turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- CAE Simulation - Femap Forum
- Surface Meshing

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

12-25-2014 12:33 AM - edited 01-08-2015 01:21 PM

What's the best way to mesh this model for CFD analysis.

Your comments are welcome!.

Thanks,

Aero1

Solved! Go to Solution.

9 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

12-26-2014 06:33 AM

Dear Aero1,

As a rule of thumb, you need to create a solid geometry around the wing to mesh the air volume that should extend roughly 10 times the size of the wing body in every direction.

Also, for turbulence modelling the mesh size next to flow surfaces and adiabatic walls is important and depends on the selected turbulence model because the mean velocity increases with the wall distance. Boundary layer meshes are preferred for turbulence modeling even if you could obtain the same wall mesh size requirements using equally spaced meshes at a cost of overall number of elements.

When creating the mesh for turbulence modeling, the first node inside the boundary layer should always be in the inner layer. Further care must be made on where the first node needs to be inside the inner layer depending on the turbulence model used, and whether or not wall functions are used.

The appropriate mesh size next to walls is determined by the y+ value of the centroid of the wall-adjacent control volume. FEMAP can display y+ results at element nodes, simply request it when using FEMAP TMG/Flow solver.

The Y+ values indicate the position of the first internal node in relation to the boundary layer. The fully turbulent region of the boundary layer is for Y+ values above 30. Although results will be more accurate with Y+ values greater than 30, the **Mixing Length** and **k-Epsilon** turbulence models in **FEMAP/TMG Flow** account for small Y+ values by adding a damping function on the turbulent viscosity. This damping effectively reduces the near wall turbulent viscosity, forcing it to zero as Y+ tends to zero. Because of this damping on the turbulent viscosity, the mixing length and k-Epsilon models give reasonable flow and thermal solutions even for Y+ values less than 30.

As a reference, the figures below illustrate an example of an ideal 3D mesh of a wing:

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

12-28-2014 02:02 AM

Blas, thanks for your comprehensive comments, I'll definitely take your suggestions into consideration.

Regards,

Aero1

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

12-28-2014 08:16 PM

Blas, I have couple of questions about your comments:

1- How did you configure your mesh parameters in Mesh menu to get a result like "3D-Mesh-wing2.png" snapshot?

2-To get result similar to yours, do I need to sort all the similar components (based on their shapes, sizes, curvatures,...) in different layers/groups or Femap does that automatically?

3-After I made the air volume, do I need to subtract the wing-engine model out of that volume? (to create a void volume)

Thanks,

Aero1

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

12-29-2014 05:01 AM

Dear Aero1,

1.- Use 2-D mesh of type "Plot-Only" as seed mesh to control 3-D solid tetraedral mesh.

2.- FEMAP do not do things for you, the use of LAYERS is critical to manage complex assemblies with success.

3.- You need to arrive to valid solids to mesh with 3-D Solid tetraedral elements, then the use of boolean operations is quite typical.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

12-29-2014 02:14 PM

Blas,

Right after I meshed the model, the original colors that I have assigned to the componants have been replaced with just two colors (light blue and transparent blue) as shown in the attached file.

What do these colors mean? How can I retrive the original colors that I had before the mesh?

Regards,

Aero1

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

12-29-2014 03:08 PM

Dear Aero1,

When using commnd "**Mesh > Mesh Control > Size on Solids**" and you select more than **ONE** solid then FEMAP will try to detect matching surfaces with identical area. If any "pair" is found then FEMAP will create master & slaves relations between both surfaces, making the mesh size identical, and then merging of nodes could be performed with success (in case of activated) during next TET or HEX meshing task, OK?.

This is perfectly explained in the FEMAP manuals (remember, all are in the manuals!!)

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

12-29-2014 04:53 PM

Got it, thank you!.

Regards,

Aero1

Regards,

Aero1

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

01-08-2015 01:50 AM

Hi Blas,

So far I've managed to prepare the model as well as the far-feild BC, what I would like to do is to start the mesh from the surface of the far-feild and stop them within a specific distance (away) from the surface of the model and then create another dense mesh from that imaginary surface to the real surface of the model, is this doable without using TMG? How? "Thanks",

Regards,

Aero1

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

01-10-2015 05:12 PM

Hello!,

I will slice the full fluid domain in more portions (or parts) normal in the direction of the mesh transition, this way you can prescribe local element size and perform a mesh transition from local to global (do not forget to activate the "adjacement surface matching", linking is required to guarantee a continuous mesh).

Best regards,

Blas.

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc