CATIA V5 – Part Design Features Recognition

The Part Design Feature Recognition Function Part Design Feature Recognition  allows you to modify the model, although its initial specifications are lost or not available. With this function, it is possible (at least partially) to recreate tree specs, which later enable simpler modifications to the model.

The following simple example illustrates the basic elements of this function. The picture below shows a model that does not contain the specifications of individual features in the tree (no history), which occurs when a body is copied from one model to another without a link.


part_design_feature_recognition

It is possible to manually identify the individual elements of the model by clicking the Manual Feature Recognition  part_design_feature_recognition_icon. A new window opens where you can select feature (Pad, Pocket, Holes, Fillets, Chamfers, Shaft, Groove, Boolean, Draft). A hole (Holes) was selected on the picture below, then the cylindrical surface of the hole was selected. To confirm, click Apply. The Hole.1 feature was added to the tree. The system does not show a hole because it is automatically positioned in Solid.1. To see a hole, we need to position ourselves in Body.1 (Define in wok object).



positioning_in_body1_define_in_wok_object

Publications and constraints cannot be identified during the recognition process. The sketch is created as positioned and it is not associative. To make it associative it is necessary to link it to the planar surface of the model or plane.

In the same way, it is possible to recognize fillets. It is necessary to mark Fillets in the menu and select the surface. Here it is sufficient to select the front rounded surface and the system automatically recognizes the other 4 surfaces that together with the selected one make a fillet. By clicking Apply, the command ends. If we are now positioned in Body.1, the recognized hole and rounding are visible on the model as in the tree, so it is possible to edit them.


positioning_in_body1_fillet

In addition to manual recognition of individual model elements, automatic recognition can also be made by clicking on the Automatic Feature Recognition  icon_automatic_feature_recognition .In this way it is possible to recognize Hole, Fillet and Chamfer. Fillets and Chamfers are selected in the picture of the menu below. The system recognized all the Fillets that were then added to the tree.



fillets_added_to_the_tree

In some cases, the automatic recognition of rounded or sloping edges will fail. This is due to the fact that automatic recognition is closely related to geometric properties such as slope or proportion (in the case of tilted edges). In the example on the picture below, the fillet (red) will not be automatically recognized due to a small value of the angle. In order to solve this case, it is necessary to use the Manual Feature Recognition function.


manual_feature_recognition
In more complex models, the Local Feature Recognition feature allows you to identify elements on a particular part of the model instead of the entire model. It is necessary to enable the Local Feature Recognition feature in the Automatic Feature Recognition menu. In the Chain Up to Face field, select the limiting surfaces (in this case, 3 surfaces of the cyan color), in the Selected Faces field, it is enough to click one face (Face) and the system will automatically add all the others, respecting the given 3 surfaces as limiting. The All option is used with which the system searches all the model elements at once.

system_searching_for_all_elements_of_a_model_at_once

In addition to manual and automatic recognition of elements, by clicking on the Part Analysis part_analysis_icon it is possible to graphically identify Fillets and Rounds. The Part Analysis Menu is divided into two parts, the left part refers to the Rounds analysis and the right on the Fillets analysis. It is necessary to select the body and choose the color.


 selektovanje_i_biranje_bojeselecting_and_choosing_colour_2