Conversion of hybrid to Non - hybrid environment

Add Favorites
Description

Introduction

The Hybrid design option is introduced in the CATIA Version 5 Release 14 . Hybrid design / Environment is an option available in CATIA V5, used to insert wireframe and surface elements in Part bodies.
In CATIA version 5 Release 14, when a new part is opened, a dialog box containing the field “Enable hybrid design” is displayed as shown below. Selection of that will allow to work with hybrid Design.

 

 

 

 

The Fig shows the History tree created in a hybrid and non - hybrid environment.

Hybrid Design Settings

1. Select Tools > Options. A dialog box appears.

2. Select Infrastructure > Part infrastructure.

3. Click on Part document tab > Hybrid design category.

Click on the check box to enable the hybrid design as default environment and click ok, to work in hybrid environment.

Graphical Representation of Bodies and Solid Bodies in Hybrid Design

Part Body Includes solids, wireframe and surface elements.
The part body icon appears,
● Green in hybrid environment (Default environment)
● Yellow in non - hybrid environment

 

Solid Part body Cannot include wireframe and surface elements.
The solid part body icon appears,
● Gray in hybrid environment (Default environment)
● Green in non - hybrid environment

 

Advantages of Hybrid Design

  • The splitted / trimmed surfaces will not get into “No Space” window and it will be in the active window. But this will not be seen or appear visually in the active window.This will reduce the .prt fi le size.
  • The features in the history tree are in logical format, so as even a lay man can
    understand how the model is created.

Disadvantages of Hybrid Design

  • The biggest problem is the re-use of data as parent features are absorbed by the child features.
    Ex: If you split an extruded surface with a plane and then try to reuse that surface for another operation, you cannot. because it is absorbed by the child feature (Split).

  • It is diffi cult to clean-up a part that was started with hybrid bodies and switched to non-hybrid later.

Why to Clean the Hybrid Structure?

The surface elements, once used to create some child features, cannot be re-used again.

Ex: An extruded surface after splitting up with a plane cannot be used again for another operation.

Procedure to Cleanup Hybrid Designed History Tree

Let us take an example of a mobile phone with the history tree as shown:

Points to be Noted

1. The history tree shows it as hybrid design, as part body has both solids and surfaces.
2. Although the part body contains both solids and surfaces, the part body displays green color, as it’s in hybrid environment.

STEP 1: CHANGE THE PART TO NON - HYBRID ENVIRONMENT

Go to
Tools > Options > Infrastructure > Part infrastructure > Part document > Hybrid design

Deselect the check box to disablethe hybrid design

Now its noted that , as it’s converted to non-hybrid environment, the part body has changed to yellow color.

STEP 2: INSERT A BODY AND GEOMETRICAL SET

Create a body and a geometrical set under Part1 to separate the history tree (part body)

STEP 3: COPY AND PASTE - SOLIDS AND SURFACES

Copy the wireframe and surface elements from the hybrid part body and paste it in the Geometrical set.1
Similarly, copy and paste the solid from the part body and paste in the Body.1
Note:
While copying and pasting the solids, copy and paste solid features one by one in to Body.1

Thus, the history tree shows that the wireframe and surface elements are copied and pasted under Geometrical set.1 and the solids are pasted under the Body.1

STEP 4: REPLACE THE ORIGINAL WIREFRAME AND SURFACE ELEMENTS WITH THECOPIED ONES

Select sketch.1 from history tree, replace with sketch.5,(Geometrical set.1)

A replace viewer dialog box opens.
1. The first window shows the edge which needs replacement.
2. Now select the appropriate edge in the second window for replacement.
3. Be sure that the arrow directions are same. Similarly, replace the required edges, click ok.
Now, the sketch.1 is replaced and does not have any child Relation

Similarly for replacing surfaces ,

  • In the replace viewer, select the appropriate face in second window, which needs to be replaced.
  • Make sure the directions are same and enter ok.
  • Now the original surface in the part body will not have any child relation.

STEP 5: DELETE THE WIREFRAME AND SURFACE ELEMENTS IN PART BODY

After replacing the wireframe and surface elements, delete the original elements in the part body.


Note:

  • Before deleting the wireframe and surface elements check for any parent/ children relation exists for each elements.
  • If no such relation exist, delete the elements.
  • Incase any relation exist, then re-route the required relation to the newly copied ones and delete the original elements in the part body.

STEP 6: DELETION OF SOLID FEATURES IN THE PART BODY

  • Unlike surface elements, the solid features cannot be replaced.
  • The solid features, should be deleted from the last feature to fi rst feature in the part body history tree.
  • The solid features must be checked for children relation. If no such relation exist, then delete the solid feature.
  • If there ‘s any children relation, re-route the reference’s to the newly copied solid features in the body.1

Ex: The picture shows pocket.1(part body) feature has a link with child feature sketch.9(body.1).
Note:
The fi rst solid feature of the history tree can be deleted only after the deletion of all the remaining solid features.

STEP 7: CHANGE THE PART BODY

After deleting all the features in part body, the Body.1(includes pure solids) has to be changed to current part body, so as to delete the old one (yellow color ).

 

 

A dialog box as shown is displayed, click “ok” to change part body.

Thus, the part body is changed. The green color Body.1 becomes “part body” and the previous “part body” (yellow color) is changed as “Body.1 Renamed" as shown.

Now, delete the “Body.1 Renamed“ to get the history tree without hybrid Environment.
Now , the hybrid environment history tree is cleaned up to non- hybrid environment.
Finally we have,

  • Pure solids in part body and no surfaces / wireframe elements in it.
  • Green colored part body icon.
  • All surface and wireframe elements in geometrical set.
Membership Access

This video/series is available for;

Everyone
You have access
Video/Series Details
Introduction The Hybrid design option is introduced in the CATIA Version 5 Release 14 . Hybrid design / Environment is an option available in CATIA V5, used to insert wireframe and surface elements in
  • Video ID: 65
  • 0 Videos in series:
  • Running Time:
  • Added: March 22, 2014 10:57 pm
  • Category: Part Design
  • Skill Level: All Levels
  • Views: 29,799
65
All Levels
View More

Similar Videos

Not convinced? Check out some of these similar videos.