For Pro-E, creating a round / fillet and selecting the conic option is probably the easiest method and the results will be close, but I would like to replicate the method in Pro-E similar to the method previously used in SolidWorks. The “delete face” tool in SolidWorks is useful for removing the face of a tangent fillet (C1) so that it can be replaced with a curvature continuous (C2) fillet. The technique of using a “Boundary Surface” was discussed in the previous posting, but how is this done in Pro-E as no exact equivalent exists for the “delete face” tool?

Boundary Blend "Nose"

Before I answer the question, I had remodeled the previous SolidWorks model in Pro-E using Pro-E features. The nose-shaped protrusion, which was an “indent feature” in SolidWorks, has been modeled as a “boundary Blend” using a projected curve as a base, and an intersecting sketched spline to create the top ridge surface. Pro-E has no equivalent to the “indent feature” for injection-molded plastic parts, although in sheet metal a forming tool could be used to create complex shapes.

To remove the shape edges between the main surface body, and the “nose”, a fillet feature was added. Notice that the fillet did not automatically trim the surface in the cross-section view. Therefore, this required a trim feature be used twice (top & bottom). On the second trim feature, we do not want to keep the round/ fillet, and hiding the fillet surface is probably not the best modeling practice. Instead, I discovered a trick, at least new to me, where the trimming surface can be removed after the operation.  Verify the “keep trimming surface” option is unchecked (checked by default), and the result will be an open space where the fillet previously existed (similar to SolidWorks “delete face” tool).

Trim "Nose" using fillet surface

Now comes the fun part. Create a curvature continuous (C2) fillet by using a “Boundary Blend” feature much like we previously did in SolidWorks using the “Boundary Surface” feature. Be sure to select the edge chain of each surface as a loop, and set the boundary conditions to curvature. This new surface fills in the opening or gap, and will need to be merged (knitted) to each surface. Pro-E does not permit merging more the two surfaces until Pro-E Wildfire 4.0, where in SolidWorks multiple surfaces can be knitted (merged) or trimmed in one operation.

Before shelling to produce a wall of constant thickness, a “fill” feature is used to complete the bottom, and then is merged to the previous surface body.  The merged surfaces need to be turned into a solid body using the “solidify” tool before a “shell” feature is possible. The x-section shows the completed model as a solid of constant thickness.

"Keep Trimming Surface" option unchecked

The last step is to use the “shaded curvature” tool to exam the gauss curvature (not available in SolidWorks) and the results indicate considerably less deviation in the curvature than the previous SolidWorks model (imported into Pro-E as a STEP file). Could the difference be in the tolerance of the surfaces during export (from SolidWorks) and import (into Pro-E)? As SolidWorks does not have the Gaussian Curvature tool, exporting the SW model and importing it into Pro-E seems to be only option for making the comparison.

As of SolidWorks 2010, conics in sketches or fillets is not available. My hope is SolidWorks will add this functionality in the future, although I wonder if it has been delayed as both SolidWorks and Catia are owned by the same parent company.  As Catia is more expensive, I would guess the reason it has not been added as to prevent Catia customers from migrating to SW, but I could be wrong.

Boundary Blend (C2) fillet

X-section of completed shell

Gaussian Curvature Plot (Pro-E)