Toothbrush Head Stand

A daily-life problem
Electric toothbrushes rarely come with a head stand, while in a family you will often see multiple heads used with one body. Many people facing a common problem lead us to a variety of solutions, as you can see on Thingiverse (200-800 projects are related to that). Here is the first answer and how to design it.

This tutorial will take you through the steps needed to model the part shown in the image below using basic tools from the Part Design Workbench (many of the tools and capabilities are not covered).



First idea : a plate

 * From the start-page, select [[Image:Workbench_PartDesign.png‎‎]] Part Design, or create a new document and select the Part Design workbench.

Create a sketch

 * Click on [[Image:Sketcher_NewSketch.png|32px]] New sketch. Either from the contextual task menu at the left, or the toolbar above or from the Part Design menu at the top.

A dialog prompts you to choose the sketch orientation and provide an offset.


 * We will pick the XY Plane as shown in the image above (that orientation correspond to the common build plate of most 3D printers), then click OK.



You now are facing the XY plane from above, and have access to the drawing tools.


 * Click on Sketcher_CreateRectangle.png Rectangle.
 * Place a first point.
 * Place the opposite corner.
 * Press or click the right mouse button to stop using the tool.



You now have a floating rectangle of unspecified dimensions.


 * Click on a line of the rectangle, you now have access to the constraint tools at the right of the toolbar (depending of the size of your screen you may need to drag them to the left in order to see them all)
 * Click on Constraint_Length.png Length
 * A dialog prompts you to set a dimension. Enter 80mm, click OK.
 * Repeat with the other side of the rectangle, also 80mm.



You now have a floating square.


 * Click on the lower left point of the square.
 * Click on the origin of the XY plane (at the intersection of the two thick lines).
 * Click on Constraint_PointOnPoint.png Coincident.



You now have a totally constrained sketch, as you are told by the solver on the left and the change of color. It is a good practice to always have a totally constrained sketch.

An under-constrained sketch can leave room for unwanted change, if you modify something later on. On the opposite, an over-constrained sketch is also not good. In that case the solver warn you of redundant constraints and you should remove some of them.


 * To leave the sketch, click either on the "Close" button on the left, or the Sketcher_LeaveSketch.png icon in the toolbar, or press.



You now only see the square, and the contextual task menu on the left show you more options than before.

Create a pad

 * Click on [[Image:View-axometric.png|32px]] Axonometric among the standard views, to better see what will happen.
 * Click on PartDesign_Pad.png Pad.
 * Enter 4mm and click OK.



Your sketch is now in volume !

Create a sketch on it

 * Select the upper face



The color of the face change and you have more options in the contextual task menu.


 * Click on [[Image:Sketcher_NewSketch.png|32px]] New sketch. As a face was selected it will not ask you to choose a plane.




 * Click on Sketcher_Circle.png Circle, place the center, then the radius.
 * Draw 4 circles
 * Press or click the right mouse button to stop using the tool.




 * Select the circles
 * Click on Constraint_EqualLength.png Equal Length



Now the circles share the same radius.


 * Click on Sketcher_External.png External geometry.
 * Click on the four sides of the square, it add lines, color magenta.



Theses lines will serve as reference to position the circles.


 * Use Constraint_Length.png Length to position them at 20mm from the edges.




 * Click on a circle
 * Click on Constraint_Radius.png Radius and set it at 1,5mm.




 * To leave the sketch, click either on the "Close" button on the left, or the Sketcher_LeaveSketch.png icon in the toolbar, or press.



Create a pad

 * Click on [[Image:View-axometric.png|32px]] Axonometric among the standard views, to better see what will happen.
 * Click on PartDesign_Pad.png Pad.
 * Enter 25mm and click OK.



You have the basic shape, it just need final touches.

Rounding the corners

 * Holding click on the vertical edge at each corner to select the four of them.

Don't hesitate to help you by switching the display mode (just at the left of the Axonometric View) between Wireframe and  Wireframe and shadow.




 * Click on PartDesign_Fillet.png Fillet.
 * Set the radius at 20mm.



Much better.

Making it more robust
We need to add material at the base of the cylinders to make them less prone to snap. Because of the printing orientation these small surfaces will be fragile at the junction with the base.


 * Select the circles at the base of the cylinders




 * Click on PartDesign_Chamfer.png Chamfer.
 * Set it to 2mm.



Chamfer the edges

 * Select the face under the base, add a PartDesign_Chamfer.png Chamfer of 0,5mm.

The first layer of plastic is often being squashed a little too much, this will compensate that and save you time in cleaning the model. If the first layer is ok that will make it only nicer




 * Select the edges at the border of the upper face (holding ).




 * Add a PartDesign_Chamfer.png Chamfer of 1mm. This one is only aesthetic.



Tadaa !

Export as a .STL

 * In the Combo View on the left, select the tree view instead of the contextual task menu, click on the last feature (the chamfer).




 * Now you can select "Export..." from the File menu at the top left, and select the file format .STL.
 * Just print it :-)

Second idea : a band
The above model make a good starting point to use FreeCAD, but as a toothbrush head stand it have its flaws.

To be continued