How to Mesh in FEMAP with HEX and TET elements

I have answered a question in the FEMAP FORUM about how to mesh with 3-D solid elements a complex assembly, here the requirement was to have at least 3 elements in the AIR VOLUME GAP between solid capacitors to capture with accuracy the fluid flow between components. The following picture shows the simplified geometry proposed by the end user and uploaded to the FEMAP Community to be used to show how to mesh with 3-D solid elements.

1.- HEX Meshing using SWEEP method

I have recorded a video where I teach how to mesh the above assembly using an alternate method to the classical one based in slicing solids and later use command MESH > MESH CONTROL > SIZE ON SOLID that automatically performs the multi-solid sizing in assemblies. Not, my alternative method is “manual” but not complex at all, basically we use the commands MESH > SWEEP followed by MODIFY > ASSOCIATIVITY > AUTOMATIC that allows to generate perfectly shaped hexahedral 8-nodes elements with excellent quality and very low reduced model size, valid only in such special cases where the geometry has a predominant direction of extrusion.

The first step in the model geometry preparation is to use command TOOLS > CONVERT UNITS because I noted the geometry was in meters, and the wall thickness of AIR GAP is only 2.54 mm, then to have 3 elements in the thickness the element size should be 2.54/3=0.85 mm (ie, 0.00085 meters). My experience tells me that working in meters in FEMAP is not recommended at all for both meshing and geometry reasons, the mesher can give error due to tight tolerances used internally by FEMAP. To help the conversion units more automatically search in the FEMAP directory where you have *.CT files like IDEAS_from_m_N_degK_to_mm_N_degC.CF that include all parameters to convert the full database of FEMAP (not only geometry, but also material properties, loads, etc..) from meters to milimeters:

The next step is to prepare the base 2-D mesh to sweep along a curve in the extrusion direction: the key is to use GEOMETRY > Curve – from Surface > Project command, first select the top surface and next select ALL curves to project over that surface, the result will be the following figure:

The next step is to mesh the splitted surfaces with 2-D Plot-Only elements: to arrive to a mapped mesh the key is to use MESH > MESH CONTROL > APPROACH ON SURFACE command and prescribe to all surfaces the option MAPPED – FOUR CORNER, the result after meshing is great, magic!, see next picture.

Next after using the MESH > SWEEP command the resulting HEXAHEDRAL 8-nodes 3-D solid elements will have an extremely good quality mesh, you can see yourself, the ASPECT RATIO = 1.0, perfect!. And the resulting model size is really, really low, the lowest possible. Also HEXAHEDRAL elements provide the best accuracy possible, they have superior performance to ANY other 3-D solid element, nothing compares.

The final step will be to use MODIFY > ASSOCIATIVITY > AUTOMATIC command, select ALL elements, next select ALL solids, and do not forget to activate the option DETAILED ASSOCIATIVITY SUMMARY, this will help you to control that not any element or node failed to associate with geometry. This command is great, in addition to the nodes and elements being associated to the main entity, they will then also be associated to the surfaces of solids, curves on those surfaces, and points on those curves allowing you to use geometry based commands in FEMAP (i.e., Loads and Constraints on geometry, any selection method using a geometric entity, etc.).

To learn more how to do it, please take a look to this video and enjoy!. By the way, sorry for my bad english speaking, I need to practice more!.

Also take a look to this another video, I have recorded as well to explain how to use HEX meshing with simply geometry solids, the idea was to explain how simple is to HEX mesh solids, then not need to think in meshing with tetrahedral elements all the time. The geometry is simply, I tried to explain basically the above geometry manipulation and meshing procedures. Ah!, enjoy the Country music.

And finally another example of HEX meshing using the great “MESH > SWEEP” command in FEMAP, in this case the solid part was meshed originally with TET10 elements resulting in a total model size of 49437 nodes: the same geometry meshed with HEX8 elements using exactly the same element size results in only 6872 nodes, a reduction of more than 86%, ie, meshing with TET10 elements will increase the model size in more than 7x times!! (enjoy the COUNTRY music again, I love it!, definitely I am a man of few words, better facts!!).

2.- TET Meshing using NonManifold-Add 

The next recorded video shows the Tetrahedral meshing approach that need to be followed with multi-solid assemblies where touching solid faces don´t have the same size. Here, I will show you how the two commands GEOMETRY > SURFACE > NonManifold-Add and GEOMETRY > SURFACE > RECOVER MANIFOLD GEOMETRY plays a critical role in cases where adjacent surfaces DON’T HAVE THE SAME SIZE: solid faces are coincident (touching each-other, yes), but if the two surfaces don’t have exactly the same size the mesh matching is not performed successfully, and the mesher will give errors of type “Unable to link mesh locations between Surface XXX and Surface YYY. Surfaces must be on same solid or coincident“.

