3d modelling

Stamp

1. SECTION 1: 3D model with Fusion 360

1.1 Stamp with On Shape

Onshape is a powerful online 3D parametric CAD. The Free Plan allows free users to create and edit public data for personal and open source projects.
After sign in on cad.onshape.com, you can see this screen:

Click on Create and Document... to start a new project. Choose a Document name and Create public documente. Now you can see the navbar, the toolbar, the part studio sidebar, the part windows and the footer. In this tutorial we can ingnore navbar and footer.
In the toolbar you can found all available commands including Variable, useful to reuse more time a value and edit it later automatilly. Click on and edit the dialog box. Use width as Name and 30 as Value.

You repeat this step with depth as Name and 5 as Value. On part studio sidebar you can see the variables that you have added and after all sketchs and 3D functions used.

First to build a 3D figure you need to start from 2D draw then click on Sketch and select the Top plane. To see better what you are doing you can change the view clicking on a face or corner of the cube. In this case the Top face.

We start with a simple square: click on down arrow near the rectangle in the toolbar and select Center poinnt rectangle.

Select the origin point and click in a genric point to make a rectangle.
Note: when you pass with mouse arrow on an element (a point in this case) It will color it orange and near a icon appear. Orange rappresent the selected element and icon the constraint that you create.

Now the rectangle is blue with black center point. The blue means that the element is free to move, instead the black means that the elemnet is fixed.

Then click on Dimension and select a side of rectangle to quote the line. Use #width as value to connect the quote with the variable.

Note: now two rectangle side are black and two are blue.
To transform the rectangle in a square click on down arrow placed on right side of the toolbar and select fist the Equal constraint and after two neighbouring lines.

This is the result of first sketch:
To make it a 3D figure we Extrude but when you click on function you can't see the his direction. Then click we need to change view: click on right little cube and Isometric.

You use #depth as Depth and change direction (to simplify next steps).

Next sketch need a plane that does not coincide with any Default geometry or planar face. Then we make a Plane, use the bottom face of the extrusion (Tips: Press and hold down the mouse wheel and move it to change the view) as Entities and #depth as Offset distance.

Now make a sketch on this plane, if you can't select it you can Hide planes clicking on eye that appear when you pass mouse on it in the part studio sidebar.

Change view and Show Sketch 1. Select Text, click on two genric point, select Roboto Slab as font, Bold, Flip horizontal and write F.

Select a top right point of Sketch 1 and top right point of letter and select Coincident as constraint. Repeat with bottom left point of bottom line (Warning: the outline rectangle is not a square as Sketch 1, then you do not must select two points).

Extrude the sketch changing End type to Up to surface and select the bottom face of Extrue 1. Add Draft and use 45 as value.

Select Sketch 1 and Extrude to reuse the same sketch, but this time we select Intersect and Through all (in addition to the right direction) to remove all parts that aren't under the Sketch 1.

To design the handle create a new sketch on Front plane. Select Line and draw starting from Origin as in figure:

Select Center point circle and click on long horizontal line as starting point and on him end point as radius position.

With Tangent constraint selected, click on the circle and the oblique line. Repeat with Coincident and the end point of the oblique line.

Select Trim feature and click on left part of the circle and on the remaining section inside the area.

Now make Equal the horizontal line, the oblique line and the vertical line that connects them.

With Dimension selected, click on the veritcal line and the oblique line. Note: the two lines aren't parallel, then you quote the angle. Use 30deg as value.

Draw a horizontal line that start from end point of horizontal line already existing and ends beyond extrusion. Select the new line and click on Construction. Note: construcion geometry is ignored when the sketch region is used for features.

Make Coincident the corner of Sketch 1 and the end of construction line and Equal the two horizontal lines. Now the sketch is fixed.

Click on Revolve and select the long horizontal line as Revolve axis.

Use Fillet feature on circular face of Revolve 1 and use #width/8 as Radius.

The stamp is finished!

Export clicking with mouse's left button on Part 1 in the part studio sidebar.

Note: choose STL as Format if you want print it.

Variable

Sketch

Center point rectangle

Dimension

Equal

Extrude

Isometric

Plane

Hide

Text

Show

Coincident

Line

Center point circle

Tangent

Trim

Construction

Revolve

Fillet

Document