PartDesign AdditivePipe

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

 * : name given to the operation, this name can be changed at convenience.
 * : true or false. If set to true, cleans the solid from residual edges left by features. See Part RefineShape for more details.
 * : lists the sections used.
 * : true or false (default). True extends the path to include tangent edges.
 * : true or false (default). True extends the auxiliary path to include tangent edges.
 * : true or false (default). True calculates normal between equidistant points on both spines.
 * : profile mode. 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.

Limitations

 * Only up to : It is not possible to loft to a Vertex. Since you can loft from or towards single vertices of sketches or bodies.
 * A cross-section cannot lie on the same plane as the one immediately preceding it.
 * When you select a Vertex as section, it must be the last section of the pipe. You can change the order of the sections by dragging them in the list. (Otherwise the pipe body would consist at its thinnest section only of a point. This would violates the CAD kernel's definition of a 3D object.)
 * The path can only be from a single sketch, feature or ShapeBinder. In case you want to sweep along several edges from different sketches, use a.
 * The path must not contain branches or T-junctions etc. Loops are allowed.
 * It can lead to issues if the cross-section is not perpendicular to the path in 3D (some other CAD systems consider the origin of the cross-section as the path and do not require to place that sketch explicitly).
 * The cross-sections must not contain disjoint or crossing loops.