|Part Design → Create a substractive feature → Subtractive pipe|
|Introduced in version|
|PartDesign AdditivePipe, PartDesign SubtractiveLoft|
Subtractive Pipe creates a subtractive solid in the active Body by sweeping one or more sketches (also referred to as cross-sections) along an open or closed path. Its shape is then subtracted from the existing solid. SubtractivePipe is often used in connection with Part Helix and PartDesign ShapeBinder to create a thread; see the Thread for Screw Tutorial for details.
- Press the button.
- In the Select feature dialog, select a sketch to be used as first cross-section and click
- Alternatively, a sketch or a face of a 3D object (introduced in version 0.20) can be selected prior to pressing the Subtractive pipe button.
- In the Pipe parameters under Profile, press the button.
- Select the sketch to be used as path in the 3D view:
- Alternatively, edges of the body can be selected by pressing and selecting edges in the 3D view.
- To use more than one cross-section, under Section transformation set the Transform mode to Multisection; press then select a sketch in the 3D view. Repeat for each additional cross-section.
- Set options if needed and click .
- Select Constant to use a single profile
- Select Multisection to use multiple profiles
- This keeps the cross section shape perpendicular to the path. This is the default setting.
- 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.
- Create minimum possible twisting of profile. For more info, see Frenet-Serret Formulas
- 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 Curvelinear equivalence is set, then the Q points are scaled proportionally along the sweep path, regardless of is length.
- Specify binormal vector in X, Y and Z
- 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.
- To better control the shape of the pipe, it is recommended that all cross-sections have the same number of segments. For example, for a pipe between a rectangle and a circle, the circle should be broken down into 4 connected arcs.
- You can pipe from or toward a single vertex from a sketch or the body. introduced in version 0.20
- When you select a vertex as section, it must in most cases be the last section of the pipe. You can change the order of the sections by dragging them in the list.
- 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.
- A cross-section cannot lie on the same plane as the one immediately preceding it.
- The cross-sections must not contain disjoint or crossing loops.