Imprinting Sketches Onto Bodies and Faces
You can split a surface of a face or body by imprinting a 2D or 3D sketch onto it. You can perform the sketch imprint on a CAD body or face as well as a faceted body or face.
You can then use the split surface in order to create a boundary condition within regions, for example.
Requirements
To successfully imprint a sketch onto a surface, the following criteria must be satisfied:
- The sketch can lie on the same plane as the target surface, or it can be projected onto the target surface from a distance.
- The sketch can be 2D or 3D.
- The target surface can be planar or curved.
- The sketch can contain closed loops or open profiles. Multiple profiles in one sketch are permitted.
- An open profile can terminate within the bounds of the target surface or it can cross the target surface entirely.
- If the sketch lies partially on the target surface, this part of the sketch is used to split the surface.
Creating The Imprint
In the following example, the sketch
of a circle is imprinted onto the top surface of a solid block. The sketch lies on
the plane of the top surface.
To create a sketch imprint:
- Either:
- Right-click on the desired sketch in the 3D-CAD object tree and select .
- Right-click on the desired sketch in the 3D-CAD View window and select .
The Imprint Sketch panel appears and the selected sketch is highlighted in the 3D-CAD View scene, as shown above.
- Choose the imprint options. For this case, where the sketch lies on the same plane as the body surface, the default options are appropriate. For cases where the sketch lies on a different plane, or in the case of a 3D sketch, adjust the imprint options accordingly. See Sketch Imprint Properties.
- Click OK to imprint the sketch. The imprinted sketch splits the original face of the block. The new face that is created by the imprint feature is shown highlighted below.
Sketch Imprint Properties
The sketch imprint properties control
the behaviour of the imprint for a sketch. You can imprint a sketch that lies on the
same plane as the body/face that you want to imprint, or you can project the sketch
onto a body/face that lies some distance away from it.
- Sketch
- Specifies the sketch that is imprinted onto the body surface.
- Imprint by
- Specifies the method that is used to imprint onto body surfaces.
- Sheet from Sketch—generates an artificial sheet body from the sketch with which to intersect and imprint the sketch onto the body. The sketch must lie on the same plane as the surface and the sheet must intersect the surface. This method does not support the imprinting of sheet bodies.
- Project Curves on Bodies—projects the sketch onto the selected bodies. The direction of the projection is controlled using the Direction Type and the subsequent options that appear for that particular direction type.
- Project Curves on Faces—projects the sketch onto the selected faces. The direction of the projection is controlled using the Direction Type and the subsequent options that appear for that particular direction type.
- Direction Type
- Specifies the direction of the projection. There are five options for
this:
- Proximal—specifies the direction to match the face normal. The length of the projection is specified using a maximum distance, Max Projection Distance.
- Normal—specifies the direction to be normal to the sketch plane. The sketch must be 2D.
- Reverse—specifies the direction to be the reverse of the normal direction. The sketch must be 2D.
- Specified—allows you to specify a custom direction using the Coordinate System Source options.
- Reference Axis—specifies the direction using a reference axis that you created. See Working With Reference Geometry in 3D-CAD: Reference Axes.
- Coordinate System Source
- Defines the custom direction for the projection using coordinate
systems. This option appears when you set Direction Type to
Specified. There are three options for this:
- Sketch Plane—uses the coordinate system from the sketch plane.
- Imported—uses an imported coordinate system. Select a coordinate system from the drop-down list that appears below this option.
- Reference Coordinate System—uses a reference coordinate system which you create. Click in the selection field that appears below this option and select the reference coordinate system in the 3D-CAD View scene. See Working With Reference Geometry in 3D-CAD: Reference Coordinate Systems.
- Direction Vector
- Defines the direction of the projection using X, Y, and Z direction vectors.
- Projection Options
- Specifies whether the sketch is projected forward or backwards from its initial position. One Way projects the sketch forward using the parameters that you set for the direction of the projection. Two Way projects the sketch forwards and backwards using the parameters that you specify
- Bodies/Faces to Imprint
- Specifies the bodies/faces that are imprinted by the sketch. You can imprint onto CAD sheet bodies, solid bodies, and faceted bodies as well as CAD faces and faceted faces.
- Max Projection Distance
- Specifies the maximum distance for the sketch to project. This option is only valid when you set Direction Type to Proximal. If a body or face falls within this distance, the sketch is imprinted on this body/face. Bodies/faces that lie outside this distance are not imprinted.