How to model a Light Bulb using Solidworks
Hello Grabcad community! Today we are going to learn how to model and render a light bulb. In this tutorial we will take advantage of 3D sketch. I will show you how to make a composite curve and also how to model a thread, it seems that Solidworks hasn’t any specific tool to do this job. At the end of this tutorial I will try to show also how can we make renders using Photoview 360
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Step 1:
1 – Create a new part and start a new sketch on Right Plane
Still under development
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Step 2:
2 – We will draw half of the base (do not forget to draw the axis of revolutions using a line “for construction” as we will create in the next step our solid using revolve command. Draw as follows:
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Step 3:
3 – Now use Revolve command. It should looks like this:
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Step 4:
4 – Now create another sketch in the right plane, and draw a line and dimension it as follows:
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Step 5:
5 – We will create a plane perpendicular to the line created in last step and passing at the top end of it. Click in “Reference Geometry” it will show a drop-down menu where we will select “Plane”. Than follow the steps described in the image below:
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Step 6:
6 - Now we will start to create a segment of our helical geometry that composes the glass part. Create a new sketch in the plane created just in the step above (his name should be Plane1)
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Step 7:
7 – Draw a circle centred at the origin with 29 mm:
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Step 8:
8 – Now go to the top bar of Solidworks, click “Insert”, than “Curve” and finally “Helical/Spiral”. It will show a new menu where we will define our helical line. For this specific case I decided to define it by “Height and Revolutions” with 50 mm and 2 units respectively. At the end set also “Start Angle” as 0 degrees. Finally click “OK”.
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Step 9:
9 – Repeat the same as described in step 8 but now set “Start Angle” to 180 degrees.
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Step 10:
10 – Now we should link the two helical lines at the top with a kind of “chicane”. Create a new 3DSketch and use a “Spline” to connect the two helical as described in the image:
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Step 11:
11 – Select the top view than right-click over the spline and select “Insert Spline Point”
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Step 12:
12 – The new “Spline Point” should be installed over the origin as suggested in the image below:
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Step 13:
13 – We will now guarantee that our new Spline is tangencial to the two helical segments. To do this job begin to select simultaneously a helical segment and the new spline. A new menu appears on the left and you just need to click in “tangent”.
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Step 14:
14 – Repeat the step 13 but now selecting the other helical segment and simultaneously the new spline. When you finish this step the spline should be similar to the one below:
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Step 15:
15 – Return to the “Top Plane View” and manipulate the “Spline Vectors” to obtain a geometry similar to the one below. When you finish this task you can exit 3DSketch.
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Step 16:
16 – At this stage we linked the two helicals using a spline. Now we will finish this “structure” linking it to the base using a similar procedure.
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Step 17:
17 – Create a new sketch at the face shown in the image:
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Step 18:
18 – Now draw as follow:
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Step 19:
19 – Exit the Sketch and create a new 3DSketch. Next using a Spline link the two points shown in the image below:
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Step 20:
20 – Now using the same procedure as described in step 13 make the new spline tangent to the helical segment. If you experience some problems selecting the helical segment use command “Convert Entities” and mark this line as “for construction” and then you should be able to select it.
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Step 21:
21 – As we want this segment to finish vertical we need to create first a vertical line marked “for construction” at the end point and then selecting it and the spline we add a tangent relation. Create the line at the end point and to make sure it is “fully vertical” click at “Along Y” as shown in the figure below:
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Step 22:
22 – Now as described above select the vertical line and the spline and add a tangent relation. After you do this we have completed one more segment and remains only one that is the same as the previous.
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Step 23:
23 – Repeat steps from “19 to 22”
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Step 24:
24 – At this point we have completed all segments and it should look like this:
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Step 25:
25 – Now we will merge all the segments in a “composite curve”. To do this task click at the drop-down menu “Curve” in the top menu of Solidworks and select “Composite Curve”. If you don’t find the button, see the image below:
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Step 26:
26 – Select all 5 segments and then click “ok”
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Step 27:
27 – Now we only have a “composite curve”:
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Step 28:
28 – Let’s create the section to be sweeped. Create a new sketch in the plane shown in the figure:
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Step 29:
29 – Draw a circle with 8 mm of diameter centred at the end point of our composite curve as more a time as shown in the figure:
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Step 30:
30 – Let’s aplly a Sweep command using this section and our composite curve to see how beautiful will be this part :D
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Step 31:
31 – Now create a new Sketch in the plane shown in the image:
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Step 32:
32 – Draw a geometry like the one in the image
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Step 33:
33 – Now apply an extrude-cut and the end condition will be “Up to Surface” witch will be the one represented in the image:
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Step 34:
34 –Create a new sketch on the pink surface (see image step 33) and draw two concentric circles to the arc created in the last step and with 10 mm of diameter
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Step 35:
35 – Apply again an extrude-cut and use a depth of 10 mm
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Step 36:
36 – As you can see after the creation of this two holes, our “glass segment” is separated from the base. We will create a sketch on the bottom face of our segment and then extrude it until we reach the bottom of the hole. I think at this step you easily can make this task so I will jump a few steps. In the next image you see the final result:
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Step 37:
37 – Let’s move on and do our thread witch is a M27 x 3 mm. Like you will see this is easy to do and we will use tools that we already have talked about. To begin, start a new sketch in the right plane and draw a line like it’s represented in the image below:
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Step 38:
38 – Using the line and the below end point create a new plane (follow the same procedure as described in step 5). The new plane should be installed like in the image:
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Step 39:
39 – Start a new sketch In the new plane and draw a concentric circle with 27 mm of diameter
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Step 40:
40 – Then using this new sketch make a Helical segment. It should be defined by height (14.5 mm) and pitch (3mm). Make sure you have “Start Angle” as 0 degrees
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Step 41:
41 – Now let’s draw the section of the thread. Start a new sketch on the right plane and then draw as represented on the figure:
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Step 42:
42 – And finally create a “Sweep-cut” and use this profile. In the path field select this new helical segment.
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Step 43:
43 – Congrats! You have completed successfully the light bulb! Here is the final result:
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Step 44:
44 – In the next steps I will try to show how we can render our designs. We will have to turn PhotoView 360 on. To do this follow the steps presented in the next image:
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Step 45:
45 – After you activate the Photoview 360 it will appear a new tab named “Render tools”. Click it.
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Step 46:
46 – Let’s apply glass material. Select the faces (see image), than in the right menu (Appearances, Scenes and Decals) search for “clear thick glass” than right click “Add appearance to selection”. Check image:
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Step 47:
47 – Next using the same procedure we will apply “white high gloss plastic” to the base.
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Step 48:
48 – And now we will apply “polished aluminium” to the thread.
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Step 49:
49 – We now just need to apply a scene wich will be “3 Point Orange”. If you don’t find it see the image below:
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Step 50:
50 – This is the basic step you need to do a basic render. Off course, there is a lot more options that you can use such as lights for example. You can find those options in the tab shown in the next image:
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Step 51:
51 – And now the last step! Adjust the camera as you want and click “Final Render”
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Step 52:
52 – Now you just need to wait until render is completely done! If you want to share with us your own render feel free to upload it! I would love to see alternatives! Here is my own:
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Step 53:
And finally if you like it don't forget to vote "it work"
Best regards
David Nelson
