PartDesign AdditivePipe/en

Description
Additive Pipe creates a solid in the active Body by sweeping one or more sketches (also referred to as cross-sections) along an open or closed path. If the Body already contains features, the additive pipe will be merged to them.



Usage
The example image above shows two different cross-section shapes. The text below will describe the procedure with a single shape only. This will achieve a part with the same cross-section along the whole path.


 * 1) Create two separate sketches;
 * 2) * one for the path, e.g two lines connected by a curve as in the image above,
 * 3) * one for the cross-section shape, e.g. a circle as the first shape in the image above. Instead of a sketch also the face of a 3D object can be used.
 * 4) Arrange the two shapes in 3D correctly. It is recommended to place the origin of the cross-section onto the line of the path. The two sketches should in most cases be orthogonal. This can be done with the 'Map Mode' function (make both sketches visible with . Select the cross-section sketch. Select Properties/DataTab/MapMode. Click the appearing  button at the right side. In the Attachment Dialog select a vertex of the path sketch and select the correct mode to get the two sketches aligned correctly).
 * 5) Press the  button.
 * 6) In the Select feature dialog select a sketch to be used cross-section and click.
 * 7) * Alternatively, a sketch or a face of a 3D object can be selected prior to pressing the Additive pipe button. In that case you will not get a "Select feature' dialog.
 * 8) In the Pipe parameters under Path to sweep along, press the  button.
 * 9) Select the sketch to be used as path in the 3D view. In this case the whole sketch will be used as path.
 * 10) * Alternatively, single edges of the sketch can be selected by pressing and selecting edges in the 3D view. Note that you must press the  for each edge again. You must select a continous line with no branches.
 * 11) The other settings should work with the default settings in most cases.
 * 12) Click.

To use more than one cross-section, start with the first cross-section sketch as described above. Then under Section transformation set the Transform mode to Multisection; press then select a sketch in the 3D view. Repeat for each additional cross-section.

Options
Section Transformation: Section Orientation: Corner Transition
 * Select Constant to use a single profile
 * Select Multisection to use multiple profiles
 * Standard
 * This keeps the cross section shape perpendicular to the path. This is the default setting.
 * Fixed
 * Orientation set by first profile and constant throughout. This deactivates the alignment to the path normal vector. That means that the cross-section shape will not rotate with the path. Sweep along a circle to see the effect.
 * Frenet
 * Create minimum possible twisting of profile. For more info, see Frenet-Serret Formulas
 * Auxiliary
 * Specify secondary path to guide pipe.
 * For each point along the sweep path, there will be a corresponding point  on the auxiliary path.
 * As the profile is swept, it will be transformed such that the line is the normal of the sweep path.
 * If is set, then the  points are scaled proportionally along the sweep path, regardless of it's length.
 * Binormal
 * Specify binormal vector in X, Y and Z
 * Transformed
 * Right
 * Rounded

Properties
See also: Property editor.

A PartDesign AdditivePipe object is derived from a Part Feature object and inherits all its properties. It also has the following additional properties:

Data



 * : true or false. If set to true, cleans the solid from residual edges left by features. See Part RefineShape for more details.


 * : reference to sketch.
 * : extrude symmetrically to sketch face.
 * : reverses extrusion direction.
 * : face where feature will end.
 * : allow multiple faces in profile.


 * : lists the sections used.
 * : spine (path) to sweep along.
 * : true or false (default). True extends the spine to include tangent edges.
 * : secondary spine (path) to orient the Sweep.
 * : true or false (default). True extends the auxiliary spine to include tangent edges.
 * : true or false (default). True calculates the normal between equidistant points on both spines.
 * : profile mode. Options are Fixed, Frenet, Auxiliary or Binormal. See Options.
 * : binormal vector for corresponding orientation mode.
 * : transition mode. Options are Transformed, Right Corner or Round Corner.
 * : Constant uses a single cross-section. Multisection uses two or more cross-sections. Linear, S-shape and Interpolation are currently not functional.