Part Modeling > Construction Features > Pipes > About Pipes
About Pipes
The pipe feature is a three-dimensional centerline that represents the centerline of a pipe. Given the diameter of a pipe and, for a hollow pipe, the wall thickness, a pipe connects selected datum points either with a combination of straight lines and arcs of specified bend radius, or a spline.
After the pipe feature is created, you can view its length by clicking Tools > Feature and selecting the pipe feature.
After the pipe is created, you can modify the diameter, wall thickness (if any), and bend radii.
You can redefine the feature attributes by toggling between the following OPTION menu commands:
Geometry and No geometry—If you choose Geometry, the pipe feature is constructed with hollow or solid geometry. If you choose No geometry, the system constructs the pipe trajectory with no hollow or solid geometry.
Hollow and Solid
You cannot redefine the pipe trajectory type or toggle between the following pipe attributes:
Line/Arc and Spline
Constant Rad and Multiple Rad
You can redefine the feature references. When you choose References from the REDEFINE menu, the CONNECT TYPE and GET SELECT menus are redisplayed.
* You can insert datum points as you redefine a pipe feature. To do this, the datum points must be older than the pipe feature. If they are not, you can reorder them.
Creating Pipes in Assembly Mode
You can construct pipes in Assembly mode as either a part feature or an assembly feature.
When you create a pipe as a part feature in Assembly mode, you can use datum points on other parts. However, when you attempt to retrieve and regenerate the model in Part mode, the system issues a warning if some of the datum points belong to other parts.
Although the system displays the pipe trajectory, it will not show the "external" datum points. To resolve the conflict, you can change the pipe trajectory in Part mode by modifying the remaining datum points.
A pipe can also be an Assembly feature, although it will have no geometry. The process of creating an Assembly pipe feature is the same as described previously, but the system does not display the Geometry and No geometry options.
Creating a Part Consisting Only of a Pipe Feature
To create a part consisting only of a pipe feature, start with three default datum planes, create a datum point array, then create a pipe.
Creating Pipe Connections
For two separate pipes to be connected without creating an unattached feature, you must align their segments.
How to Create Pipe Connections
1. Create both datum point arrays using the same coordinate system.
2. Create an intermediate one-point array using that coordinate system.
3. Write relations to determine coordinates of the intermediate point, relative to those of its neighbors. For instance, in the example below, the relations are as follows:
DX6 = (DX2 + DX3) / 2
DY6 = (DY2 + DY3) / 2
DZ6 = (DZ2 + DZ3) / 2
To find the dimension symbols corresponding to the X, Y, and Z coordinates of the points, use the Info option.
4. Create the pipes, using the intermediate point as the last point in one pipe and the first in another.
5. Regenerate the model.
Compound pipe
1. First array
2. Intermediate point, located on the line connecting points 2 and 3
3. Second array
4. First pipe created through points 0, 1, 2, and 6 with bend radius R1; second pipe created through points 6, 3, 4, and 5 with bend radius R2
Specifying Part Accuracy for Pipes
The part accuracy value is very important, especially when you are creating long, thin pipes.
Creating Pipes with Multiple Radii
If you create a pipe with multiple radii, make sure all the radial values are different. Otherwise, the system creates only one dimension for equal radii and you will not be able to control them individually.
If equal radii are required, modify the pipe after it has been created.