In this article, we will discuss additional rules to be considered when defining part files. This article closes the main set of modelling methodology for prismatic geometry driven parts, with single body.
The following rules are inserted in this article, as a complimentary group of rules, which are to be considered additionally to the others presented in previous articles.
Part number must be defined
Every modelled part file defines the geometry of a real part; that is either bought or manufactured. For this reason, all parts need to be correctly identified with a part number defined according to company standards. This will help when files are saved, as CATIA will automatically apply the part number to the file name. It also help with instantiation at assembly level because CATIA defines the instance number according to the part number of the file instantiated in the assembly.
Do not insert geometrical sets inside bodies
A body and ordered geometrical sets are linear containers; you can define an in work object and the order of the elements will affect the final geometry.
A geometrical set is a non-linear container; there is no in work object and the order of the elements stored in them is irrelevant for the final geometry.
CATIA allows a geometrical set to be inserted inside a body but it is bad practice as their behaviour in an update cycle is different and this can cause issues in the model.
Use the publication tool
A publication is an internal pointer in a part file. Publication is useful to define all elements in a part that have external relations.
Publications are particularly interesting when working in concurrent environment or when developing a new product because links between files will be done using the published entities and their respective name instead of the elements defined in the specification tree. This makes replacing a component at assembly level much easier and avoiding all the problems with broken links.
Publish the positioning entities
Publishing the positioning entities helps to guarantee that the assembly level constraints are always linking the correct elements between files. For this reason, all positioning elements of a part should be published.
Check for micro-bodies
In some situations, usually deriving from Boolean operations and multi-body methodology, we may have a loose volume of solid geometry hovering in space next to our modelled part; these are called micro-bodies or lumps and need to be removed from the model always.
Easiest way is to apply the remove lump tool to eliminate the lump.
Break all links to external files
A finished model represents a part that is ready for production.
Beside the modelled geometry, that part file has a part number, material, mass and dynamic properties and a cost associated to it. All of these elements are considered for multiple aspects of a project and cannot be subject to unintentional change. For this reason, all external links that can affect a part and its geometry must be isolated once a part is finished and the geometry modelled in it correctly.
Delete empty containers
You can create as many bodies and geometrical sets as required in a model but remember to delete them if you are not using them when the model is complete. Empty containers make the model harder to analyse and edit at a later stage.
Hide all non-solid geometry entities
To clarify representation of parts, all geometrical entities should be in hidden space apart from the solid geometry representing the model, stored in the PartBody.Define your PartBody as your in work object before save
This will guarantee that the model’s in work object is the last geometrical feature in the body and therefor all geometrical features in the body are represented in the model.
Update before save
The update is just to guarantee that there are no unresolved elements in the model’s tree that may prevent its complete update cycle, prevent its reopening or cause issues at assembly level. This is particularly important when there is linked geometry between multiple files at assembly level.
Create Master Part (define standardized file for part families)
A master part is a part that is used to define other parts that are similar or share similar geometry. The master part is never used to represent a part for production. Master parts can have linked geometry and deactivated elements if necessary.
A master part is defined with the knowledge that it will be used to define a part family. The time used to guarantee proper design intent would be greatly compensated with the new parts created for the part family, as they are needed.
Edit similar parts
The idea behind is to never re-invent the wheel; if you need to model a part, which is similar to previously created part, then you should use the previously created part and start from there. This is why parts should be modelled with design intent and using all the rules mentioned before. As mentioned above, if you need to create a family of parts, all sharing similar geometry, then you should create a Master Part and use it as discussed above.
The use of symmetry will reduce design time and avoids unnecessary modelling. When a part is only partially symmetric, create only the symmetry for the required geometry and complete the remaining modelling operations as normal.
Declare user-defined parameters
User-defined parameters are extremely useful to convey design intent into a model, in particular, if you feel you will need to edit it at a later stage. They need to be associated to the model through formulas.
With declared user-defined parameters, you can control the model’s geometry outside the geometrical features and control multiple elements with a single parameter.
Relations are created to convey design intent in a model as required by the designer. Relations come often in the form of formulas, equivalence conditions or design tables. Relations often come together with user-defined parameters, presented above.
Do not use filters and layers in 3D design
CATIA V5 does not require layers or filters because it has geometrical sets and bodies to store wireframe and surface elements or solid geometry respectively. CATIA V5 has layers for legacy purposes only.
Multibody parts are not assemblies
Apart from a short number of exceptions (such as flo
w analysis over an assembly) a part should never represent an assembly. A multibody part should not be used as such. An assembly defined in this manner should be transformed to a product file with each body defined in individual part files.
In this article, we discussed additional rules for part file definition in CATIA V5.
In the next article, we are going to discuss surface based part design.
Figure 3 - PartBody structure, with functional groups