate the LE and TE of the airfoil solved my problem!

Now I have to adjust the surface control values to refine even better the final mesh, but at least now this procedure worked for the problem that I had!

Thank you very much for your help!