Cancel
Showing results for
Did you mean:

# Hex Meshing

Experimenter

Dear All,

I have a model, as per figure below

I am about to hex mesh the geometry. I was using command of Mesh - Mesh Control - Size on Solid.

Then, I use the command Mesh - Geometry - Hexmesh Solid.

But, some of the part is not hex mesh at all. The result are below,

Is there anyone have idea how to have a hex mesh the geometry above?

Here I attahed the model.

Regards.

21 REPLIES
Highlighted

# Re: Hex Meshing

Siemens Phenom

I recommend that you mesh the end surfaces with a good mesh quality.  In this case, I set the mesh size on the larger curves using a size of 6 and a bias of 2.  I also set the mesh approach to 3 Corner Mapped Fan.

Once you have the end surfaces meshed, you can create the hex mesh with the command, Mesh > Geometry > Hex Mesh From Elements.  You select the elements one of the surfaces as the base and the elements on the other meshed surface as the top and specify a mesh sizing between the surfaces.

Finally, you should associate the elements to the solids.

You'll also need to perform more solid splitting to match the meshes.

Best Regards,
Chip Fricke
Principal Applications Engineer - Femap Product Development

# Re: Hex Meshing

Experimenter

Hi Chip Fricke

If you are not mind, I still have a question.

I was trying to create a good mesh on the end of the surface, but I didnt make it.

Could you please explain me how to set the mesh size of 6 and bias of 2? and also using 3 corner mapped fan?

what command you have used? kindly please explain.

Thanks.

# Re: Hex Meshing

Solution Partner Phenom

Hello!,

As a complement of the Chip suggestion, in hex mesh regions that do not have straight lines that connect the top and bottom regions you can consider the following command: MESH > GEOMETRY > HEX MESH FROM ELEMENTS:

1.- SLICE the solid this way using command GEOMETRY > SOLID > SLICE:

2.- Next map mesh all the external surfaces that enclose the solid volume using a 2-D PLOT ONLY QUAD mesh, I used an element size around =10

3.- Next use command Mesh, Geometry, HexMesh from Elements... you will first select the 2-D PLOT ONLY elements that form the mapped base region (use METHOD>ON SURFACE), in this case I used the bottom inner surface. Then you will be prompted to select ALL of the rest 2-D PLOT ONLY elements that form ALL the remainder of the enclosing volume.

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/

# Re: Hex Meshing

Pioneer

Hi, Blas,

I used NX command "3D swept mesh" with option "Until target"to mesh this body according to your guide,

but i found some elements insde are distorted very much, as picture below,

do you have same problem ?

and any way to improve ?

