Flexible Pipes between 2 Parts CATIA
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 :)
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
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 *
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 *
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