Advanced Assembly Design

This Article explains some advanced Catia V5 Assembly options.

• Assembly Feature Hole Series
• Flexible-Rigid Sub-Assembly
• 3D Section Cuts
• External Parameter creation
• Quick Constraint
• Constraint Creation Mode (Chain, Stack & Default Mode)
• Fast Multi-Instantiation
• Smart Move

Assembly Feature Hole Series

Using the Assembly Hole Feature, we can make different type of holes in different parts at a time.
To create a Counter bore series Hole:
1. Select the hole icon in Assembly.
2. Select the top face of a component and then click Add All Parts button. In
the Hole Defi nition panel, provide the details for a Counter bore Hole.


To create a Simple Hole series :

• Click the Add Series Button.
• In this New Series, using control button, select the required parts and then click select button.
• Notify the status changed to Yes from No.
• In the Hole Defi nition panel, give the details for a Simple Hole.

To create a Threaded Hole series

• Click Add Series Button.
• In this New Series, using control button select the required parts and then click select button.
• Notify the status changed to Yes from No.
• In the Hole Defi nition panel give the details for a Threaded Hole.

Flexible-Rigid Sub-Assembly

Normally all Sub-Assembly in a particular assembly is said to be Rigid. At Assembly level, we cannot move the components of the Sub-Assembly separately. This separate movement in Sub-Assembly can be done by making the Sub-Assembly Flexible. In this case, Chain1 is Flexible and Chain2 is Rigid. If we try to move the Link1 in Chain2, both the Link1 and Link2 get move together. However, the Link1 in Chain1 or Link2 in Chain1 can move separately. After providing update, both Link1 and Link2 will go to the original position.

• Make Chain1 as fl exible. In the specifi cation tree, the color will be changed for the Flexible Assembly.
• Give the Angle Constrained between Link 1 and Link 2 of Chain 2 and change the Angle value.
• Link 1 and Link 2 of Chain 2 will change its position. But Chain 1 is not getting affected since it is a Flexible Assembly.
• By changing the Chain 1 as Rigid from fl exible, the position of Link 1 and Link 2 of Chain 1 also changed as per Chain 2.

3D Section Cuts

For creating Sections in Assembly, we have to go for DMU Navigator.
Click Insert --- > Sectioning
By Default, it will give the Section curve of all components. However, section curves for the selected components can be created by giving
multiple selection in Selection Tab.

We can Manipulate the Section Plane through the positioning Tab available in the Section Dialog box

• We can export the Section result as Catpart, Catdwg, iges, dwg, dxf etc., through Reslt Tab.
• Preview can be set as fi lled or with grid.
• We can Lock the Section that was created in Catia through Behavior Tab.

External Parameter creation

A parameter of one part can be linked to other part so that the change in the fi rst part’s parameter will refl ect in both. Right click the parameter or
variable that needs to be changed from some other parameter or variable.

1. Go to the Edit formula from the contextual menu.
2. Click the required driven parameter along with the formula.

Quick Constraint

The Quick Constraint option will create constraints based on the selections.

1. Select the Quick constraint icon and then select the required Axis/ Face/Edge or any entities.
2. If two axis are selected then it will create coincide constraint.
3. If two planes or surfaces are selected then it will create Contact constraint.

Constraint Creation Mode (Chain, Stack & Default Mode)

1. Click the required constrained Mode and then double click any constrain (Example with Offset Constrain).
2. Select the Faces/ Entities for creating Constraints .
3. In Default Mode, every time the two selections for constraint creation need to be selected. In Stake & Chain Mode the Last selection of fi rst constraint creation will be taken as the First Selection for the next set.

Fast Multi-Instantiation

• While doing Instantiation the data will be stored.
• By clicking Fast Multi-Instantiation and clicking the component, the Instantiation will be performed immediately with the previous data available.

Smart Move

It will create the possible constraints after selection of Two faces/ Edges/Axes or any Two entities.
We can use this option for Quick constraint creation or Translation (By making Automatic Constraint creation Mode OFF).
After selection of Two entities, it will list all the possible constraints. We have to move the required constraint to the First. The Possible constraint will be created from that order shown.