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Combining Helixes, Surfaces and Sweeps.

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



Andy Fulcher | June 19, 2014, 10:59am
Good blog Chris. A nice example and well presented!
Douglas Bliss | June 19, 2014, 7:06pm
I failed. I can't make a plane using the mid point of the spline as a reference. I don't know how to select the midpoint. I can however make the part. The brute force method is to make an additional surface representing the center of the cut.
Chris morrogh | July 31, 2014, 6:09pm
Hi Douglas, I realise the confusion I must have caused, by mid point I was referring to a sketch point that I put on the spline approximately in the middle for me to select it. I seem to have forgotten about this when I was writing it up. Apologies for all the headache but I'm glad you were able to work around it!

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