This class defines the methods and properties that pertain to the definition of a rib feature.
| Name | Description |
| classType |
Static function that all classes support that returns the type of the class as a string. The returned string matches the string returned by the objectType property. For example if you have a reference to an object and you want to check if it's a SketchLine you can use myObject.objectType == fusion.SketchLine.classType(). |
| setDistanceExtent |
Sets the extent type of the rib so that it extends a specified distance. This sets the extentType property to DistanceRibWebExtentType. |
| setToNextExtent |
Sets the extent type of the rib so that it extends until it intersects the next face. This sets the extentType property to ToNextRibWebExtentType. |
| Name | Description |
| creationOccurrence | In order for geometry to be transformed correctly, an Occurrence for creation needs to be specified when the rib feature is created based on geometry (e.g. sketch curves) in another component AND (the rib feature) is not in the root component. The creationOccurrence is analogous to the active occurrence in the UI |
| curves | Gets and sets an array of SketchCurve objects that form a single connected chain defining the rib profile. |
| depth | Gets the ValueInput object that defines the depth of the rib when the extent type is DistanceRibWebExtentType. Use the setDistanceExtent method to set the depth. |
| draftAngle | Gets and sets the ValueInput object that defines the draft angle applied to the rib walls. A value of zero (the default) results in no draft being applied. Setting a non-zero draft angle requires the Plastic Design Tools capability (Fusion Design Extension), otherwise setting this property fails. |
| draftPullDirection | Gets and sets the entity that defines the pull direction used when a draft angle is applied. This can be defined using either a planar BRepFace or a ConstructionPlane. A draft pull direction is required when a non-zero draft angle is set. Setting this property requires the Plastic Design Tools capability (Fusion Design Extension), otherwise setting this property fails. |
| extentType | Gets the extent type of the rib. By default this property is ToNextRibWebExtentType. Use the setToNextExtent and setDistanceExtent methods to change the extent type. |
| filletRadius | Gets and sets the ValueInput object that defines the fillet radius applied along the edges where the rib meets the target body. A value of zero (the default) results in no fillet being applied. Setting a non-zero fillet radius requires the Plastic Design Tools capability (Fusion Design Extension), otherwise setting this property fails. |
| isDraftDirectionFlipped | Gets and sets whether the draft pull direction is reversed. When false (the default), the draft uses the normal of the draftPullDirection face or construction plane. When true, the pull direction is reversed. Setting this property requires the Plastic Design Tools capability (Fusion Design Extension), otherwise setting this property fails. |
| isFlipped | Gets and sets whether the rib extrusion direction is flipped. When false (the default), the rib extends in the direction of the cross product of the sketch curve tangent and the sketch plane normal. When true, the rib extends in the opposite direction. |
| isSymmetric | Gets and sets whether the rib thickness is symmetric about the profile. By default this property is true. |
| isThicknessFromTop | Gets and sets whether the rib thickness is measured from the top of the rib rather than the bottom when a draft angle is applied. By default this property is false, meaning the thickness is measured at the bottom of the rib. Setting this property requires the Plastic Design Tools capability (Fusion Design Extension), otherwise setting this property fails. |
| isValid | Indicates if this object is still valid, i.e. hasn't been deleted or some other action done to invalidate the reference. |
| objectType | This property is supported by all objects in the API and returns a string that contains the full name (namespace::objecttype) describing the type of the object. It's often useful to use this in combination with the classType method to see if an object is a certain type. For example: if obj.objectType == adsk.core.Point3D.classType(): |
| targetBaseFeature | When creating a feature that is owned by a base feature, set this property to the base feature you want to associate the new feature with. By default, this is null, meaning it will not be associated with a base feature. Because of a current limitation, if you want to create a feature associated with a base feature, you must set this property AND call the startEdit method of the base feature, create the feature, and then call the finishEdit method of the base feature. The base feature must be in an "edit" state to be able to add any additional items to it. |
| targetBody | Gets and sets the BRepBody that the rib will be created on. |
| thickness | Gets and sets the ValueInput object that defines the thickness of the rib. |