Feature Recognition in CATIA

Rand 3D

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.

Figure 1-1   
Figure 1-1 with Feature History                     

  Figure 1-2
  Figure 1-2 with no Feature History

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.


Figure 1-3Figure 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.)

The first step is to define the Solid as the Work in Object as shown below.
Figure 1-4
Figure 1-4

Manual Feature Recognition

The first icon in the toolbar is the manual recognition. This allows the user to decide what features need to be pulled out. Click on the manual icon as shown in Figure 1-5.
Figure 1-5
Figure 1-5

A dialog box opens as shown in Figure 1-6.
Figure 1-6
Figure 1-6

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.
Figure 1-7
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.)

Figure 1-8
Figure 1-8

Now let’s move onto the holes. Select the manual feature recognition icon again. This time change to the hole feature option and select the holes in the model as shown in Figure 1-9.
Figure 1-9
Figure 1-9

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.)
Figure 1-10
Figure 1-10

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.
Figure 1-11
Figure 1-11

In order to pull out the Pad feature we need to select on a Recognize up to face. We will add the back face into the dialog box as shown in Figure 1-12.
Figure 1-12Figure 1-12

Click 'ok' to the dialog box. The Pad feature was pulled out from the Solid. The solid branch disappears since all features have been recognize as shown in Figure 1-13.
FIgure 1-13
Figure 1-13

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.
Figure 1-14
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.
Figure 1-15
Figure 1-15

Click 'ok' to the dialog box. The features have been pulled out and the solid branch is no longer represented in the specification tree as shown in Figure 1-16.
Figure 1-16
Figure 1-16

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.

First we will define ourselves into the last feature created which is Fillet.2 as shown in Figure 1-17.
Figure 1-17
Figure 1-17

Next, select the Defeature icon from the toolbar as shown in Figure 1-18.
Figure 1-18
Figure 1-18

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.
Figure 1-19

 

 

 

 

 

 

 

 


Figure 1-19

 

Click on the plus icon again. This time, select hole filter. Adjust the minimum and maximum diameter value you want CATIA to defeature as shown in Figure 1-20.
Figure 1-20
Figure 1-20

Click 'ok' to the dialog box. Both filters should be added to the defeature dialog box as shown in Figure 1-21.
Figure 1-21
Figure 1-21

Click 'ok' to the defeaturing dialog box. Notice that the features disappear from the model. Figure 1-22 shows what the model and specification tree looks like.
Figure 1-22
Figure 1-22



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