PartDesign AdditiveLoft

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PartDesign AdditiveLoft.svg PartDesign AdditiveLoft

Menu location
Part Design → Additive loft
Default shortcut
Introduced in version
See also
PartDesign AdditivePipe


Additive Loft creates a solid in the active Body by making a transition between two or more sketches (also referred to as cross-sections). If the Body already contains features, the additive loft will be merged to them.

PartDesign AddLoft example.png

On the left: cross-sections (A), (B) and (C); created Additive loft on the right.


Dialog-based Workflow

  1. Press the PartDesign AdditiveLoft.svg Additive loft button.
  2. In the Select feature dialog, select a sketch to be used as base profile object and click OK.
    • Alternatively, a single sketch can be selected prior to pressing the Additive loft button.
  3. In the Loft parameters, press the Add Section button.
  4. Select the next sketch in the 3D view. Repeat to select more sketches in the order you want them to be lofted through.
  5. Set options if needed and click OK.

Selection-based Workflow introduced in version 0.19

  1. Select several sketches. It is hereby important in what order you select them:
    • The sketch selected at first will become the base profile object in the next step
    • The sketch(es) selected after the first one will become the loft section(s). Also here the selection order is important: The sketch selected as second will become the first loft section, the one selected as third becomes the second section and so on.
  2. Press the PartDesign AdditiveLoft.svg Additive loft button.
  3. Set options if needed and click OK.


  • Ruled surface: makes straight transitions between cross-sections. Dos not apply to a loft with two cross-sections. If not checked, transitions will be smooth.
  • Closed: makes a transition from the last cross-section to the first, creating a loop.


  • DataLabel: name given to the operation, this name can be changed at convenience.
  • DataSections: lists the sections used.
  • DataRuled: see Options.
  • DataClosed: see Options.
  • DataRefine: true or false. If set to true, cleans the solid from residual edges left by features. See Part RefineShape for more details.
  • DataProfile: the see base profile object of the loft.
  • DataMidplane: non applicable.
  • DataReversed: non applicable.
  • DataUp To Face: non applicable.
  • DataAllow Multi Face: non applicable.


  • Sketches must form closed profiles.
  • It is not possible to loft to a vertex.
  • A cross-section cannot lie on the same plane as the one immediately preceding it.
  • To better control the shape of the loft, it is recommended that all the cross-sections have the same number of segments. For example, for a loft between a rectangle and a circle, the circle may be broken down into 4 connected arcs.
  • Loft will be created in the order that cross sections were added

Known Issues

  • Some failure modes will turn the part black