CATIA V5 POWER'BY Integration in Assembly Design

Commands

Behaviors in 3DEXPERIENCE

Update

Update Assistant

The 3DEXPERIENCE update status is based on 3DEXPERIENCE components may be inconsistent with the CATIA V5 update status based on CATIA V5 component.

Important:

The Update may modify instances position according to engineering connections available in 3DEXPERIENCE only, and it will ignore the V5 constraints.

Hence when opening the assembly this one maybe up-to-date in 3DEXPERIENCE and out-of-date in CATIA V5, or out-of-date in 3DEXPERIENCE and up-to-date in CATIA V5.

In a similar way, the CATIA V5 assembly constraints are ignored when moving components under constraint in 3DEXPERIENCE.

Links and Relations

You can reconnect a 3DEXPERIENCE relation with a path containing CATIA V5 instances.

Important:

CATIA V5 relations are not visible in 3DEXPERIENCE.
The synchronization is not possible when pointing not certified CATIA V5 parts.

Measure Inertia

The CATIA V5 Inertia measure features are not opened in 3DEXPERIENCE.

Engineering Connections

Fix

CATIA V5 assembly constraints are not opened in 3DEXPERIENCE.

You can create engineering connections by selecting CATIA V5 products.

Engineering connections created in 3DEXPERIENCE are not visible in CATIA V5 and saved position modifications may be not consistent in with CATIA V5 assembly constraints.

Important:

The Update may modify instances position according to engineering connections available in 3DEXPERIENCE only, and it will ignore the V5 constraints.

Hence when opening the assembly this one maybe up-to-date in 3DEXPERIENCE and out-of-date in CATIA V5, or out-of-date in 3DEXPERIENCE and up-to-date in CATIA V5.

In a similar way, the CATIA V5 assembly constraints are ignored when moving components under constraint in 3DEXPERIENCE.

Interface-based Connection

This command is based on interfaces created in dedicated 3DEXPERIENCE apps.

Manipulate

Snap

Smart Move

The positions modified by the 3DEXPERIENCE commands are propagated and visible in CATIA V5.

Moving under constraint in 3DEXPERIENCE is based on engineering connections only.CATIA V5 assembly constraints are ignored in 3DEXPERIENCE.

Assembly Hole

Assembly Protected

Assembly Cut

Assembly Added

Assembly Feature

You can create a 3DEXPERIENCE assembly feature under a CATIA V5 product and the specification feature is created in a new 3DEXPERIENCE 3D Shape.

The assembly features created in 3DEXPERIENCE are not visible in CATIA V5.

The assembly features created in CATIA V5 are not visible in 3DEXPERIENCE and affected representations are open in visualization mode in read-only.

Important:

You cannot reuse or create a specification feature in a CATIA V5 representations.
You cannot select CATIA V5 representations as affected.

Axis System

Point

Line

Plane

Positioned Sketch

Rectangular Pattern

Circular Pattern

User Pattern

You can create a new 3D Shape under a CATIA V5 product to add geometry inside it.

Important: You cannot create geometry in a CATIA V5 representation.

Derived Representation

You can create the target representation under a CATIA V5 product.

Important:

You cannot use a CATIA V5 representation as target.
You cannot select a not certified CATIA V5 representation as source.

Threads and Taps Analysis

This command is an analysis tool and does not modify the data.

Important: Non certified CATIA V5 parts cannot be analyzed.

Degrees of freedom Display

You can compute the degrees of freedom of a CATIA V5 assembly.

Degrees of freedom computation in 3DEXPERIENCE is based on engineering connections only.CATIA V5 assembly constraints are ignored in 3DEXPERIENCE.

Assembly Symmetry

The Assembly Symmetry command remains available in the Action bar and Action pad whichever the UI-active is. Its availability in the Context bar depends on the direct parent of the selected product.

Symmetric Reference:
You can apply the new reference option on a CATIA V5 reference when creating a symmetric assembly:
- for CATIA V5 product or certified part in data base.
- for instance of a CATIA V5 product or certified part in a 3DEXPERIENCE assembly.
- for 3DEXPERIENCEassembly containing a CATIA V5 sub-assembly or a certified CATIA V5 part
The resulting symmetric product is a V6 product, instantiated under a V6 product structure; it is therefore not opened in V5.

Important: Not certified CATIA V5 parts cannot be symmetrized as new reference, their instances will remain as no symmetry.
Symmetric Instance:
The Assembly Symmetry command does not modify the CATIA V5 assemblies: it is not possible to select an instance right under a V5 product and therefore instantiate the symmetric product under a CATIA V5 product.

The Assembly Symmetry command is not available in the Context bar if the direct parent of the selected product is a CATIA V5 product.

Assembly Pattern

The Assembly Pattern command remains available in the Action bar, Action pad and Context bar whichever the active product is.

Pattern feature:

You can create a new 3D Shape under a CATIA V5 product to add a new pattern feature inside it.

Important:

You can reuse a pattern feature from a certified CATIA V5 part, but this one cannot be modified.
You cannot create the pattern feature in a CATIA V5 part.

Product to pattern:
The Assembly Pattern command is allowed to modify the CATIA V5 assemblies. You can launch the command when the UI-active product is a CATIA V5 product.

When the UI-active product is a CATIA V5 product:
- The Assembly Pattern command is enabled in the Action bar, Action pad.
- You can select component under the active product..
- You cannot select component selections that do not belong to the active product. Tooltip will indicate invalid selection.
- All Instances under Component option is not available.
- The Assembly Pattern command is only available in the Context bar when selecting any product under the active product.