Monday June 9, 2014 at 5:27pm
In this week’s blog I’m going to show how to use a
combination of simple commands to create this seemingly complex component.
The part will start with a simple sphere, a groove will be then
cut using a path that was created using a helix and a surface. A multiple
profile sweep will create the variable cut gradient, before pattering the
groove around the sphere to achieve the desired ‘notched’ result.
After creating the sphere we will create a helix that ‘cuts’
through the body. At the centre point of the Helix sketch we will draw a
straight line, this will be the profile that we will sweep around the Helix to
create a curved surface (Pictured below).
Note: Because we are
using a Surface sweep as opposed to a Solid Sweep the profile can be a single
line.
Once this surface has been created we are able to use the
sketch tool ‘intersection curve’.
Using this tool in combination with a 3D sketch will create
a 3D sketched path where the sphere and the curved surface meet, all we have to
do is select both faces this will be used as the path for our swept cut
feature.
The next step is to create the profiles for the swept cut
groove, to do this we must create some reference planes.
The first references of these planes will be perpendicular
to the spline, the second references will be coincident to the spline end and
mid points, leaving an arrangement displayed below.
This is where simple becomes clever, we will now sketch
identical circular profiles on each plane. The two end profiles will have a
coincident relation between the circle and the endpoint so the circles appear ‘tangent’
with the 3D path and sphere.
The middle profile’s centre point is then given a pierce
relation to the spline. The difference in the location of the profile with
regard to the spline will help us achieve the variable depth cut.
A little known fact is that you are able to use multiple
profiles within a sweep feature, the order in which they are selected is
critical to the sweep feature working, you should select it in the order that
the sweep would travel i.e. from top to bottom or vice versa.
With this groove created, we can now add a fillet on the
edges to smooth it out, create an axis with two planes and with that axis apply
a circular pattern to wrap grooves around the model.
To finish the model off I applied a brushed bronze finish to
it and placed it in a Courtyard background both can be found within the standard
SOLIDWORKS appearances.
What really adds to the finish are that all the view
settings are switched on: Real Viewgraphics, ambient occlusion, shadows in
shaded mode and perspective.
By Chris Morrogh
Applications Engineer