Flexible Pipes between 2 Parts CATIA

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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: 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

  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

Comments

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    Jack K

    Thanks for the step-by-step instructions, AND the video.

    March 27th, 2019 17:29