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diff between hybrid & non hybrid design


New member
Hybrid means Mixed... as i understand, hybrid (design) modeling is the mixture of solid modeling and surface modeling...

For product design, i would use "surface modeling" to build the whole outlook because i can build face by face, & control all surface curvatures, continuities & draft directions. After the outlook is completed, i would use "solid modeling" to build the internal mechanical features, like ribs & screw bosses. The features are simple in shape, and ineedn't build face by face. The solid-modeling features are easier to change in shape & location.

In catia, when starting a new part,you will be askedwhether Hybrid Design mode is on or off. Thisactually affects the tree structure only. For both modes, you can use surface & solid modelings together.

=========== Tree structure

If Hybrid OFF, solids will be stored in the folder "Part-body" while surfaces/curves will be in another folder "Geometrical set". On the tree, you can see both folders.

If Hybrid ON, solids/Curves/surfaces all will be stored in "part-body", which is like Solidworks

============ Parent Features Keep/ not Keep

Suppose i create an Extrude surface, then trim a hole on this surface....

If Hybrid OFF, we have two surfaces, the trimmed surface in SHOW area and the originaluntrimmed Extrude surface in NOSHOW area.

If Hybrid ON, we only have one surface, the trimmed surface. The original surface is "ABSORDBED", as Solidworks does

============ Features Grouping

If Hybrid OFF, all features in a Geometrical set can be moved into another Geometrical set anytime. The ordering is not important. It is useful to hide a group of features (maybe some surfaces with some curves)

If Hybrid ON, we cannot move a surface into a Geometrical set because the tree ordering is important. To hide a group of features,first define a "SELECTION SET" and then hide the selection set. This concept is like Layeringin UG/ Autocad.

============ Features Re-use

If Hybrid OFF, allparent surfaceswill be kept and can be found in NOSHOW area. We can re-usethem anytime

If Hybrid ON, first"ROLL BACK"the tree, justunder theparent surface, then "EXTRACT" it to duplicateone more for another feature.

==========Some comments

For simple models with little surface-modeling,both are ok;thetreewill beeasier to understand if Hybrid is ON. Solidworks enthusiasts may find easier to accept.

For complex models with lots of surfaces &curves, hybrid OFF is better. it is better for feature re-use & re-grouping.

CATIA is designed for everyone with different backgrounds and different design practices...

-Dickson SHAM