FEMAP adjacent surfaces mesh problem

Experimenter
Experimenter

Hi everyone!

 

I am currently working on my masters thesis (composite aircraft wheel) and after fixing the problem with laminate material orientation in FEMAP v 11.1.2. I was able to do the static analysis. What happened is that the meshis breaking on free edges that should not exist. I meshed the geometry via Mesh > Mesh Control> Size on surface; Mesh > Geometry > Surface. Geometry was created by revolving a set of curves made in ACAD, saved in DXF(fig 1) to form surfaces. After creating surfaces in FEMAP, by revolving curves, i found issues between adjacent surfaces, seems like they are not properly revolved, so connection seems poor(fig 2). Surfaces are meshed with different properties, depending on thickness of laminate etc.

 

fig 1

geometry_curves.JPG

 

fig2

geometry.JPG

 

After goint through the static analysis, i get these results. You can clearly see the mesh breaking at surface connections (fig 3). The reason is that the mesh sizing is obviously different on connecting surfaces(fig 4), thus nodes are not connected so I got free edges(fig 5), where they should not be. I tried using the Geometry > Solid > Cleanup, and Meshing toolbox > Combined / Boundary Surfaces, and also Geometry > Solid > Stitch, but it helps on some and on some not. After trying to remesh model I get "Free edges of selected elements do not form a single closed boundary". What else can I do, or what am I doing wrong ?

 

Thanks in advance !

Petar

 

fig 3 

mesh_breaking.JPG

 

fig 4

nodes_not_connected.JPG

 

fig 5 

free_edge.JPG

 

 

 

 

 

8 REPLIES 8

Re: FEMAP adjacent surfaces mesh problem

Siemens Phenom Siemens Phenom
Siemens Phenom

Does it help if you bump up the Gap Tolerance when using Geometry > Solid > Stitch? You may want to measure the distance between the biggest gap in adjacent surfaces you see in the model and use just slightly over that. 

 

If not, are you able to post the model here?

Re: FEMAP adjacent surfaces mesh problem

Experimenter
Experimenter

Here are the models, one is with results, and another one is for experimenting:

 

main_model

experimental

 

Thanks for quick response!

Petar

Re: FEMAP adjacent surfaces mesh problem

Gears Phenom Gears Phenom
Gears Phenom

 I would say the "sticth" option is for small gaps.With large tolerances you have the risk to deteriorate the surfaces. I have no time to check your models but maybe the best option is to close the gap with surfaces (build the geometry) and then, if the elements after meshing are too small :

- under meshing >perpare geometry

- or in the meshing toolbox delete lines under feature removal(or another option)

Re: FEMAP adjacent surfaces mesh problem

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Petar,

If I look to your "main_model" what I see is a lot of unconnected cylindrical surfaces, I don't understand the meaning of this geometry (simply color all surfaces randomly doing MODIFY > COLOR > SOLID > SELECT ALL), non sense to me.

rounded-geo.png

rounded-mesh.png

In any case, you need to stitch your surfaces geometry together to create PARASOLID sheet solid bodies from a series of tangent surfaces, this is the first step to me, meshing will be the last task, use command GEOMETRY > SOLID > STITCH and select all the tangent surfaces of the rim, don't select any T-JOINT surfaces because PARASOLID do not support t-joints and will give you error. If the geometry don't feature gaps, ie, is well created in the CAD system (FEMAP make miracles most of the times) then you will see how many tangent isolated surfaces are stitched forming only ONE entity sheet body, then merging nodes will be performed for sure correctly because only "one" surfaces is shared between two surfaces. Repeat the command with every section with tangent surfaces.

Because stitching is done as an iterative process, the Gap Tolerance should be set to the largest distance which should be considered when attempting to close gaps between surface edges (start with default value 1e-6). This is a very useful command when reading trimmed surfaces from an IGES file. You can read an IGES file, and then use this command to generate a Parasolid solid from the IGES surfaces. You can then manipulate this solid just like any other solid you would have created in FEMAP.

Warning: from material properties to me you run in meters, wrong!!, convert your geometry to millimeters better and work in MPa, if not tolerance will be a problem ...

rounded-stitch.png

 

And finally joint all the sheet bodies together using command GEOMETRY > SURFACE > NON MANIFOLD-ADD, this way you will have ONE body properly stitched and ready to mesh with success, OK?.

Best regards,
Blas.

PD

Please note also: geometry stitching is critical also to have surfaces normal properly oriented, consistently oriented with all surfaces in the same direction, I see

rounded-vector.png

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

Re: FEMAP adjacent surfaces mesh problem

Experimenter
Experimenter

Hi Blas, and thank you for a thorough response!

Cylindrical surfaces are glued together, and are given laminate property - the idea behind it was to use laminate property, and avoid the solid. I tested this on a simple model, giving several surfaces 1 ply as property compared to one layup on one surface, and the differences in results are minimal. They are created this way so i can recreate the original shape as closely as possible.

I managed to fix geometry following your advice. Stitch was working well for tangent surfaces, but what was bothering me was the protrusion of the vertical surface - it still looked like inaccuracy, so i was confused. I will also switch, as you suggested, properties, material and layups into mm.

Once again, thank you for a solution and wish you all the best.

Petar






 

Re: FEMAP adjacent surfaces mesh problem

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Petar,

To switch loads, properties & geometry to mm do not do it manually, it can be performed automatically at full model using command TOOLS > CONVERT UNITS and load file IDEAS_from_m_N_degK_to_mm_N_degC.CF from <FEMAP_install> directory that include internally all parameters to perform the job with success:

convert-units-meter-to-mm.png

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: FEMAP adjacent surfaces mesh problem

Experimenter
Experimenter

Hi Blas !

Thank you for quick response.

I already imported geometry in mm with scale factor 1:1, is it possible to solely scale properties (including layups and material definition), and leave geometry as it is. 

 

Kind regards,

Petar

Highlighted

Re: FEMAP adjacent surfaces mesh problem

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Petar,

Uhmm, be careful, when you import geometry in FEMAP (for instance, from Parasolid or Acis) the geometric scale 1 means you import geometry in meters, not millimeters, OK?.

geometry-import.png

FEMAP use by default the options defined by the user in FILE > PREFERENCES > GEOMETRY where you can set the scale factor to use when importing geometry, as you can see, 1000 means millimeters, this is because PARASOLID internally use meters as geometry kernel.

Parasolid geometry is always stored internally in SI (meters) no matter what unit it is created in.
Parasolid has a “box” with dimensions of 1000 x 1000 x 1000 meters with it’s origin at the center of the box. When the models length is in millimeters, a length of 1.0 mm on the desktop will be stored as .001 meters in the database.

file-preferences-geometry.png

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/