Wing meshing 1

[mohanadelsayed]

hello
I need help in meshing this wing, I watched a lot of tutorials but nothing helped me
what's the best number and shape of mesh for this wing?
and is there a function in Femap that calculate the best number of meshes or error estimation?
thanks in advance

 

[BlasMolero]

Hello!,
First at all I suggest to update your FEMAP program, I note you run old version 10.30.

1.- I note you have a lot of sheet bodies, isolated (RUN "modify > color > surfaces > select all > select a color > random"), then shell meshing will be a pain!!.

2.- First select the outer skin and run command "GEOMETRY > SOLID > STITCH", this way all your outer skin surfaces will be a sheet body, correctly oriented its surfaces normals. Make sure NOT TO SELECT any of the transverse sheets, this is critical for properly creation of the stitched body.

3.- Next issue command "Geometry > Surface > NonManifold Add" and select ALL your surfaces. The result will be ONE body, with only ONE curve between surfaces, this way mesh maching is assured, not need to perform any "node merging" command, continuity is assured!!.

4.- Next use command "Mesh > Mesh Control > Approach on Surface" and select ONE triangular surface. Here apply the option "Mapped - Three Corner" and let the selction of corner points empty, FEMAP will select automatically the mesh control points. Repeat the command three times with the other three triangular surfaces.

5.- Prescribe an element size in surfaces of say 12/6=2. Here is very important to have EVEN number of element divisions on curves!!. This way the resulting mesh quality is higher because mesh distortion is lower.


6.- And finally mesh your body with Shell elements using command "Mesh > Geometry > Surface > Method = Solid". The resulting mesh is the following (plotting mesh quality ALT TAPER check results):

7.- To know the mesh quality run command "Tools > Check > Element Quality" and select your mesh, you will have the following listing:

Check Element Quality
2998 Element(s) Selected...
Element Quality
   Quality Check               Number Failed      Worst Value
      Aspect Ratio                       0            2.39799
      Taper                              0            1.84606
      Alternate Taper                    0            0.45443
      Internal Angles                   92            61.9275
      Skew                               0            30.5338
      Warping                            0            0.78164
      Nastran Warping                    0          0.0015869
      Tet Collapse                       0                 0.
      Jacobian                           8            0.62489
      Combined Quality                  98                 1.
      Explicit Time Step              2998                 0.
 
   2998 Elements Failed out of 2998 Checked.

Enjoy!.
Best regards,
Blas.


~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[mohanadelsayed]

thanks a lot Blas, you're genius.
I have some questions for you..

1- how can I validate a model like this one?
2- Is there a way to change mesh size for all structure without remeshing all the surfaceses particularly again?
3- i want to plot a curve between mesh error (max stress or deflection) and mesh size, how can I do such thing in easiest way ?
4- Is there a resource that you can recommend it to me to learn more about Femap?

attached 2 separate analysis, the first before your help, the second is after, the stresses and deflections are way different, that's why I need a validation.
and thank you in advance.

 

[mohanadelsayed]

this's the first.

 

[BlasMolero]

Hello!,

You have full information in the NX NASTRAN USER'S GUIDE, take a look to the NX NASTRAN manuals, no need to look for "strange" resources, you have the "best" in your own hands, in FEMAP click in "HELP > NX NASTRAN" and you are done!:

1.- The first check should be that LOADS and REACTIONS are in agreement, if this is not the case then the simulation results are useless. Check the OLOAD RESULTANT and SPCFORCE RESULTANT results (written in the F06 file) are the same, but with different sign.

2.- To change the mesh size of all the structure, simply use command "Mesh > Mesh Control > Size on Surfaces" and enter the element size you like. Remesh all surfaces with "Mesh > Geometry > Surfaces" and FEMAP will ask you to "Delete Existing Mesh and Remesh".

3.- In FEMAP do not exist an automated procedure to plot results vs. mesh Size, but you can do it yourself: take note of maximum results (Stress, displacements, etc..) achieved with every mesh size and plot the curve either in EXCEL or create a function plot in FEMAP.

4.- See my introduction.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[rb1957]

is this a structures model or a CFD model ?

what is the internal structure of the wing like ? stringers and ribs ?? solid ??

does the trailing edge really look like that ????

another day in paradise, or is paradise one day closer ?