Topological naming problem/es

Introducción
El problema de denominación topológica en FreeCAD se refiere a la cuestión de que una forma cambie su nombre interno después de que se realice una operación de modelado (almohadilla, corte, unión, chaflán, filete, etc.). Esto dará lugar a que se rompan o se calculen incorrectamente otras características paramétricas que dependen de esa forma. Este problema afecta a todos los objetos de FreeCAD, pero es especialmente notable cuando se construyen sólidos con el Ambiente de trabajo DiseñoPieza, y al dimensionar esos sólidos con el  Ambiente de trabajo Dibujo Técnico.
 * En [[Image:Workbench_PartDesign.svg|24px]] DiseñoPieza, si un rasgo se apoya en una cara (o borde o vértice), el rasgo puede romperse si el sólido subyacente cambia de tamaño u orientación, ya que la cara (o borde o vértice) original puede ser renombrada internamente.
 * En [[Image:Workbench_TechDraw.svg|24px]] DibujoTécnico, si una dimensión está midiendo la longitud de un borde proyectado, la dimensión puede romperse si se cambia el modelo 3D, ya que los vértices pueden ser renombrados cambiando así el borde medido.

El problema de la denominación topológica es un problema complejo en el modelado CAD que se deriva de la forma en que las rutinas internas de FreeCAD manejan las actualizaciones de las formas geométricas creadas con el OCCT kernel. A partir de FreeCAD 0.19 se están realizando esfuerzos para mejorar el manejo del núcleo de las formas con el fin de reducir o eliminar tales problemas.
 * Hilo del foro: Denominación Topológica, Mi Toma

El problema de la denominación topológica afecta y confunde con mayor frecuencia a los nuevos usuarios de FreeCAD. En DiseñoPieza, se aconseja al usuario que siga las mejores prácticas discutidas en la página edición de características. Se recomienda encarecidamente el uso de objetos de referencia de apoyo como planos y sistemas de coordenadas locales para producir modelos que no estén fácilmente sujetos a tales errores topológicos. En DibujoTécnico, se aconseja al usuario que añada dimensiones sólo cuando el modelo 3D esté completo y no se modificará más.

Ejemplo
1. En la 24px Ambiente de trabajo DiseñoPieza, crear un DiseñoPieza Cuerpo, luego use  DiseñoPieza NuevoBoceto y seleccionar el plano XY para dibujar el boceto base; luego realizar un  DiseñoPieza Pad para crear un primer sólido.



2. Select the top face of the previous solid, and then use PartDesign NewSketch to draw another sketch; then perform a second pad.

3. Select the top face of the previous extrusion, and once again create a sketch, and a pad.



4. Now, double click the second sketch, and modify it so that its length is along the X direction; doing this will recreate the second pad. The third sketch and pad will stay in the same place.



5. Now, double click the second sketch again, and adjust its points so that a portion of it is outside the limits defined by the first pad. By doing this, the second pad will recompute correctly, however, when looking at the tree view, an error will be indicated in the third pad.



6. By making visible the third sketch and pad, it is clear that the computation of the new solid did not proceed correctly. The third sketch, instead of being supported by the top face of the second pad, appears in a strange place, with its normal oriented towards the X direction. This results in an invalid pad, as this pad would be disconnected from the rest of the PartDesign Body, which is not allowed.

The problem appears to be that when the second sketch was modified, the top face of the second pad was renamed from to. The third sketch is attached to as it originally was, but since this face is now on the side (not at the top), the sketch follows its orientation and now is incorrectly positioned.

7. To fix the issue, the third sketch should be mapped to the top face again. Select the sketch, click on the ellipsis (three dots) next to the property, and choose the top face of the second pad again. Then the sketch moves to the top of the existing solid, and the third pad is generated without issues.



Remapping a sketch in this way can be done every time there is a topological naming error, however, this may be tedious if the model is complicated and there are many such sketches that need to be adjusted.

Solución


The dependency graph is a tool that is helpful to observe the relationships between the different bodies in the document. Using the original modelling workflow reveals the direct relationship that exists between the sketches and the pads. Like a chain, it is easy to see that this direct dependence will be subject to topological naming problems if any of the links in the sequence changes.

As explained in the feature editing page, a solution to this problem is to support sketches not on faces but on datum planes which are offset from the main planes of the PartDesign Body's Origin.

1. Select the origin of the PartDesign Body and make sure that it is visible. Then select the XY plane, and click on PartDesign Plane. In the attachment offset dialog, give it an offset in the Z direction so that the datum plane is coplanar with the top face of the first pad.

2. Repeat the process but this time add a larger offset so that the second datum plane is coplanar with the top face of the second pad.

3. Select the second sketch, click on the ellipsis next to the property, and then select the first datum plane. The datum plane is already offset from the body's XY plane, so no further Z offset is required for the sketch.

4. Repeat the process with the third sketch, and select the second datum plane as support. Again, no further Z offset is necessary.

5. The dependency graph now shows that the sketches and pads are supported by the datum planes. This model is more stable as each sketch can be modified essentially independently from each other.



6. Double click the second sketch and modify the shape. The second pad should update immediately without causing topological problems with the third sketch and the third pad.



7. In fact, every sketch can be modified without interfering with each other's pads. As long as the pads have sufficient extrusion length, so that they touch and form a contiguous solid, the entire body will be valid.



Notas finales
Adding datum objects is more work for the user but ultimately produces more stable models that are less subject to the topological naming problem.

Naturally, datum objects can be created before any sketches are drawn, and pads are produced. This may be helpful to visualize the approximate shape and dimensions of the final body.

Datum planes can also be based on other datum planes. This creates a chain of dependencies that could also result in topological problems; however, since datum planes are very simple objects, the risks of having these issues is less than if the face of a solid object is used as support.

Datum objects, points, lines, planes, and coordinate systems, may also be useful as reference geometry, that is, as visual aids to show the important features in the model, even if no sketch is directly attached to them.

Enlaces

 * DiseñoPieza Redondeo - Denominación topológica
 * Topological Naming, My Take, a possible solution, by realthunder.
 * Proyecto de denominación: esfuerzo para implementar una denominación topológica robusta en FreeCAD.
 * Proyecto de denominación topológica: idea para resolver el problema, por ickby.
 * Guión de datos topológicos

Vídeos

 * Why do my FreeCAD models break? - "Topological Naming Problem": A Video explanation of the underlying issues of Topological naming problem