Revolve

Idiom: There is more than one way to skin a cat!

Compassionate alternative: There is more than one way to peel a potato!

In Onshape, there are many ways to achieve the same outcome. None are right or wrong. Some are better for certain contexts or make modelling easier when your feature tree gets bigger and more complex. You learn modelling strategy as you gain experience.

To start to learn the revolve tool we are going to reverse engineer a water bottle.

Although we could model the main body of the bottle by extruding a circle sketch, it would require more overall extrude features to gain the same outcome so it is not the right strategy. Therefore, we are going to use the revolve tool.

Reverse engineering

Reverse engineering is the process of drawing an already existing product in a 3D modelling software to make a 3D model of it. Reverse engineering requires the taking of precise measurements so that the model is accurate. Vernier calipers and a Steel rule are two tools that can be used to take precise measurements.

vernier caliper

Steel rule

Revolve

Initial Sketch

The initial sketch here is complex and includes fillet details that could be added as separate features, however due to the nature of revolves, it is less overall work to add the fillets to the initial sketch.

You can write dimensions as a formula such as 48.75/2 means 48.75 (the diameter of the neck of the bottle) divided by 2.

Onshape helps do the maths for you!

Use the sketch fillet tool to add fillets inside the sketch

Use the dimension tool to add sizes

Revolve

Revolve takes the sketch shape and rotates it around a central Axis.

For information only, do not follow the red section!

Thin Feature

The thin feature lets you make a hollow shape directly from a revolve. It is an alternative to adding a shell.

Alternatively, you can draw your wall thickness in the sketch and revolve it.

ThE following details the modelling strategy that you will follow...

Shell

Use the shell tool to add a wall thickness of 2.5mm

Draw the lid

Make a new sketch on the front plane and match the dimensions shown in the sketch

Revolve the lid

This should be a new part

Add Fillets

The lid has fillets on the it, this time we have used the fillet feature to add these.

Offest Plane

The lid has a section of wood on it so we are going to use an offset plane to split the part and create this section

Split part

The lid is made from 2 parts so it needs to be split.

Sketch for O Ring

Revolve the O ring

Create a new Plane for the helix

The plane for the helix is an offset plane.

To accuratly measure you can use the base end of the vernier calipers

Create sketch for helix diameter

Make a new sketch on the plane you just created. Utilise the 'use' sketch function to project the inside diameter of the bottle neck onto the sketch plane.

This sketch will become a reference for your Helix which you will crerate next

Helix

Select the Helix function and apply the settings as above. Make sure to select the circular tab option and change the input type to 'Turns and pitch'

Notice how you now have curves as well as parts in the feature menu!

Create a curve point plane

Create a curve point plane, selecting the end point of the helix and the helix curve as references. This places a plane perpendicular to the end of the curve.

Add a sketch on the new plane

Draw a centre point circle with a diameter of 3mm coincident on the start point of the helix.

The circle shape matches the profile shape of the thread on the bottle.

Sweep

Adding fillets to the end of the sweep

Add the thread to the lid

For the next part I recommend that you hide some of the parts.

We are goint to repeat the same steps to create a Helix and sweep but this time on the lid...

Offset a plane from the bottom of the lid

Circle sketch

Add Helix

New plane

Thread profile Sketch

Sweep

Fillet ends of the sweep

Sketch Profile of the handle

Draw the shape with straight lines first. Get the angles correct using the dimension tool and line up the centre point of the circle with the horizontally inward pointing lines of the sketch. You can use the "Horizontal" constraint to do this.

ticking the Show constraints option in the sketch menu can help you see what constraints are acting on the sketch.

Make a new curve point plane

Make a new sketch

Make a new sketch on the handle sweep plane that you just made and sraw a centre point circle with a diameter of 4mm

Sweep

New sketch

Use the offset tool to make a circle that is bigger than the handle sweep profile by 0.33mm. This will mean the hole for the handle is bigger by 0.66 mm in total. This is a tolerance to allow the handle to fit.

Extrude

Make a remove extrude tet to through all. Notice how merge scope is set to Lid

Mirror the feature

If you were mirroring something more complex or multiple features you would tick reapply features

Offset a surface

In the feature tree, you should now have Surfaces as well as Parts and Curves

Create a tangent plane

Sketch and use type tool

Use the type tool, draw a rectangle to place the text and in the text pop up menu type your text and select your font

Extrude up to face

Offset a surface

Find an image from online

Find an Earthwell Logo image online and save it to the computer

New Tangent Plane

Make a tangent plane on the bottle using the front plane as reference

New sketch

Press insert image and then Import aat the bottom of the menu. Once the image uploads, you can select it and add it to the plane by drawing a rectangle.