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Tracing patterns onto 3D Surfaces

Wednesday July 16, 2014 at 4:08pm


Usually on the support desk we encounter patterns being drawn ‘freehand’ or by inserting a 2D sketch picture onto a 2D plane to ‘trace’ over.

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 workload.


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 pattern behind.

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.  

Chris Morrogh

Applications Engineer

» Categories: SOLIDWORKS 2014

1 Comment

Seth | January 27, 2015, 6:51am
A really amazing result! I have to find out if I understood everything but it shows again the power of SOLIDWORKS.

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