A useful technique to deform a part in a controllable way, using dimensions, is the indent feature. A tool body is used to deform a target body, and at least one of the bodies must be a solid. By using the indent feature, it can replace other surfacing techniques to create similar features.

Boundary surface tool

To use the indent feature (Insert –> Features –> Indent), a tool needs to be created (surface or solid) to form the indent in a target solid body, and the tool body needs to be completely inside the indented feature. To create a spout, it is necessary to first overbuild the area above the lip in the final part. This excess material will cut away at a later stage.

I choose to create the tool body as a boundary surface with influencing sketched curves in directions 1 (X & Y) and 2 (Z). These curves can be adjusted by changing the values of the dimensions as needed. An alternative, such as the freeform feature, would not have dimensions that could be adjusted. Instead, the freeform feature is controlled by push-pull points, and is a useful feature for Industrial Designers during the initial concept phase, but not so much for manufacturing injection-molded parts.  Other alternative methods are: deform curve-to-curve (Insert –> Features –> Deform choosing the curve-to-curve option), and creating a surface feature (boundary or loft), thickening, and then combining. The later would require more work than necessary in my opinion given the functionality of the indent feature.

Indent Feature (SolidWorks)

When creating the indent feature for this spot, select the target body (solid) followed by the tool body (surface). Do not select the “cut” option as the will cut away the material instead of deforming it. Next, choose the thickness (same as wall thickness of shell), and the clearance between the tool & target body (currently set to zero). Flip the direction if necessary. The deform feature will appear, however, I think it is best to remove the tool body as it is no longer needed for other features.

Select delete body (Insert –> Features –> Delete Body) and select the tool body surface. This will remove it from view and well as from the surface body folder. The feature is not actually “deleted”, but is removed from the model tree. Delete body can be thought of as a housing cleaning tool to remove bodies (surfaces & solids) that are no longer needed.

To finish the part, the top surface needs to be cut away for the lip & spout. Select Cut with Surface (Insert –> Cut –> With Surface), and select a plane or surface to be used to cut away a solid body, and direction of cut. This leaves the part with a spout that can be modified as the design requirements changes. To eliminate the sharp edges, fillets can be added (not shown).

Finished Spout (SolidWorks)

As this part is injection molded, I recommend adding a fillet to the outside edge (example: .030 inches), and then adding a fillet to the inside edge. Create an equation where the inside fillet = outside fillet + wall thickness. The part is now finished for the purpose of this tutorial.

Concerning Pro/Engineer, I am not aware of an exact equivalent to the SolidWorks indent feature. To model this in Pro-E would require a different technique which I may discuss in a future post.