First the body of the lamp is created by revolving a closed sketch geometry on the Front Plane.
The diameter is about 1.5 inches so the top line was dimensioned at .75 inches in anticipation of the revolve. Fillets are then later added to smooth out the edges as you can see in the picture. Next we proceed to create the base piece where the threads will be created. Create a new sketch with two opposing circles on the top face of the body. Dimension them about .4 inches from the origin and extrude upwards just a tad bit, and extrude downwards using Direction 2, utilizing the 'Up to Next' extrude option.
To achieve this I sketched a circle on the bottom face of the body and extruded it to an arbitrary distance while checking the Draft button in the Extrude Property Manager in order to create a 2 degree inwards taper. I finished the base off with a smooth bottom Fillet. Notice how base is a different color. This is done by unchecking the Merge Faces feature in the Property Manager, so that the extrusion creates a new solid body. We officially have a multi-body part. A different material is then subsequently added to the body and the base, hence the contrasting colors. Next, lets add the thread.
Notice that before I have made the actual thread, a helix was made to wrap around the base which will serve us our Sweep Path for when we cut the thread. In order to make this helix, first create a plane offset from the bottom face of the body. Make sure to offset the plane at a distance around where you want the top of the thread to end. In this case, it should be just a little bit below the body. Once you have created your offset plane, create a New Sketch on it, then click Convert Entitites on the Sketch Toolbar. Notice how a sketch of a circle is created perfectly around the edge of the base.
Now once you have done this, exit the sketch you created. Select the circle and click Helix under Curves in the Features Toolbar. I used a pitch of about .125 inches and set it to 6 entire revolutions. Make sure to check the Taper Helix option in the Helix Property Manager and choose the same value that coincides with the value of the Draft option you used to extrude the base. In this case 2 degrees inward. Click the checkmark and you should have a helix like the one above. After you have made your helix, create a new 3D sketch. Now select Convert Entities and select the helix. Exit the sketch. This turns your helix into a fully defined 3D sketch. Next I'll show you how to make the actual thread.
Click on Reference Geometry on the Features Toolbar. Then select the bottom point of the helix and then click the helix curve. This will create a plane perpendicular to the curve and coincident with the bottom point. Click the OK then proceed to create a new sketch on that plane. Sketch a circle away from the helix and dimension it to about .1 inches. Next select the center point of the circle and while holding down ctrl, select the helix curvature. Add a Pierce Point relation on the Sketch Property Manager. Once you have done this, the circle should be aligned with the bottom of the Helix like in the picture above. Exit the sketch and select Sweep Cut from the Features Toolbar. Select the circle for your profile and the helix for your profile path. You should see a preview like the one above. Click OK, and voila! You can fillet the edges of your thread if you want.
Now lets add the bottom contact piece. After you created your thread click the bottom face of the base. Create a new sketch on it. Draw a circle and then extrude it outwards a small distance. Draft it about 30 degrees for the taper. Click ok. Select Dome and click the top face of the newly created contact. Play around with the distance and options until you have a nice smooth dome you are content with.
Now lets work on creating the 3D curve where you'll actually be sweeping your bulb. Create a new sketch on the front plane and draw a centerline down the middle to the origin. Starting from the bottom, create a horizontal line followed by a vertical line. Then draw a two point spline from the top to the centerline. Dimension it something like in the picture below. Add a horizontal and vertical sketch relation to the spline handles as depicted below.
Next select Revolve Surface from the Surfaces Toolbar and select the open sketch profile. The preview should look like the image below.
Now once you have created this fine piece of construction, open the display pane and check the Transparency option so that you can see through it as so.
Now let us create a new sketch on the top face of the body. Draw a centerline starting at the origin and extending outwards. Next, draw a line diagonal to it like in the picture below. Add a midpoint relationship between the newly created line and the origin. Dimension it to 45 degrees. Exit the sketch.
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Create a new sketch on the Front Plane. Draw a line coming up from the origin and dimension it about 1.125 inches as so.
We now have the entities we need to do a surface sweep. Select Surface Sweep from the Surfaces Toolbar. Select the bottom line as your sketch profile and the vertical line you just created as your sketch path. You should see this preview.
Now click the drop-box under Orientation Style in the Surface Sweep Property Manager. Select twist along path. Define the twist using turns and enter a value of 6 turns. This is what you should see in your preview.
Click OK.
You should have something like this now. Now here comes the fun part. You can make this easier by selecting the Front View. Once you've done that, under the flyout menu under Convert Entities in your Sketch Toolbar, select Intersection Curve. Select the two faces as shown in the picture below. Click OK.
A new 3D-sketch has automatically been created. Hide the last swept surfaces to observe what just happened. In the image below, only the last surface sweep was hidden. You should now have something like this if the conversion of the intersecting surfaces was successful.
Next let us add the top section to this twisting helical path. In order to do this, select Spline on Surface from under the Spline tool in the Sketch Toolbar.
Sketch a spline like the one above by clicking one of the top endpoints, the center of the dome, and the opposite endpoint. You now have a 3 point spline created on the surface of the top dome. Add an equal curvature relation to the newly created spline and the two opposing helical curves. Click View, then Temporary Axis, then create a coincident relationship between the middle spline point, and the center axis like the one pictured above. Next, lets finish the bottom half of the 3D-curve.
Create two, two point splines connecting the bottom points of your curve to the center of the extruded circles of the main body. Add an equal curvature relationship between each of the splines and the conjoined curvature. Then, select the bottom spline drag handles one by one and select Along Y axis, to make them vertical as so. Drag them upwards to about the height above. Exit the sketch. Now hide the revolved surface to get a better view of the 3D-sketch.
Pretty cool huh? Now select one of the faces where the 3D-curves meet the body. Create a new sketch on it. Sketch a circle to and dimension it about .3 inches. Select the center of the circle you just created and while holding down ctrl select the curve and add a Pierce relation. the center of the hole will align perpendicular to the curve. Now exit the sketch.
Finally, select Sweep Surface from the Surfaces Toolbar. Select the sketch containing the circle as the sketch profile and the 3D-curve as the sketch path. This is what you should see.
Click ok. You are finished. Great job!
I went a little further and added material to the bulb itself from the materials library. I used white light for a final rendered image looking like this.
Now time for me to go to bed. Lights out! Hope everyone enjoyed.
