Toothbrush Head Stand

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Base ExampleCommandModel.png Tutorial
Topic
Modeling
Level
Beginner
Time to complete
1 hour
Author
EmmanuelG
FreeCAD version
0.16 or greater
Example files
Thingiverse 2403310


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).

TBHS-model.png

First idea : a plate

  • From the start-page, select Workbench PartDesign.png Part Design, or create a new document and select the Part Design workbench.
TBHS-0.png

Create a sketch

  • Click on Sketcher NewSketch.png New sketch. Either from the contextual task menu at the left, or the toolbar above or from the Part Design menu at the top.
TBHS-1.JPG


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.
TBHS-2.JPG


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

  • Click on Sketcher CreateRectangle.png Rectangle.
  • Click to place a first point.
  • Click to place the opposite corner.
  • Press ESC or click the right mouse button to stop using the tool.
TBHS-3.JPG


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 Sketcher ConstrainDistance.png Distance
  • A dialog prompts you to set a dimension. Enter 80mm, click OK.
  • Repeat with the other side of the rectangle, also 80mm.
TBHS-4.JPG


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 Sketcher ConstrainCoincident.png Coincident.
TBHS-5.JPG


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 ESC.
TBHS-6.JPG


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 View-axometric.png Axonometric among the standard views, to better see what will happen.
  • Click on PartDesign Pad.png Pad.
  • Enter 4mm and click OK.
TBHS-7.JPG


Your sketch is now in volume !

Create a sketch on it

  • Select the upper face
TBHS-8.JPG


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

  • Click on Sketcher NewSketch.png New sketch. As a face was selected it will not ask you to choose a plane.
TBHS-9.JPG


  • Click on Sketcher Circle.png Circle, click to place the center, move the pointer and click to define the radius.
  • Draw 4 circles on the pad (of any size)
  • Press ESC or click the right mouse button to stop using the tool.
TBHS-10.JPG


TBHS-11.JPG


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.
TBHS-12.JPG


Theses lines will serve as reference to position the circles.

  • Use Sketcher ConstrainDistance.png Distance to position them at 20mm from the edges.
TBHS-13.JPG


  • Click on a circle
  • Click on Sketcher ConstrainRadius.png Radius and set it at 1,5mm.
TBHS-14.JPG


  • To leave the sketch, click either on the "Close" button on the left, or the Sketcher LeaveSketch.png icon in the toolbar, or press ESC.
TBHS-15.JPG

Create a pad

  • Click on View-axometric.png Axonometric among the standard views, to better see what will happen.
  • Click on PartDesign Pad.png Pad.
  • Enter 25mm and click OK.
TBHS-16.JPG


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

Rounding the corners

  • Holding CTRL 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 DrawStyleWireFrame.svg Wireframe and DrawStyleFlatLines.svg Wireframe and shadow.

TBHS-17.JPG


  • Click on PartDesign Fillet.png Fillet.
  • Set the radius at 20mm.
TBHS-18.JPG


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
TBHS-19.JPG


TBHS-20.JPG

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

TBHS-21.JPG


  • Select the edges at the border of the upper face (holding CTRL ).
TBHS-23.JPG


  • Add a PartDesign Chamfer.png Chamfer of 1mm. This one is only aesthetic.
TBHS-22.JPG


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).
TBHS-24.JPG


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

Inspiration

The above model make a good starting point to use FreeCAD, but as a toothbrush head stand it have its flaws : due to the print orientation and small surface the sticks are prone to break.

Inspired by the variety of solutions other people came up with, we will make this second version which will be much better.

TBHS-v2.jpg


Don't worry it is often needed to go through several revision for an idea (e.g. : once the prototype on the picture was used, we added more space between the heads so that they should not touch).

In this second part you will also learn to use more tools, like the powerful Linear repetition.

Second idea : a band

  • Create a new document and select the Workbench PartDesign.png Part Design workbench.

Create a sketch

  • Create a Sketcher NewSketch.png New sketch, on the XY plan.
TBHS-1.JPG


  • Draw a Sketcher CreateSlot.png Slot
    • Click to place the first center
    • Move to define the length and radius
    • Click to set the second center.
TBHS2-1.JPG


You now have a floating slot of unspecified dimensions.

  • Click on one of the horizontal line of the slot
  • Click on Sketcher ConstrainDistance.png Distance
  • A dialog prompts you to set a dimension. Enter 75mm, click OK.
    • that's for a 3 head stand, count 25mm for each, if you want more
TBHS2-2.JPG


  • Click on one point of the horizontal line
  • Click on one point of the other horizontal line
  • Click on Sketcher ConstrainDistance.png Distance
  • A dialog prompts you to set a dimension. Enter 29mm, click OK.
TBHS2-3.JPG


  • Draw a Sketcher CreateSlot.png Slot around the first slot.
TBHS2-4.JPG


  • Make the centers of the second slot coincident with the centers of the first slot with Sketcher ConstrainCoincident.png Coincident.
TBHS2-5.JPG


  • Click on one point of the horizontal line of the first slot
  • Click on one point of the nearest horizontal line of the second slot
  • Click on Sketcher ConstrainDistance.png Distance
  • A dialog prompts you to set a dimension. Enter 3mm, click OK.
TBHS2-6.JPG


