This is the sixth article of a series concerning how to implement and use modelling methodology in CATIA V5.
In this article, we will discuss methodology and rules to be considered when defining features.
We will use the same example component, introduced in previous articles, called Angle bracket.
We discussed, in article 5, the solid modelling stage in detail; the PartBody container and how to organize features into different groups, considering their function in the part. We defined group sequence, group rules and feature naming. With this in mind, we guaranteed that our part is editable.
Editability is essential in any CAD model, regardless of the software used to model it. When we design, we want to guarantee that we can correct the model or that we can reuse it to create a new part. This saves time and increases efficiency. Feature sequence is important but most models are created with almost complete disregard for it.
Feature definition rules
The PartBody is a First Level container. In it, we will insert the solid modelling features that define the modelled geometry of a part. In the following section, we will discuss rules for feature definition that will help us implement design intent in a model, at feature level and some additional rules to be considered when modelling solid geometry.
Figure 1-The Angle Bracket part’s modelling stage
Create features that depend on external inputs first
This may seem obvious but most models are not started this way. The external inputs are driving factors for the part’s modelled geometry, therefor should be addressed first. This will help to use them as the driving elements of the parts design.
Sketches are always picked from the Skeleton
The sketches have to be defined in a geometrical set, outside the PartBody. This makes it easier to check the model’s specification tree and correct the sketches when necessary. Apart from holes, that create a sketch automatically to define the centre point, all other sketch-based features will let the user pick an existing sketch. The reasons why we should have the sketches in the Skeleton geometrical set have been discussed in previous articles.
One profile per solid feature
Apart from multipad and multipocket tool that have multiple domains by definition, the features defining solid geometry must use a single domain of a sketch (if you have several domains in a sketch and you still want to use it then you should use the sub-elements of a sketch option).
Using a single domain will guarantee that you will add or subtract one volume of material to your solid with each feature. This way you will never have two parallel extrusions controlled with a single feature; this would be confusing to analyse and harder to edit at a later stage.
Define features using reference elements
Many features can use reference elements to define height or depth instead of a dimension. Use reference elements instead of dimensional control because they help implement design intent and minimize the number of required modifications when editing a part.
Apply additive features before subtractive features
An additive feature can overlap other additive features without issue, when working on the same body and the same is true when we overlap subtractive features. We need to be careful not to refill a cavity, or the open side of a cavity, when we apply additive features so we always apply subtractive features after we apply the additive ones.
Use the most adequate axis system to define your geometry
A part can have as many axis systems defined in it as required. This can be useful for referencing to other parts at assembly level and useful to define geometrical elements using a more suitable, local, axis system.
Fix all features with warnings or errors
By the end of our modelling stage, we will have features that may have warnings or even errors and cannot be resolved properly. An unresolved element is an entity that cannot be updated properly therefor; all of these must be addressed and sorted out before a part can be considered complete.
Delete deactivated features
Deactivated features represent geometry that is not being used to define the model. For that reason, they must be deleted. If they are not deleted, these features can be reactivated at a later stage and create update issues in the model.
Master parts are the exception to this rule; they can have deactivated features because they are never sent to production and can be developed to create part families; some components may have different specification tree within the part family.
Do not recolour geometry in red or orange
Red is CATIA’s diagnostic colour, it applies it over elements that need updating and orange is the colour it applies over selected elements.
Applying any of these two colours to your geometry may cause confusion or mislead other users that may need to use models you made.
Avoid hollow voids in parts
It is perfectly possible for CATIA to create and model hollow parts. We need to be careful with these because hollow parts are complicated to manufacture and will require special manufacturing processes which are much more expensive.
When editing a part with subtractive features and if these are not positioned or defined properly, it is very easy to have situations where the designer has a subtractive feature inside the solid geometry, thus creating an accidental hollow void. These voids must be eliminated and the subtractive feature needs to be defined properly.
Never use undo features
An undo feature is a feature that is applied to remove the geometry defined in the model by other features. In many situations with complex models, it is faster and easier to apply an undo feature on a model than it is to backtrack and correct the original features to get the desired final geometry.
Applying undo features creates heavier models, because we are adding additional features to the tree and creates a snowball effect when it comes to editing because we make the model even harder to edit in a future situation.
However, undo features are essential to work with imported bodies and cannot be avoided in these situations because an imported body has no features, so cannot be edited.
Many geometrical features allow multiple input selection and affect all of them. When you define them this will work just fine, however when you need to edit the part at a later stage, complex features are harder to edit and are more brittle. In both cases, because of the number of inputs they are manipulating, this happens often with fillet features. For this reason, it is recommended to decompose a complex feature into multiple, simpler, features.
In this article, we discussed rules for feature definition in modelled parts with CATIA V5.
In the next article, we are going to discuss some additional rules to take into consideration in part files.