# Flexible Pipes between 2 Parts CATIA

https://youtu.be/OlRkCLi2Jj4

Hello CATIA 3DExperience Fans,

Here is my last tutorial Design Fast #4 edition!

I will learn you how to design a pipe between 2 parts in Assembly Design.

1 part is fixed and can be manually moved. The pipe will automatically follow the new position and update the curve between the 2 parts.

Use Captions and Enjoy :)

1. ### Step 1: Assembly and Parts Preparation

Create a Physical Product (assembly)

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Insert a new Part called "Socket Fix"

In part Design, Sketch a circular socket Ø40mm

Use the feature Shaft to make a cylindrical socket

Add a geometrical set in the part

Create a point in the center of the cylinder

Create a line from the point and the direction of the cylinder

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Insert a new Part Called "Socket Move"

Repeat the same step as the previous part

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Go back to assembly application

Use the engineering connection and Fix the "Socket Fix"

Use the robot to move the "Socket Move" in 3D

2. ### Step 2: Create a flexible pipe

Insert a new 3D Part in the assembly

Call it "Flexible Pipe"

Switch to Generative Shape Design

Insert a geometrical set in the part

Create a spline between the 2 points using the lines as support

change the connection to Curvature continuity

* The link should be kept between the 3 parts *

Now you have a 3D Curve

Use the sweep feature with the option Radius and center

Select the 3d curve and put a Ø40mm

* The surface is created *

3. ### Step 3: Transform a Surface into a Solid

The pipe surface is created in the geometrical set

now define in work object the body and switch to Part Design

Click on the feature Thick Surface

Select the pipe surface created

put 2mm thickness

* The pipe is now a solid *

4. ### Step 4: Move the socket and update the Assembly

It is time to go back to assembly design

Use the robot to move in 3D the "Socket Move"

* the pipe will become red *

Use the update button

* the pipe is updated and it will follow the direction of the new socket *

[ Be careful, if the curve is too curvy, you will have singularity in your design and the pipe will not be created ]

• End of the tutorial