To set the element size in multi-solid assemblies using the classical command MESH > MESH CONTROL > SIZE ON SOLIDS you need to SELECT ALL SOLIDS AT THE SAME TIME, and FEMAP will set a “slaved” mesh approach on surfaces that are adjacent to each other and with the same size. The user must ensure that the meshes on these two surfaces are identical. Setting one of the surfaces as a slave to the other insures a consistent mesh. This option automatically finds surfaces which are adjacent between multiple solids and slaves them to each other.

In cases where solid faces are touching each-other but don’t have the same size, simply run command Geometry > Surface > NonManifold-Add, select all solids and done!. The result will be ONENon-Manifold Solid Geometry”, an option in the Parasolid modeling kernel which creates “General Bodies” as opposed to regular solids (FEMAP solids). The command allows you to essentially Boolean Add solids to one another.

The key will be next to use immediately the command “Geometry > Surface > Recover Manifold Geometry“, here FEMAP will take the selected “general body” in your model and separate them into component “Manifold” Parasolid solids (FEMAP solids), maintaining the imprinted curves between touching surfaces, in summary, having coincident surfaces between solids with exactly the same size, and then the process of slaving mesh approach required to have consistent mesh between coincident surfaces will be successfully performed, OK?.

In the next video you can see that ALL solid bodies are initially perfectly cleaned, not any imprint exist, like the air component of the following image:

After using the command NonManifold-Add selecting all solids, followed by Recover Manifold Geometry then all components are each-other imprinted, see the result on the Air component:

It’s surprising how the command NonManifold-Add that is used mainly to work with stitched surfaces to mesh with 2-D Shell elements plays an important role (together with Recover Manifold Geometry command) to mesh multi-solid assemblies with 3-D Solid elements. Well, take a look to the following video where I explain how to perform the meshing approach, I hope you understand perfectly the workflow, if you have any question please do not hesitate to contact me, it will be a pleasure to be of help!!. Ah!, again the system of units here is critical, more than ever, working in millimeters is mandatory, forget at all to use meters. If for any reason you need to work in meters (typical in CFD jobs), first solve the meshing task in millimeters and when successful use command TOOLS > CONVERT UNITS to convert your model from millimeters to meters, OK?.




Es un lujo poder combinar la ingeniería y el placer por los Elementos Finitos usando FEMAP y NX NASTRAN con el amor por la bicicleta de montaña MTB, todo ello se ha visto reunido en este “ejercicio de ingeniería” realizado con la ORBEA Rallon X10, una máquina perfecta para practicar la especialidad Enduro en MTB con descensos rápidos en la montaña.

La siguiente imagen muestra la malla por elementos finitos del cuadro a partir del modelo CAD 3-D utilizando elementos Shell 2-D CQUAD4 y elementos sólidos 3-D CHEXA de 8-nodos. La capacidad de FEMAP de creación automática de superficies medias (midsurfacing) a partir de modelos sólidos es vital a la hora de afrontar el mallado con elementos Shell de componentes de pequeño espesor y gran longitud. Masivamente he utilizado la capacidad de FEMAP y NX NASTRAN de unir mallas incompatibles Shell-Sólido mediante la opción “GLUE edge-to-face” y mallas no coincidentes Sólido-Sólido con “GLUE Face-to-face“, lo cual ofrece una total libertad de mallado y permite concentrarnos en obtener mallas de máxima calidad y mínima distorsión. El uso de elementos hexaédricos permite reducir el tamaño del modelo al máximo manteniendo una elevada precisión de resultados a un coste muy reducido gracias a las capacidades de mallado hexaédrico de FEMAP (haz click en la imagen para verla en su tamaño completo).

La siguiente imagen muestra el detalle de la unión entre elementos sólidos Tetraédricos 3-D CTETRA de 10-nodos y elementos viga 1-D CBEAM utilizando elementos rígidos RBE2: es un recurso muy interesante que utilizo muy a menudo para reducir el tamaño del modelo en componentes que actúan como una viga, trabajando masivamente a flexión (haz click en la imagen para verla en su tamaño completo).