# Re: Hex Meshing

Solution Partner Phenom

Hello!,

With FEMAP V11.4.1 the element quality achieved using the previous explained method is correct, here you are the output of command TOOLS > CHECK > ELEMENT QUALITY using the defaults settings of NX NASTRAN solver, all 3-D solid HEX8 elements passed with success!!:

```Check Element Quality
24200 Element(s) Selected...
No Elements Outside of Maximum Allowable Value.

Quality Check               Number Failed      Worst Value
Hex AR                             0           5.438054
Hex DetJ                           0           6.983279
Hex Warp                           0           0.990921

0 Elements Failed out of 24200 Checked.```

If I "erase" elements from the screen using the powerful tool "Draw/Erase Select Elements" this is what we have, the internal elements are well shaped, not too bad:

If you ask this question is because you didn't followed my suggested HEX meshing approach, try yourself and you will see the easy & powerful it is, OK?. This is FEMAP, not NX.

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/

# Re: Hex Meshing

Experimenter

Unfortunately it doesn't work always! Sometimes I'm meshing the top and bottom surfaces using the same approach, but still the parallel meshes are not always exact, so they cannot match for a successful hex-meshing. If however I decrease the mesh size, it works

# Re: Hex Meshing

Solution Partner Phenom

Hello!,

It seems that my explanations were not well understood, here you are the procedure to follow explained more in detail, step by step:

1.- This is the original geometry found in your posted FEMAP model. By the way, I note the FEMAP model is a very old version 11.10 (released in Novemeber 2013, five years old!!), time to update, don' t you. It is very important to run the last versions, severe errors are fixed and the meshing & geometric capabilities of current FEMAP V11.4.1 compared with old V11.10 nothing to see ....

2.- The TARGET is to convert all in a solid body, I will use command GEOMETRY> SOLID > ADD to form one solid from multiple, connected solids. Next I will use command GEOMETRY > SOLID > CLEANUP to make sure the geometry is perfectly cleaned. The result is the following (I changed the color as well, life is easy):

3.- Next using command GEOMETRY > SOLID > SLICE the solid is cut by three points, one the center (0,0,0) and the other two the end points A & B.

Repeat the other side and you will have the following (I change colors "randomly" using command MODIFY > COLOR > SOLID to demostrate that I have three solids):

Repeat cuts in solids by plane Z-X at both ends, and also at top by plane X-Y, and finally you will arrive to the following image (don´t forget to use GEOMETRY > SOLID > CLEANUP to let the solid perfectly cleaned after cuts):

5.- Once you have your portion of solid isolated, now proceed as explained at the beginning of the threeth, mesh the exterior surfaces with 2-D "PLOT PLANAR" 4-nodes quadrilateral elements using an element size of 8 mm and the resulting mesh will pass the minimum quality checks of both FEMAP & NX NASTRAN:

`Check Element Quality8520 Element(s) Selected...No Elements Outside of Maximum Allowable Value.Element Quality Quality Check Number Failed Worst Value Aspect Ratio 0 2.241092 Taper 0 1.052677 Alternate Taper 0 0.0277245 Skew 0 40.77757 Warping 0 2.565675 Nastran Warping 0 0.00359994 Tet Collapse 0 0. Jacobian 0 0.0539384  0 Elements Failed out of 8520 Checked.`

6.- And the finall step is to use this PLOT PLANAR 2-D mesh as seed of the 3-D solid mesh using command MESH > GEOMETRY > HEX MESH FROM ELEMENTS. The key is to select first the BASE elements in the inner face:

Click OK and and next select the elements in the other surfaces, the resulting mesh will be the following:

```Check Element Quality
46368 Element(s) Selected...
No Elements Outside of Maximum Allowable Value.

Quality Check               Number Failed      Worst Value
Hex AR                             0           2.466404
Hex DetJ                           0           2.876476
Hex Warp                           0           0.984442

0 Elements Failed out of 46368 Checked.```

The mesher algoritm works better with improved mesh density, using a coarse element size the result could be wrong, depending the geometry. The key here is first to arrive to a valid 2-D mesh (you can use the meshing toolbox, or manually prescribe a surface meshing approach of type MAPPED - FOUR CORNER and apply mesh size on surfaces) and next to select the proper BASE REGION:

Good luck & 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/

# Re: Hex Meshing

Solution Partner Phenom

Dear Alexandros,

The command MESH > GEOMETRY> HEX MESH FROM ELEMENTS is appropiate in the cases where not straight lines exist between top & bottom regions, in your case you have a straight line, then if not running this is because either top or bottom mesh is not exactly the same, you need mapped mesh.

To assure this, better use command MESH > MESH CONTROL > APPROACH ON SURFACE and select the option MATCHED - LINK TO SURFACE where basically it simply instructs FEMAP to make the mesh on the selected surface match the one on the surface that you link it to. This approach is primarily used to insure compatible meshing in a single solid for hex meshing. With the following conditions:

• Surfaces to be linked must either be on the same solid, or must be adjacent/coincident in space, or must at least be closely aligned.

• Surfaces to linked must also have the same mesh sizing, or they will not mesh properly. In order for a linked sur­face to be meshed, it must have the same mesh sizing as the master surface.

Best regards,
Blas.

Alexandros wrote:

Unfortunately it doesn't work always! Sometimes I'm meshing the top and bottom surfaces using the same approach, but still the parallel meshes are not always exact, so they cannot match for a successful hex-meshing. If however I decrease the mesh size, it works

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

# Re: Hex Meshing

Experimenter

Dear Blas,

thanks for the detailed instructions. As you adviced in this case I'm not using the command MESH > GEOMETRY> HEX MESH FROM ELEMENTS but MESH > GEOMETRY> HEX MESH SOLIDS.

I've tried with another solid and still not get matched results, although I linked the surfaces and did the same sizing.