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Hello there! This time we’re going to create a speaker set with woofer and chords using SolidWorks.
Although, we’re eliminating interior components and rendering the model. I have created this tutorial with a bunch of .pdf files which describe, step-by-step, one of many approaches to the model and bunch of supplementary videos which give more insights into steps to be followed. Some of the components used in the tutorial are readily available in .step format so you can import them into any version of software you might be using (browse to Reference components folder)
The tutorial teaches you surface modeling techniques, assembly modeling basics, and associative design in which changing one component changes others referenced to it. Image below shows the outcome of this tutorial (without rendering though).
Make sure to plug-in the power cable before you render it! Or turn the power LED off prior rendering!
(Download the ‘PC_Speaker_Set_SolidWorks.rar’ document from the folder)
Although, CATIA isn’t developed to create night lamps, but still one can do so! Let’s see how.
The tutorial describes a ‘how-to’ approach to the model shown below. Note that the tutorial skips rendering techniques, maintaining the overall attention to modeling. And of course, it’s just an approach, not ‘the way’.
Thanks to the powerful surfacing capabilities of SolidWorks, it’s a little easier to create complex and innovative surfaces, say surfaces of consumer products. In this post I’ll show you how to create a plastic bottle. So let’s roll!
Let me just give you a preview of what we’re gonna end up with. Nothing says more than a photo! So here it is:
(Methodology followed in this tutorial is just a how-to approach, and not ‘the’ way to create the model.)
There are some obvious steps to be followed: Start a new part document, bring the Surface tab in the command manager, if not visible (we’ll be using SolidWorks 2011), or you can use the standard toolbar interface if preferable and then start sketching on the front plane.
Create a sketch with the dimensions as shown. Each and every sketch entity is tangent with the adjacent ones. Here sketch relations are hidden for a better view.
The curve shown top is a spline having two points and curvature radii as shown (at top is 24 mm and at bottom is 72mm). Finish the sketch and try to make it fully defined. Create a revolved surface of 360⁰ with the vertical centerline as axis which gives you this result.
Try to maintain the shape. Exit from the sketch and create a reference plane which passes from the bottom end point and is normal to the arc drawn. Draw a circle having 7.5mm radius and create a swept surface with this circle as profile and the sketch previously drawn as a path. Also make circular pattern of this swept surface body having in total 8 instances. You’ll get the following.
Use trim feature now and in mutual trim option, select all the surfaces created above, in the surfaces to keep option, select the body (obviously), and inside portion of the swept surfaces and nothing else. The result is shown below.
Create two more reference planes now, one at 40mm offset (downwards) from the top plane and another at 16mm(downwards as well) from the previous one. Draw two sketches in these two planes as shown (order doesn’t matter). Diameter of the circle will be same as the body dia.
Use Curve Through Reference Points option and join the 8 points of the above two sketches. (You could use a 3d sketch to draw these sketch eliminating need of the reference planes.) Use closed curve option.
Draw a circle on front plane now and assign a pierce relation with the curve and center-point of the circle and make a swept surface, with linear pattern in vertical direction having in total 5 instances. Hide the unnecessary elements if required. Here’s the result. (the body surface is hidden in this view).
Make another reference plane which passes from the top end point of the 72mm long line and which is also normal to the line and draw this sketch. Make sure to assign pierce relation with the arc center and the 72mm line of the previous sketch. (You could also use a 3d sketch over here to eliminate need of reference plane). And then use extrude surface tool to get this (78mm, in downward dir.)
Create circular pattern with five instances and use mutual trim to cut the surfaces. Again maintain the body and the inside portion of these extruded surfaces.
Apply 0.5mm thickness to this surface using Thicken tool.
Creating threads on top will make this a more realistic, right? So let’s do so. The top most face of the body should be planner, so make a reference plane at 20mm offset from there, draw a sketch in which create an intersection curve with the sketch plane and the cylindrical top face of the bottle mouth. Create now helix with this circle having 7.5mm pitch and 2 revolutions (start angle = 90⁰). Now to create threads more realistic, i.e., having smooth start and end transition, we need to do a little ‘workaround’ over here. So create two 3d sketches from the start and end point of the helix, which contains an arc in 3d. Each arc starts from the start and end point of the helix and is tangent with it as well. Try to get the following.
Use now the Composite Curve tool and create a combined curve consisting of the helix, and the two 3d sketches. One more reference plane needs to be created, which passes from the end point (any) of the composite curve and normal to it as well. Draw sketch on this plane like this (pierce relation with composite curve and mid-point of the vertical line.)
Use PhotoView 360 tools to create realistic images as shown below…