Toothbrush Head Stand/de

Ein alltägliches Problem
Elektrische Zahnbürsten kommen selten mit einem Ständer für die Köpfe, während Sie in einer Familie oftmals mehrere Köpfe sehen, die mit einem Gerät benutzt werden. Viele Leute, die ein gemeinsames Problem haben, führen zu einer Vielzahl von Lösungen, wie man u.a. auf Thingiverse sieht (200-800 Projekte befassen sich damit). Hier ist die erste Antwort und wie man sie entwirft.

Dieses Tutorial wird Sie durch die notwendigen Schritte führen, um das in der folgenden Abbildung gezeigte Teil mit Hilfe von grundlegenden Werkzeugen aus dem Part Design-Arbeitsbereich zu modellieren (viele der Werkzeuge und Möglichkeiten werden nicht behandelt).



Erste Idee: Eine Platte

 * Auf der Startseite von FreeCAD wählen Sie [[Image:Workbench_PartDesign.png‎‎]] Part Design, oder erstellen Sie ein neues Dokument und wählen Sie den Part Design-Arbeitsbereich.

Eine Skizze erstellen

 * Klicken Sie auf [[Image:Sketcher_NewSketch.png|32px]] Neue Skizze, entweder aus dem Aufgabenmenü auf der linken Seite, der Werkzeugleiste oben oder dem PartDesign-Menü oben.

Ein Dialog fragt Sie nach der Skizzenorientierug und dem Offset.


 * Wir wählen die XY-Ebene wie in der obigen Abbildung gezeigt (diese Orientierung entspricht der üblichen Ebene der meisten 3D-Drucker) und drücken dann OK.



Sie sehen nun die XY-Ebene von oben und haben Zugriff auf die Zeichenwerkzeuge.


 * Click on Sketcher_CreateRectangle.png Rectangle.
 * Click to place a first point.
 * Click to 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, click to place the center, move the pointer and click to define the radius.
 * Draw 4 circles on the pad (of any size)
 * 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 :-)

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.



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 [[Image:Workbench_PartDesign.png‎‎]] Part Design workbench.

Create a sketch

 * Create a [[Image:Sketcher_NewSketch.png|32px]] New sketch, on the XY plan.


 * Draw a [[Image:Sketcher_CreateSlot.png|32px]] Slot
 * Click to place the first center
 * Move to define the length and radius
 * Click to set the second center.

You now have a floating slot of unspecified dimensions.


 * Click on one of the horizontal line of the slot
 * Click on Constraint_Length.png Length
 * 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


 * Click on one point of the horizontal line
 * Click on one point of the other horizontal line
 * Click on Constraint_Length.png Length
 * A dialog prompts you to set a dimension. Enter 29mm, click OK.


 * Draw a [[Image:Sketcher_CreateSlot.png|32px]] Slot around the first slot.


 * Make the centers of the second slot coincident with the centers of the first slot with Constraint_PointOnPoint.png Coincident.


 * 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 Constraint_Length.png Length
 * A dialog prompts you to set a dimension. Enter 3mm, click OK.


 * 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 Constraint_PointOnPoint.png Coincident


 * 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 30mm and click OK.

Create a sketch on it

 * Select the upper face


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


 * Draw an [[Image:Sketcher_CreateHexagon.png|32px]] Hexagon
 * Click to place the center
 * Move to define the radius
 * Click to set


 * Click on an edge of the hexagon
 * Click on [[Image:Constraint_Horizontal.png|32px]] Horizontal


 * Click on the center of the hexagon
 * Click on the horizontal line of the XY plane
 * Click on Constraint_Length.png Length
 * A dialog prompts you to set a dimension. Enter 15mm, click OK.


 * Click on the center of the hexagon
 * Click on the vertical of the XY plane
 * Click on Constraint_Length.png Length
 * A dialog prompts you to set a dimension. Enter 10mm, click OK.


 * Click on the blue circle of the hexagon
 * Click on Constraint_Radius.png Radius
 * A dialog prompts you to set a dimension. Enter 8mm, click OK.


 * 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 hole

 * Click on [[Image:View-axometric.png|32px]] 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.

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.

Create a sketch on it

 * Select the inner face


 * Create a [[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, click to place the center, move the pointer and click to define the radius.


 * Click on the center of the circle
 * Click on the horizontal line of the XY plane
 * Click on Constraint_Length.png Length
 * A dialog prompts you to set a dimension. Enter 15mm, click OK.


 * Click on the center of the circle
 * Click on the vertical of the XY plane
 * Click on Constraint_Length.png Length
 * A dialog prompts you to set a dimension. Enter 10mm, click OK.


 * Click on the circle
 * Click on Constraint_Radius.png Radius
 * A dialog prompts you to set a dimension. Enter 3.5mm, click OK.


 * 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 4mm and click OK.

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.

Draft

 * Select the side of each round pads


 * 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".

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

Chamfer = left / Draft = right



Finitions

 * Holding select the bottom and top faces.


 * Add a PartDesign_Chamfer.png Chamfer of 0,5mm.

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).




 * 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 ;-)