Sahaj Panchal's Blog

Your 'Freesource' for CAD Education.

Create bottle in SolidWorks


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:

clip_image002 Don’t be scared! It’s easy with SolidWorks. Let’s see how.

(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.

clip_image004 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.

clip_image006 Now create a sketch on front plane approximately as shown.

clip_image008 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.

clip_image010 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.

clip_image011 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.

clip_image013clip_image015

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.

clip_image017Draw 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).

clip_image019 Again use the trim surface tool and select all the surfaces and in keep selection box, select the body and the inside portion of the above surfaces.

clip_image020 Now let’s create the remaining bottom surfaces. To do so, draw a sketch on front plane.

clip_image022 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.)

clip_image024clip_image026

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.

clip_image028 Apply fillet to the sharp edges(highlighted in a fig below), having radius equal to 1mm, 1mm, and 4mm (from top to bottom).

clip_image032clip_image033

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.

clip_image035clip_image037

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.)

clip_image038 Use Swept boss/base tool to create threads, but notice that it’s been extended ‘into’ the bottle mouth, which is not necessary, so you can use revolved cut and remove it.

clip_image040 clip_image042 That’s it! The bottle is ready!!


Use PhotoView 360 tools to create realistic images as shown below…

clip_image044

clip_image046

Advertisements

2 responses to “Create bottle in SolidWorks

  1. Dillon Chaffey (Chafflube) July 31, 2012 at 2:09 PM

    Excellent tutorial. Very well written and very informative. Good work, mate!

Leave a Reply

Fill in your details below or click an icon to log in:

WordPress.com Logo

You are commenting using your WordPress.com account. Log Out / Change )

Twitter picture

You are commenting using your Twitter account. Log Out / Change )

Facebook photo

You are commenting using your Facebook account. Log Out / Change )

Google+ photo

You are commenting using your Google+ account. Log Out / Change )

Connecting to %s

%d bloggers like this: