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You
can create parts and part features quickly and simply using
the powerful “Thin Feature” option in SolidWorks.
An entire part can be created using a simple open sketch entity
inside a standard feature, such as extrude or revolve, by
checking the thin feature option. This option allows a thickness
to be created off the sketch in one-direction, from the mid-plane
or in two-direction, at different thicknesses. Depending on
the type of feature you can also auto-fillet corners or cap
ends. Best of all, this all takes place in one feature.
See the examples and types below, on how this is done.
Extrude Thin Feature Uses an open or closed sketch, single
or multiple entities. A closed sketch results in a hollow
part. The example below shows two sketch entities with the
thin feature option set to one-direction, the thickness set
to .10 and the auto-fillet corners option set to .125.
If
the reverse direction option is selected, notice the same
part is now built to the outside of the line instead of the
inside line, in the next image. Compare this to the previous
image.
If you select the Mid-plane option
the thickness will cross the sketch entity evenly in both
directions.
If you select the Two-directions
option the thickness will cross the sketch entity but allow
for a different thickness in each direction.
The next image shows the resulting
part with the auto-filleted corner.
Adding two more sketch lines results
in opened end box, notice we now have the option to cap the
ends.
If check the "cap ends" option,
we now have hollow closed box.
Revolve Thin Feature
Uses an open or closed sketch. A closed sketch results in
a hollow part. The example below shows two open sketch entities
with the thin feature option set, using a similar sketch as
the first example but with a centerline add to revolve around.
The
next image shows the same feature with a closed sketch. Again
notice the hollow part.
Extruded
Cut Thin Feature , Must
be a closed sketch, must be used on an existing solid feature,
results in multiple bodies. In this example a cylinder has
a circular sketch on the top face cutting down through the
part with the thin feature outside the sketch.
This
image shows the part with the option to keep all bodies or
selected bodies.
The
final part, notice the two bodies in the solid bodies folder.
Revolve
Cut Thin Feature , Must
be a closed sketch, must be used on an existing solid feature,
results in multiple bodies. In this example a cylinder has
a circle sketch revolved around it with the thin feature selected
and a thickness set a half toroidal section will be cut away.
This
image shows the part with the option to keep all bodies or
selected bodies.
The
final part shown in section view, notice the two bodies in
the solid bodies folder.
Swept
Thin Feature
Must have at least one closed Sketch profile and one separate
sketch path. In this example two sketches are created the
first ellipse for the profile the second spline for the path.
In this case the Mid-plane option is selected.
This
is the resulting part, with the thin feature option selected.
Loft
Thin Feature
Must have two separate closed sketches and can have other
open sketch entities for guidelines but entity end points
should pierce both closed sketches. In this example three
sketches are created and dissimilar entities are lofted together,
a rectangle is lofted to a circle along the guideline of a
spline sketch.
The
thin feature is added with the one-direction set outside the
sketch.
The
resulting part
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