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.
 * 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, the cross-section sketch 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

 * Sketches used for cross-sections must form closed profiles.
 * 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 is not possible to use a vertex as cross-section.
 * 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).
 * A cross-section cannot lie on the same plane as the one immediately preceding it.
 * To better control the shape of the pipe, it is recommended that all the cross-sections have the same number of segments. For example, for a pipe between a rectangle and a circle, the circle may be broken down into 4 connected arcs.