Spiral Staircase - Scala to chiocciola - Ep.1

Hello everyone, I'm Michele Cammisa and today I'm going to deal with the Spiral Starcase design. Even if this topic in quite common among the designers web communities, I'd like to approach it by two sessions in a more pragmatic way closer to the constructive reality. So I'm not going to design the spiral staircase as a part model, but like an assembly model together with its components. This screenshot is the final result of my design. But now we start by modeling the sheet-metal side which is the main component; while for the components, I use ready-made models to save time. Let's start by a generic template, so it's better by a SolidTutorial template :-). The first step is to design the helix starting from a circle diameter 1500 mm. Thanks to "Helix" command I choose a 1500 mm pitch, number of revolutions = 1, start angle = 0 so that I get a simple point of reference. Here is the first helix. Now, in order to design the side I have to get a sheet loft: I need 2 helices for loft bend feature So I make the second helix starting like before from a circle that is 300 mm from the first one. In order to use "lofted bends" feature I have to convert the 2 helices into a 3D sketch to join them. I explained you this procedure in another Tutorial: from "Sketch 3D" menu, I choose an helix and then I convert it. The same for the second one. Now we're able to proceed with "lofted bends" feature I choose a 10 mm thickness for this side Now I need to make the holes necessary for fixing the structure. It's important to define a reference geometry to relate the holes. I need an axis that give me an angular reference to relate the plane on which I sketch the rectangle for the cut-revolve feature. Let's preselect the right and front plane, then choose "Axis" command from "Reference Geometry" Now, by "Plane" command selecting the right plane and the axis, I'm able to set a 12,5 degrees angle i.e. On this plane I'm going to sketch the rectangle and proceed by the revolved cut feature to make the hole. So, let's with a sketch of a rectangle whose dimensions I assign by the quote command. This rectangle must be referred to the intersection point with the sketch plane. In order to get all that I need to create an intersection between the sketch plane and the helicoid face. So I preselect the plane and the face, then in "Tools" menu, I go to "Sketch tools" and then I choose "Intersection Curve" that I change in Costruction line using that as the rectangle position reference. Proceeding with the "Revolved cut feature" I experience a problem because the intersection curve produced not one but 2 intersection lines so I have to remove the second line. Now I can go with the "revolved cut" feature. Here is the first hole. Now I create a Linear Pattern to obtain the second one and I choose a 100 mm distance. Now there is an important step in my design: I have to proceed to the "Driven Curve Pattern" in order to put the holes along the side It's quite important because also all the other components (the stairs i.e.) depend from this pattern. I choose the pattern as the feature so that I involve both the holes and then I choose the side as distance. I choose also the face of the side on which the holes will be perpendicular. I assign now an offset on the curve that describe the position following the helix, and I proceed. Here is the holes pattern on my sketch. I choose the pitch of my staircase. I save my component as "Side.sldprt" in a folder. Now I have to consider the other components; I start from the bar that I already designed before. I open it directly and I can build up my assembly: Open an assembly template first I insert the bar so the the side And now also the stair is necessary to my assembly, and then the support for fixing the stair to the bar. Now I take the vertical element of the banister and then the entire handrail. I proceed by mating the components thanks to the "Multiple Mate Mode" option. It's necessary now to align correctly the stair with its support; so I proceed by creating the 2 planes of simmetry for these components. Now the stair must be fixed to the side thanks to the "concentric" mating feature. Done! And now I consider the vertical element of the banister (the rod) And also here, by the "Concentric" mating functionality first, for both the holes, and then by the "Tangent" mate command, such element is correctly placed in my assembly. Now, thanks to INGWorks -the new mechanical library for SolidWorks- I choose, by drag 'n drop functionality, the right screw for fixing the element of the banister to the side of my staircase. In order to be sure the screw length is enough, by "Change Transparency Mode" command the stair appears transparent and I can check if my choice is right. For the second hole and related screw, I select the screw in INGWorks. I can invert the selection thanks to the TAB key and change its length. Now I can finish the first part of my spiral staircase design using the "feature driven Component pattern" command The components are: the stair, the support, the rod, and the hardware. The leading feature is the "driven curve pattern" within the side. Last but not the least, I select the handrail and place it by some mates: the "Coincident" mate with the side and "Tangent" mate between the external face of the handrail and the internal face of the banister. So it's enough to move it on the upper side of the banister and create the holes for fixing it. Well! the first episode of the Spiral Staircase design is at the end In the next episode I'll explain you how to correctly create and manage the design control parameters Thank you for your attention and see you soon!