By Amy Rath
Have you ever had a model that was imported in as an isolated model? Meaning it didn’t have history to it or any features listed in the specification tree except a solid branch. Here is an example shown in Figure 1-1 and Figure 1-2.
If there’s no feature history displayed in the specification tree, it makes it difficult to make changes to the features. What if you need to change the fillet size or need to modify the size of the hole? In the Part Design workbench there is a toolbar that allows you to pull out features from isolated models. The toolbar is called PartDesign Feature Recognition shown in Figure 1-3.
(Note: Sometimes additional licenses need to be purchased in order to have this toolbar appear. FR1 license can sometimes be turned on under the shareable products tab in Tools > Options.)
Manual Feature Recognition
On the left hand side of the dialog box. The feature you want to recognize can be selected. We will start by pulling out the fillet. Now select the fillet in the 3D model as shown in Figure 1-7.
Click 'ok' to the dialog box. Notice that the Fillets are no longer showing in the model. CATIA added two Fillet feature branches in the specification tree as shown in Figure 1-8. Now the Fillet feature can easily be changed larger or smaller by typing in a different value into the dialog box. (Note: The reason we can’t see the fillets in the model is due to the defined object. We are still defined back in history in the Solid.)
Click 'ok' to the dialog box. The holes were removed from the model and two hole feature branches were added into the specification tree as shown in Figure 1-10. Now the hole features can easily be changed larger or smaller by typing in a different value or changing the depth option in the dialog box. (Note: The reason we can’t see the holes in the model is due to the defined object. We are still defined back in history of the Solid.)
We have one more feature to recognize in order to complete the model. We will select the manual feature recognition icon one more time. Switch the option to Pad. Select the front face to add into the dialog box as shown in Figure 1-11.
We took a model that had no history and pulled out each feature so that changes could be made easily.
Automatic Feature Recognition
The next icon in the toolbar is the automatic feature recognition. This will automatically compile the features from the options selected from the dialog box. The automatic Feature Recognition is pictured in Figure 1-14.
Turn on the Local Feature Recognition. This will allow you to select the features that you want to recognize. We will turn on Pad, Fillet, and hole as shown in Figure 1-15. Select all the faces that you want to be recognized.
DeFeature a Shape
The last icon in the toolbar is DeFeature. This means that if the feature history is there you can remove it or strip it from the model.
From the dialog box, click on the red plus icon and select the fillet option. This will open an additional dialog box allowing you to enter the minimum and maximum value in which you want CATIA to defeature as shown in Figure 1-19. Our fillets are created at a 5mm radius so putting 10mm as our maximum, CATIA will defeature these Fillets. Click ok to the Filter Filter dialog box.