Modeling with advanced techniques > Freeform parts > Create a pipe from 2D or 3D connected edges (curves)
  
Create a pipe from 2D or 3D connected edges (curves)
You can use the Pipe Add and Pipe Remove commands to create a pipe using 2D or 3D connected edges (curves).
• The Pipe Add command adds material to 2D or 3D connected edges (curves) and creates a pipe solid.
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When you add material, you can type a value in the Thickness box to create a pipe hole.
• The Pipe Remove command removes material and creates a pipe hole.
To create a pipe from 2D or 3D connected edges (curves),
1. Click Modeling and then, in the Model group, click More.
2. Click Pipe Add or Pipe Remove under Basic Sweep. The Pipe dialog box opens and Add or Remove is selected by default respectively.
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You can also select a 3D curve and click on the Command Mini Toolbar (CMT) to open the Pipe dialog box with Add selected by default.
3. Select or type a Part name.
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• Select a new or an existing part to add material.
• Select an existing part to remove material.
4. Click the Chain Selection check box if you want to select all the tangential connected 2D or 3D curves with a single click. The selection stops when two curves are not tangentially connected.
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You can also press SPACEBAR or the assigned key and click Chain on the Option Mini Toolbar (OMT).
5. Select 2D or a 3D connected edge (curve) to be used as a spine path for pipe creation. A dragger appears on the selected element.
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• You can select connected 2D or 3D planar edges, or tangentially connected 3D edges even if they are not planar.
• If the Chain Selection check box is clicked, all tangential connected edges are used as spine path.
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To select multiple connected edges,
• Press SHIFT and select the edges or,
• Press SPACEBAR or the assigned key, click on the Option Mini Toolbar (OMT), and select the edges.
6. Drag or type a value in the Diameter box to add material, or to remove material and create the pipe.
7. When you add material, you can type a value in the Thickness box to create a pipe hole.
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• If you type a positive (greater than 0) thickness value:
◦ The value in the Diameter box represents the value of the outer diameter (D1).
◦ Creo Elements/Direct Modeling calculates the value of the inner diameter (D2) as follows:
(D2) = D1 – 2*<thickness value>.
• If you type a negative (lesser than 0) thickness value:
◦ The pipe becomes larger and the value in the Diameter box represents the value of the inner diameter (D2).
◦ Creo Elements/Direct Modeling calculates the value of the outer diameter (D1) as follows:
(D1) = D2 + 2*<thickness value>.
8. Click the Check Part check box to verify the part's integrity during the pipe operation to detect a corrupt part.
9. Click to complete the operation.