Flexible Pipes between 2 Parts CATIA

Maxime Chagnot

26 Mar, 2019 01:11 PM

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.

Do no hesitate to add comments or send me message about new topics for instance! Please subscribe and visit our website: http://www.plm-technology.com/

Use Captions and Enjoy :)

1. Step 1: Video

   
   

2. Step 2: Assembly and Parts Preparation

   Create a Physical Product (assembly)

   -

   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

   -

   Insert a new Part Called "Socket Move"

   Repeat the same step as the previous part

   -

   Go back to assembly application

   Use the engineering connection and Fix the "Socket Fix"

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

3. Step 3: 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 *

4. Step 4: 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 *

5. Step 5: 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