PartDesign AdditivePipe/tr

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This page is a translated version of the page PartDesign AdditivePipe and the translation is 6% complete.
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PartDesign AdditivePipe.svg PartDesign AdditivePipe

Menu location
PartDesign → Create an additive feature → Additive pipe
Default shortcut
Introduced in version
See also
PartDesign Additive Loft, PartDesign Subtractive Pipe


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.

PartDesign AdditivePipe example.svg

On the left: cross-sections (A) and (B) to be swept along path (C); resulting Additive pipe on the right.


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;
    • one for the path, e.g two lines connected by a curve as in the image above,
    • 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. (introduced in version 0.20)
  2. 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 Space. 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).
  3. Press the PartDesign AdditivePipe.svg Additive pipe button.
  4. In the Select feature dialog, select either a sketch or a the face of a 3D object (introduced in version 0.20) to be used cross-section and click OK.
    • Alternatively, the cross-section sketch or face can be selected prior to pressing the Additive pipe button. In that case you will not get a "Select feature' dialog.
  5. In the Pipe parameters under Path to sweep along, press the Object button.
  6. Select the sketch to be used as path in the 3D view. In this case the whole sketch will be used as path.
    • Alternatively, single edges of the sketch can be selected by pressing Add Edge and selecting edges in the 3D view. Note that you must press the Add Edge for each edge again. You must select a continous line with no branches.
  7. The other settings should work with the default settings in most cases.
  8. Click OK.

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 Add Section then select a sketch in the 3D view. Repeat for each additional cross-section.


Section Transformation:

  • Select Constant to use a single profile
  • Select Multisection to use multiple profiles

Section Orientation:

  • 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
  • Auxiliary
    • Specify secondary path to guide pipe.
    • For each point P along the sweep path, there will be a corresponding point Q on the auxiliary path.
    • As the profile is swept, it will be transformed such that the PQ line is the normal of the sweep path.
    • If Curvilinear is set, then the Q points are scaled proportionally along the sweep path, regardless of it's length.
  • Binormal
    • Specify binormal vector in X, Y and Z

Corner Transition

  • Transformed
  • Right
  • Rounded


  • VeriLabel: name given to the operation, this name can be changed at convenience.
  • VeriRefine: true or false. If set to true, cleans the solid from residual edges left by features. See Part RefineShape for more details.
  • VeriSections: lists the sections used.
  • VeriSpine Tangent: true or false (default). True extends the path to include tangent edges.
  • VeriAuxiliary Spine Tangent: true or false (default). True extends the auxiliary path to include tangent edges.
  • VeriAuxiliary Curvelinear: true or false (default). True calculates normal between equidistant points on both spines.
  • VeriMode: profile mode. See Options.
  • VeriBinormal: binormal vector for corresponding orientation mode.
  • VeriTransition: transition mode. Options are Transformed, Right Corner or Round Corner.
  • VeriTransformation: Constant uses a single cross-section. Multisection uses two or more cross-sections. Linear, S-shape and Interpolation are currently not functional.


  • 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 PartDesign SubShapeBinder.svg SubShapeBinder.
  • 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.
  • The cross-sections must not contain disjoint or crossing loops.