Usually on the support desk we encounter patterns being
drawn ‘freehand’ or by inserting a 2D sketch picture onto a 2D plane to ‘trace’
However on this call our customer wanted to know if there was a way for her to
transfer and cut her selected pattern onto a sphere tricky to say the least.
In the end we were able to achieve her desired result using
spherical mapping on the appearances tab, spline on surface to trace over the
pattern and delete face.
Here I will show you how to create this geometry using the fire pit as my
desired outcome and the flame as the pattern we will use.
This is how we did it:
We started off with half a sphere, later on we will use the
mirror feature to get finalise the shape.
By using a hemisphere it gives us a sense of perspective
whilst sketching which can get lost when using a sphere, it will also halve our
The flame pattern was saved as a JPEG file, a plain
appearance was then added to the spherical face of the component. It is
important that the appearance is added to the face and not the part or feature,
this is for clarity later on when we position the pattern.
Now it’s time to find the appearance we’ve added and edit
it, in the appearance file path we will browse to our pattern.
Once we select it SOLIDWORKS will convert the JPEG file into
a vector file so it can be used as an appearance.
Once this pattern has been added it becomes a case of
adjusting the size and angle of rotation in the mapping tab to achieve the
desired result. In this example because we are using a sphere the spherical
mapping option becomes a godsend as it nicely wraps the image around the curvature
of the face.
It is important to spend a bit of time at this stage getting
the positioning and size right because we will use the image to trace over the
top and will be difficult to change later on.
With our image positioned correctly we will use a little
known but very handy tool to trace over our pattern.
The ‘spline on surface’ tool creates a 3D sketch which
places every point coincident with the particular surface, thanks to this we
can quickly trace over the pattern. This tool will place a spline on any 3D
face or surface.
Found in Tools >
Sketch Entities > Spine on Surface
With our shape traced out we will use the sketch line to split the spherical
face. To do this we employed the ‘split face’ command selecting the intersect
option and using our 3D sketch as the splitting body.
Found in Insert >
Curve > Split line
This split line now allows us to select a newly created
face, having this differentiation allows us to delete it and thus leave our
Found in Insert >
Face > Delete
With our face deleted our hemisphere becomes a surface body,
we can then mirror this to achieve the spherical result below. Using our delete
face command once more we can get rid of the center faces leaving us with the
bowl that we see here.
Now I just want to add a flat to this bowl so it can sit up
straight, to do this I extruded a surface that passed through the component.
Using ‘surface trim’ I removed the excess faces leaving me with the final bowl.
This command also knits the remaining surfaces together
leaving us with a single surface body which we can now thicken so make a solid.
Found in: Insert > Surface > Trim
Insert > Surface > Thicken
It is important to remember that this technique is not
limited to spheres but with a little tweaking of the method here and there it
should be possible to place a pre-defined pattern onto most faces and surfaces.