Round a face
Description: 5 minutes; Lab exercise: 20
minutes
Create a chain of blend-like faces in order to
tangentially connect two face parts sets.
Round a face, or Face Round, is new
functionality with OneSpace Designer Modeling 2005.
The standard blend
functionality in Modify 3D works with solids only and depends on the edges
between faces.
Features of Face Round
-
When you round a face the generated faces have
a circular cross section of a specified radius.
-
The length of the face chain can be limited by
two optional Stop Edges. Closed face chains are recognized automatically (you
don't have to specify Stop Edges to prevent the system from extending
forever).
-
By default, the boundary edges of the
generated face chain are imprinted into the defining faces to allow a simple
integration of the face chain into the model. Most likely, you will not want
to turn off Imprint because in order to integrate the faces Imprint must be
on.
-
An additional feature was added to the
Surfacing > Gather dialog in order to support the Face Round use model.
This feature is
called Split Part. The old behavior, which is also the default for this new
option, was that the Gather dialog conducted an automatic split part.
However, when
working with Surfacing, it is not desirable for the system to do an automatic
split of the part. Turn Split Part off to gather the unconnected faces into
one face part.
Limitations
- Rounding a face only works on faces of one single part.
To use Face Round on
two parts, transfer all faces of both parts into one single part.
Use the Gather
command with the Split Part option turned off.
- All generated surfaces are freeform surfaces (NURBS), even
if the defining faces are analytics.
A cross section in
surface parameter U direction would fit to a circle.
- (Any cross section through a Bspline face is a spline.
If this face is part of a model, the model is sent to Annotation and a
suitable section view is calculated -> the geometry is not a circle and no
radius/diameter dimension can be attached to the geometry.)
- There is no modification capability available with Face
Round.
Lab exercise
Work with Face Round - a new function in the Surfacing menu.
Prerequisites
- Knowledge of Surfacing - including Gather, Grow, and
Delete.
- Save the file
round_face.pkg on your system.
Round a face
- Click Surfacing
.
- Load
round_face.pkg.
- Click Round in the
Create Face section.
- Type /round_face as a name
for the part.
- Click a point on the first face (Face
1).
- Click a point on the second face (Face
2).
The system will
calculate an initial radius based on the position of the picked points and the
face normals at those picked points.

- Use the 3D CoPilot arrows to change the radius of the face
to 8. You can also choose a value from the drop-down list next to
Radius.
- Click Extend to
create a chain of faces with edges tangent to the initial face.
Use
Stop Edges to stop the chain before
the end of the tangent edge.
Imprint
will imprint the face onto the original part.
- Click
to
complete the operation.
The boundary edges
of the face chain are imprinted on the original part.
- Click Round in the
Create Face section. Proceed with
creating faces around the rest of the part.
- After selecting Face 1 and Face 2, open the
Advanced Options menu and select the
type of convexity you want in order to change the shape of the face chain. The
initial convexity of the face chain depends on the initial pick positions on
the two faces. Auto is the
default.
 Convex |

Concave |
- Continue creating face chains.
- Delete unwanted
faces in the original part.
- Gather to
integrate new faces into the model.
- If you want to generate a solid part, use
Grow or one of the other Surfacing
tools to close any remaining gaps.
Advanced Options:
- Stop Edges - Limit
the length of the face chain with one or two stop edges.
- Click Edge 1.
Click an edge on a face to shorten the chain of faces.
- Click Edge 2.
Click an edge on a face to shorten the chain of faces.