  • To make the sketch fully constrained
    • Click on the lower left point of the second slot
    • Click on the origin of the XY plan
    • Click on Sketcher ConstrainCoincident.png Coincident
TBHS2-7.JPG


  • To leave the sketch, click either on the "Close" button on the left, or the Sketcher LeaveSketch.png icon in the toolbar, or press ESC.
TBHS2-8.JPG

Create a pad

  • Click on View-axometric.png Axonometric among the standard views, to better see what will happen.
  • Click on PartDesign Pad.png Pad.
  • Enter 30mm and click OK.
TBHS2-9.JPG


Create a sketch on it

  • Select the upper face
TBHS2-10.JPG


  • Create a Sketcher NewSketch.png New sketch. As a face was selected it will not ask you to choose a plane.
TBHS2-11.JPG


  • Draw an Sketcher CreateHexagon.png Hexagon
    • Click to place the center
    • Move to define the radius
    • Click to set
TBHS2-12.JPG


  • Click on an edge of the hexagon
  • Click on Constraint Horizontal.png Horizontal
TBHS2-13.JPG


  • Click on the center of the hexagon
  • Click on the horizontal line of the XY plane
  • Click on Sketcher ConstrainDistance.png Distance
  • A dialog prompts you to set a dimension. Enter 15mm, click OK.
TBHS2-14.JPG


  • Click on the center of the hexagon
  • Click on the vertical of the XY plane
  • Click on Sketcher ConstrainDistance.png Distance
  • A dialog prompts you to set a dimension. Enter 10mm, click OK.
TBHS2-15.JPG


  • Click on the blue circle of the hexagon
  • Click on Sketcher ConstrainRadius.png Radius
  • A dialog prompts you to set a dimension. Enter 8mm, click OK.
TBHS2-16.JPG


  • To leave the sketch, click either on the "Close" button on the left, or the Sketcher LeaveSketch.png icon in the toolbar, or press ESC.
TBHS2-17.JPG

Create a hole

  • Click on View-axometric.png Axonometric among the standard views, to better see what will happen.
  • Click on PartDesign Pocket.png Pocket.
  • Select to the first in the dropdown menu and click OK.
TBHS2-18.JPG


Linear repetition

  • In the Combo View on the left, select the tree view instead of the contextual task menu, click on the pocket feature.
  • Click on PartDesign LinearPattern.png LinearPattern.
  • Set the length at 55mm and occurencies at 3, then click OK.
TBHS2-19.JPG

Create a sketch on it

  • Select the inner face
TBHS2-20.JPG


  • Create a Sketcher NewSketch.png New sketch. As a face was selected it will not ask you to choose a plane.
TBHS2-21.JPG


  • Click on Sketcher Circle.png Circle, click to place the center, move the pointer and click to define the radius.
TBHS2-22.JPG


  • Click on the center of the circle
  • Click on the horizontal line of the XY plane
  • Click on Sketcher ConstrainDistance.png Distance
  • A dialog prompts you to set a dimension. Enter 15mm, click OK.
TBHS2-23.JPG


  • Click on the center of the circle
  • Click on the vertical of the XY plane
  • Click on Sketcher ConstrainDistance.png Distance
  • A dialog prompts you to set a dimension. Enter 10mm, click OK.
TBHS2-24.JPG


  • Click on the circle
  • Click on Sketcher ConstrainRadius.png Radius
  • A dialog prompts you to set a dimension. Enter 3.5mm, click OK.
TBHS2-25.JPG


  • To leave the sketch, click either on the "Close" button on the left, or the Sketcher LeaveSketch.png icon in the toolbar, or press ESC.
TBHS2-26.JPG


Create a pad

  • Click on View-axometric.png Axonometric among the standard views, to better see what will happen.
  • Click on PartDesign Pad.png Pad.
  • Enter 4mm and click OK.
TBHS2-27.JPG

Linear repetition

  • In the Combo View on the left, select the tree view instead of the contextual task menu, click on the pad feature.
  • Click on PartDesign LinearPattern.png LinearPattern.
  • Set the length at 55mm and occurencies at 3, then click OK.
TBHS2-28.JPG


Draft

  • Select the side of each round pads
TBHS2-29.JPG


  • Click on PartDesign Draft.png Draft.
  • Set the draft angle at 40°.
  • Click on "Neutral plane" and select the face on which the sketch is drawn.
  • Tick "Invert the draft direction".
TBHS2-30.JPG


We could have used a chamfer to do something similar, but the draft is more appropriate in this case.

Chamfer = left / Draft = right

TBHS2-30-chamfer.JPGTBHS2-30-draft.JPG


Finitions

  • Holding CTRL select the bottom and top faces.

TBHS2-31-bottom.JPGTBHS2-31-top.JPG

    • Add a PartDesign Chamfer.png Chamfer of 0,5mm.
TBHS2-31.JPG


Perfect !

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).
TBHS2-32.JPG


  • Now you can select "Export..." from the File menu at the top left, and select the file format .STL.
  • Print it instead of the first version or to replace it if it eventually broke ;-)