En la imagen siguiente se muestra de forma comparativa la malla y la geometría de base que hace posible ese mallado tan precioso. Las claves para conseguir mallas de buena calidad son tres: partir, partir y partir!!. Es vital particionar correctamente la geometría, en FEMAP se pueden seguir múltiples caminos para conseguir una malla de calidad, los conceptos son básicos, siempre lo mismo, por eso es importante practicar y aprender bien el concepto ya que las posibilidades son numerosas.

Utilizando mallas sólidas a base de elementos hexaédricos CHEXA de 8-nodos se consiguen dos objetivos: excelente calidad de resultados (especialmente en problemas de contacto) y reducido tamaño del modelo, vital de cara a realizar análisis dinámicos tanto lineales como no lineales (haz click en la imagen para verla en su tamaño completo).

Y por último os dejo un detalle más de mallado: los agujeros en FEMAP no son un problema, podemos incluirlos perfectamente en cualquier malla local con total precisión, tenéis disponibles recursos muy potentes tales como “WASHER” y “PAD” tanto en el MESHING TOOLBOX para actualizar la malla de forma interactiva como en “Geometry > Curve – From Surface“. Las órdenes “Split Point-to-Point“, “Split Point-to-Edge“, etc.. son muy valiosas para dividir la geometría de forma rápida, ¿OK? — a disfrutar!!.



En esta última entrega de Tutoriales sobre el mallado en FEMAP V10.3 de modelos sólidos con elementos “brick” 3-D hexaédricos CHEXA de 8-nodos os voy a explicar un par de trucos que yo utilizo muy a menudo para mallar geometrías de revolución cuando falla el método automático con el siguiente mensaje de error:

Mesh Size on Solid
1 Solid(s) Selected…
Computing Mesh Sizes…
Solid 1 can not be hex meshed. Unable to identify the surfaces for the base and top of the mesh.


En la imagen siguiente os muestro cómo preparar la geometría para realizar una malla 2-D paramétrica del tipo “plot-only” (también se conoce como “seed meshing”) de excelente calidad que sirva de base a la malla 3-D utilizando las técnicas de partir geometría con “Split Point-to-Edge” y “Curve Washer“:


En la siguiente imagen tenéis la malla 2-D del tipo “Plot-Only” que servirá de base a la malla 3-D sólida hexaédrica, controlando que los paámetros más importantes de distorsión de la malla tales como JACOBIAN y ASPECT RATIO tengan unos valores lo más pequeño posible:


Utilizando la orden “Mesh > Revolve > Element” creamos una malla 3-D hexaédrica por rotación de la malla 2-D alrededor del eje de revolución un ángulo de 90º.

La malla resultante tiene una calidad excelente, con una distorsión mínima en la zona de mayor interés del redondeo creando elementos hexaédricos “bricks” de 8-nodos perfectamente construidos, mientras que en la zona próxima al eje de revolución se crean prismas triangulares “wedges” de 6-nodos:


Y por último sólo nos queda utilizar la orden “Modify > Associativity > Automatic ..” para asociar la malla sólida 3-D con la geometría sólida (puntos, curvas, superficies y sólidos):

FEMAP nos ofrece un resumen con los detalles de la operación de asociar la malla con la geometría, el resultado es perfecto, a efectos prácticos es lo mismo que si hubiéramos mallado directamente el sólido ya que podemos aplicar cargas y condiciones de contorno directamente a la geometría — qué fácil, ¿eh?.

Automatic Associativity
21375 Element(s) Selected…
1 Solid(s) Selected…
Attaching to Solid 1…
  25 Nodes associated with Point(s).
  464 Nodes associated with Curve(s).
  4018 Nodes associated with Surface(s).
  18744 Nodes associated with Solid(s).
  21375 Elements associated with Geometry.


Si quieres repetir este tutorial en tu propio ordenador pídenos los modelos con la geometría de entrada y te lo remitimos por e-mail, es un servicio gratuito para nuestros clientes de IBERISA.


Descargar vídeo (216 MB, 26 min.):

4.- Mallado con Elementos Hexaédricos (HEX Meshing-II)

En esta nueva entrada trato de explicar los conceptos básicos del mallado con hexaedros en FEMAP V10.2, a veces es mejor empezar por lo más sencillo para asegurarnos que se entienden bien las cosas.

Si quieres repetir este tutorial en tu propio ordenador pídenos los modelos con la geometría de entrada y te lo remitimos por e-mail, es un servicio gratuito para nuestros clientes de IBERISA.


Descargar vídeo (232 MB, 43 min.):