This is the fourth article of a series concerning how to implement and use modelling methodology in CATIA V5.
In this article, we will discuss methodology and rules for sketch definition.
|Figure 1 - The skeleton geometrical set|
We will continue using the same Angle bracket example part, introduced in previous articles.
In previous articles, we have discussed the skeleton and its internal structure and organization. The subsets are numbered so that the order of the subsets coincides with the order of element insertion, thus we can work sequentially inside the skeleton.
By this point, to start our article, we will consider that we have imported all necessary external data into our part and created all the necessary reference geometry.
All these elements are to be inserted in geometrical sets:
1. Input data and 2. Reference geometry.
As visible in figure-1, sketches are to be inserted inside geometrical sets:
3. Main sketches and 4. Auxiliary sketches, both inside the Skeleton.
In the following section, we will discuss important rules, which will help us define design intent in a sketch while guaranteeing their robustness to editions, which may be needed in the future.
Use positioned sketches when creating sketches with independent geometry.
Every sketch created will have an origin and an axis system. Positioned sketches give us options as to where to position the sketch origin and what orientation to give to its axis. On the other hand, a sliding sketch does not let us position our sketch origin and axis orientation; they are projections of the part’s axis system.
Figure 2 - Positioned sketch with geometry constrained to its axis system
If we are going to constrain our sketch geometry in relation to the sketch axis system then we should use positioned sketches, as represented in figure 2.
Figure 3 - Sliding sketch with geometry constrained to reference elements, independent from sketch axis
If we are going to constrain our sketch geometry in relation to external elements then use a sliding sketch, as seen in figure 3. Since the position of the sketch origin and its axis orientation is irrelevant, we can use a sliding sketch.
Respect the hierarchy rule when sketching.
Sketches need a support to define their planar location in space, a plane or a planar surface can be used to support them. These can be input data imported into the model or reference geometry defined in the model by the designer.
We can project or intersect input data elements or reference geometry onto sketches as these are of higher hierarchy than the sketch.
We can project or intersect geometry coming from other sketches also because they all have the same hierarchy level.
Figure 4 - Dependency ladder analysis of a sketch defined with robust methodology
Figure 4 represents the schematic dependency ladder of the sketch presented in figure 3, identified as 1-Wing shape. Notice that this sketch depends on several reference planes and another sketch and is the parent element of several core features and an additional sketch. This sketch was developed respecting the hierarchy rule.
Applying a sketch over a face (created by solid modelling features) must be avoided because it creates a parent-child relation between the support face and the sketch; modelled solid geometry is of a lower hierarchy level in relation to sketches so should never be used as a sketch support. The same is true regarding projections; if we project solid geometry in a sketch then that solid geometry becomes a parent element of the sketch.
Figure 5 - Dependency ladder analysis of a sketch defined with brittle methodology
Figure 5 represents a dependency ladder of a sketch created using the wrong methodology, which may make the model brittle. Notice that the sketch depends on previously created solid features (Pad.1 and Pad.2). The sketch is supported by Plane.1 but has projected elements created with solid features; this may lead to problems at a later stage during the part development. If the projected elements are modified, we will have update issues with sketch.13.
Fully constrain all sketches.
Sketches are to be iso-constrained when completed. Fully constrained sketches are reliable; they do not change shape unintentionally and help define design intent clearly. Figure 2 and figure 3 both represent iso-constrained sketches.
Figure 6 - Iso-constrained sketch, with reference sketch visible in the background
Figure 6 presents an iso-constrained sketch that defines the centre points of the holes that are to be applied on the main plate. The geometry represented in white belongs to the 2-Main plate (TOP) sketch, and is used as reference for positioning of the centre points.
Sketches are to be simple.
Sketches are of capital importance to define the profile of many features applied and to capture design intent into the model. This implies sketches, most likely, will be modified several times while a part is being developed so they need to be easily understandable and modifiable. Complex sketches are hard to decipher so will be hard to edit properly.
Do not apply chamfers or fillets in sketches.
Chamfers and fillets are to be applied as dress-up features on the solid model. If a model needs to be simplified at a later stage, it will be harder to adjust a sketch than it will be to deactivate or delete chamfer or fillet dress-up features.
This rule does not imply curves cannot be used to define a sketch; if the geometry can be achieved by a fillet operation at a later stage, and if the sketch can be defined without the curve then they should be removed from the sketch.
Optimize symmetry and parallelism in sketches.
Constrain all sketched geometry using the sketch axis system as the symmetry reference if sketch has symmetry elements. This will centre the geometry on the sketch axis system and will help us dimension the sketch.
Figure 7 - Symetrical sketch, centred on the sketch axis
Figure 7 presents 1-Side flange (TOP) sketch centred on its axis. Sketch 2-Main plate (TOP) is also visible in the background, for interpretation purposes only.
Intersect reference planes onto sketches.
It is quite common to have several planes added to serve as support for sketches or to be used as feature limits in a part but you can also use reference planes to drive the geometry in sketches, if so desired.
Figure 8 - Sketch with plane intersection projected in yellow
Figure 8 represents 1-Wing shape sketch with 1-Main plate height plane intersected over it, represented in yellow. The intersection is a reference to the plane and defines one edge of the sketch. If we edit the plane’s location, it will automatically change the location of the geometry in this sketch.
Always isolate external reference elements after a projecting or intersecting them with a sketch.
Having projected geometry is a great way to capture design intent into a sketch. Extending the concept presented in the rule above; projecting elements from an external file is also allowed but those external reference elements need to be isolated once the part is finished. This prevents unintentional modifications if source file is modified.
All unused elements in a sketch are to be deleted once a sketch is completed.
Deactivated or unused reference geometry will confuse a designer when editing a sketch, particularly if they were not the original sketch creators. With deactivation, we can try different variations of geometry and keep only the elements that suit the sketch’s desired shape. After this is done, however, we need to guarantee unnecessary geometry is deleted. That includes deactivated and unused reference geometry.
Number and rename a sketch after creating it.
This will help the designer pick the correct sketch for the correct feature during modelling stage and if a sketch needs editing at a later stage. Effectively the more complex the part is the more important renaming sketches will become.
If we evaluate any figure presented in this article, all sketches have been renamed in the specification tree.
In this article, we discussed the rules that should be followed during sketch definition.
In the next article, we are going to discuss the modelling stage of a part.