Approach to model this tap in SolidWorks 2012
oops, wrong render, See attached solidworks file which matchs the rendering for technique
This tutorial will show you how to create the blended shape faucet shell shown in the above rendering. First Download the Solidworks 2014 SLDPRT file attached. Use roll back to examine each of the steps used to generate the blended solid. If you cannot use 2014, follow along in the steps to apply the technique using older versions of Solidworks
Create a sketch and extrude the circular neck.
Create a tapered rectangle sketch on the top with ends tangent to the top cylinder. Note that the end on the cylinder has two line segments. Extrude the spout.
Use move face to cant the end of the faucet spout inward.
Use move face to tilt the bottom face of the spout upward
Use move face again to tilt the top of the spout downward
Sketch a horizontal line on the front plane. Use this sketch to split the surface of the cylinder in two. This gnerates an upper upper and lower cylinder face.
Sketch a vertical line on the right plane from where the spout joins the cylinder down to the horizontal split line. Use this sketch split the cylinder face into a front and back above the horizontal split.
Sketch a circle on the bottom face of the spout with the edges made tangent to the edges of the spout. Use this sketch to split the bottom surface of the spout into multiple parts.
Select ALL of the faces shown. Use delete face to get rid of them. NOTE: at this point the part has gone from a solid model to a surface model. We'll fix this in a couple of steps.
Create a sketch on the right plane. Create a 2 point spline which has the pierce property where it touches the cut edges we generated before. Set the ends of the spine to be tangent with the surfaces they're touching.
We are now going to create a lofted surface to fill the hole which, when we're done will look like this.
Select the Lofting tool. In Group 1, Select edges in the following order, Nearest cylinder open edge, the spline we created earlier then the other cylinder open edge. Click on the green dots to get them all over to one side.
In Group 2, Select the bottom cylinder edge then activate group select to select the nearest open edge on the spout, then the curved open edge then the other open edge. The Surface will then form to smoothly fill the opening and blend the cylinder to the spout.
We now have two surfaces in the surface body folder. Select both of them then click on knit surfaces. Select try to create solid and then activate the function (green check mark). This should change the surface model back into a solid model.
Add 2mm to 8mm variable radius fillets on the top of the spout as shown for esthetics.
Add 2mm to 0mm variable radius fillets to the bottom of the spout as show for esthetics
Add 2mm constant radius fillets to the end of the spout as shown for esthetics.