how to substract areas on femap ? 1

[ahmadmah]

hello

can any one told me how to substract areas on nastran (femap) , i draw rectangle then i draw triangle then i donot know how to substract them from each other

thanx

 

[rb1957]

assuming you want a five (or more) edged surface ...
use "boundary surface" ... you only need to define the points (corners) and then use the boundary surface command to join them together.

 

[BlasMolero]

1.- Draw a rectangle
2.- Create a closed surface using "Geometry > Boundary Surface > From curves" selecting the curves of the rectangle. Convert the Boundary Surface in regular Parasolid surface using "Geometry > Surface > Convert".
3.- Draw a triangle by curves.
4.- Using the command "Geometry > Curve - From Surface > Project" simply project the curves of the triangle over the rectangle. You will have an imprint (make sure the "Update Surfaces" togle is ON).
5.- Simply delete the inner triangle surface, and you are done!!.

Do not look for any boolean operation, simply cut the outer rectangular surface by the curves of the triangle, and delete the inner surface resulting of the operation.

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

 

[rb1957]

how'll FeMep go at meshing a 5 sided surface ? maybe a quaderlatial and a triangle would be better ??

 

[BlasMolero]

Dear rb1957,
Not problem meshing a multi-sided surface, then the automatic mesher should applied. FEMAP will create a dominant QUAD mesh mixing quadrilateral & triangular elements based in the subdivision method where the user can control element type (QUAD/TRIA), mapped meshing options, subdivision options, offset options, etc...

The Mesher section allows you to choose between meshing the surfaces with quadrilateral surface elements, where possible (Quad option), or all triangular surface elements (Tri option). When using the Tri option, you may choose to use Auto, which will examine each surface one at a time and attempt to choose the Tri mesher which will create the best overall triangular mesh on each individual surface. If you want FEMAP to use a particular Tri mesher, uncheck Auto and choose one of the three triangle meshers.

When Mapped Meshing is set to Off, FEMAP will simply mesh the selected surface(s) with a "free mesh", unless a "Mapped Meshing Approach" is set. If Mapped Meshing is On, FEMAP will attempt to create a "Mapped Mesh". FEMAP uses the values set for Max Angle Deviation and Min Corner Angle to determine "corners" it can use to attempt a mapped mesh on surfaces.

The subdivision options control the size and shape of the mesh inside the boundary. The elements along the boundary edges are defined by the mesh sizes that you choose and are unaffected by these settings. Those mesh sizes also have substantial impact on the interior of the mesh, but these options give you additional control.

Etc.., the resources available in FEMAP to mesh multi-sided surfaces are many. The classical method I use is to split the geometry in regular regions, allowing to create QUAD quality mesh.

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

 

[SAITAETGrad]

Well put, Blas. I would just continue your thought that for areas of interest, you can divide up the area and create a refined mesh with all the proper corner angles, aspect ratios, etc. for low error. You can then create another perimeter outside of this area of interest and fill the "moat" with CST elements as transitions between the area of interest and your larger model that may have a lower mesh density requirement but still needs an accurate, low error quad mesh.