The Part Design Workbench aims to provide tools for modelling complex solid parts and is based on a Feature editing methodology. It is intricately linked with the Sketcher Workbench.
The sketch is the building block for creating and editing solid parts. The workflow can be summarized by this: a sketch containing 2D geometry is created first, then a solid creation tool is used on the sketch. At the moment the available tools are:
- Pad which extrudes a sketch
- Pocket which creates a pocket on an existing solid
- Revolve which creates a solid by revolving a sketch along an axis
- Groove' which creates a groove in an existing solid
More tools are planned in future releases.
A very important concept in the PartDesign workbench is the sketch support. Sketches can be created on standard planes (XY, XZ, YZ and planes parallel to them) or on the face of an existing solid. For this last case, the existing solid becomes the support of the sketch. Several tools will only work with sketches that have a support, for example, Pocket - without a support there would be nothing to remove material from!
After solid geometry has been created it can be modified with chamfers and fillets or transformed, e.g. mirrored or patterned.
The Partdesign workbench is meant to create a single, connected solid. Multiple solids will be possible with the Assembly workbench.
The Part Design tools are all located in the Part Design menu that appears when you load the Part Design module.
They include the Sketcher Workbench tools, since the Part Design module is so dependent on them.
The Sketcher Tools
These are tools for creating objects.
- Point: Draws a point
- Arc: Draws an arc segment from center, radius, start angle and end angle
- Circle: Draws a circle from center and radius
- 2-point Line: Draws a line segment from 2 points
- Polyline (multiple-point line): Draws a line made of multiple line segments
- Rectangle: Draws a rectangle from 2 opposite points
- Fillet: Makes a fillet between two lines joined at one point. Select both lines or click on the corner point, then activate the tool.
- Trimming: Trims a line, circle or arc with respect to the clicked point.
- External Geometry: Creates an edge linked to external geometry.
- Construction Mode: Toggles an element to/from construction mode. A construction object will not be used in a 3D geometry operation.
Constraints are used to set rules between sketch elements, and to lock the sketch along the vertical and horizontal axes.
- Lock: Creates a lock constraint on the selected item by setting vertical and horizontal dimensions relative to the origin (dimensions can be edited afterwards).
- Coincident: Creates a coincident (point-on-point) constraint between two selected points.
- Point On Object: Creates a point-on-object constraint on selected items.
- Horizontal Distance: Fixes the horizontal distance between 2 points or line ends. If only one item is selected, the distance is set to the origin.
- Vertical Distance: Fixes the vertical distance between 2 points or line ends. If only one item is selected, the distance is set to the origin.
- Vertical: Creates a vertical constraint to the selected lines or polylines elements. More than one object can be selected.
- Horizontal: Creates a horizontal constraint to the selected lines or polylines elements. More than one object can be selected.
- Length: Creates a length constraint on a selected line.
- Radius: Creates a radius constraint on a selected arc or circle.
- Parallel: Creates a parallel constraint between two selected lines.
- Perpendicular: Creates a perpendicular constraint between two selected lines.
- InternalAngle: Creates an internal angle constraint between two selected lines.
- Tangent: Creates a tangent constraint between two selected entities, or a colinear constraint between two line segments.
- Equal Length: Creates an equality constraint between two selected entities. If used on circle or arcs, the radius will be set equal.
- Symmetric: Creates a symmetric constraint between 2 points with respect to a line.
- New Sketch: Creates a new sketch on a selected face or plane. If none were selected, the default work plane XY will be used.
- View sketch: Sets the model view perpendicular to the sketch plane.
- Map sketch: maps a sketch to the previously selected face of a solid.
- Leave Sketch: Leave the Sketch editing mode.
The Part Design Tools
These are tools for creating solid objects or removing material from an existing solid object.
- Pad: Extrudes a solid object from a selected sketch.
- Pocket: Creates a pocket from a selected sketch. The sketch must be mapped to an existing solid object's face.
- Revolution: Creates a solid by revolving a sketch around an axis. The sketch must be a closed profile to get a solid object.
- Groove: Creates a groove by revolving a sketch around an axis. The sketch must be mapped to an existing solid object's face.
These are tools for modifying existing objects. They will allow you to choose which object to modify.
- Fillet: Fillets (rounds) edges of an object.
- Chamfer: Chamfers edges of an object.
- Draft: Applies angular draft to faces of an object.
These are tools for transforming existing features. They will allow you to choose which features to transform.
- Mirrored: Mirrors features on a plane or face.
- Linear Pattern: Creates a linear pattern of features.
- Polar Pattern: Creates a polar pattern of features.
- Scaled: Scales features to a different size.
- MultiTransform: Allows creating a pattern with any combination of the other transformations.
Some optional functionality that has been created for the PartDesign Workbench:
- Shaft design wizard: Generates a shaft from a table of values and allows to analyze forces and moments
There are two types of feature properties, accessible through tabs at the bottom of the Property table: View properties and Data properties. All the properties of a feature that can be accessed through the dialog which opens when you edit the feature appear on the Data tab.
Every feature has a placement that can be controlled through the Data Properties table. It controls the placement of the part with respect to the coordinate system. NOTE: The placement options do not affect the physical dimensions of the feature, but merely its position in space!
The Angle argument specifies the angle to be used with the axis option (below). An angle is set here, and the axis that the angle acts upon is set with the axis option. The feature is rotated by the specified angle, about the specified axis. A usage example might be if you created a revolution feature as required, but then needed to rotate the whole feature by some amount, in order to allow it to line-up with another pre-existing feature.
This option specifies the axis/axes about which the created feature is to be rotated. The exact value of rotation comes from the angle option (above). This option takes three arguments, which are passed as numbers to either the x, y, or z boxes in the tool. Adding a value to more than one of the axes will cause the part to be rotated by the angle in each axis. For example, with an angle of 15° set, specifying a value of 1.0 for x, and 2.0 for y will cause the finished part to be rotated 15° in the x-axis AND 30° in the y-axis.
This option specifies the base point to which all dimensions refer. This option takes three arguments, which are passed as numbers to either the x, y, or z boxes in the tool. Adding a value to more than one of the boxes will cause the part to be translated by the number of units along the corresponding axis.