5. 3D Scanning and Printing¶

This week focused on the processes involved in 3D scanning and printing. I once again teamed up with Anna, Kerstin and Lars, the other students from HRW FabLab, to characterize our lab’s printers’ capabilities. You can find our group work page right here Based on the things we found out i designed and printed an object that can only be manufactured additively. To finish this week i also used our 3D scanner to compare an object to its scanned and printed counterpart.

Designing a FabLab coin in Fusion¶

The humble FabLab coin was one of the first things i was tasked to design and print when i started working at HRW FabLab in 2021. To this day we give them away to visitors, at conventions and other events. Let me tell you, once you have held one of these in your hands and let it spin a couple of times you start to understand why there once was such a hype around fidget spinners. And the best thing about it? No assembly required.

Here is a quick rundown of how i designed it:

i started by drawing three concentric circles, one for the spinning coin and two for the outer ring

then i went to the top of the circles to draw a kind of thorn shape that is going to be the hinge and indentation that will enable the whole thing to spin
i used concentric fillets on the thorn’s corners and mirrored it to the other side

next i finished the sketch and started an Extrude command where i selected both the inner coin and the outer ring and gave everything a thickness of 5mm

i headed to the CREATE menu and started a Revolve command
little thing about revolve commands: you need to only select one half of the thorn’s profile, otherwise the created body or cut would intersect itself and Fusion really doesn’t like that

so i canceled the command, went back into the sketch and drew a line that splits the thorns in half
i actually had already drawn it when dimensioning the thorn but made it a construction line by mistake

i quickly mirrored it to the other side and went back into the Revolve command
i made sure to select Cut in the Operation dropdown menu and deslected the coin in the Objects to cut window

after that i repeated the revolve with the inner part of the thorn shape and joined it with the coin

a few chamfers and fillets later it was already done

i personalized the coin with our FabLab’s logo but feel free to add whatever you want to the blank sides
you can download my Spinning_Coin.f3d Fusion file in the Download section at the bottom of this page
this kind of angled protrusion in a groove, print-in-place design is incredibly useful and i use it quite frequently
a recent example of this is a travelcase for glasses which i designed as a test for our new 5-headed Prusa XL

also a few weeks ago some of the hinges on our GS Laser Systems lasercutter so i quickly designed and printed some replacements

i wouldn’t necessarily trust these to hold much weight but since the cover is held in place tightly with screws and they only ever need to hold for a few seconds during maintenance i figured it will be fine
then again if they break i can just print more replacements but still keep any safety concerns and risks in mind when attempting stuff like this
you can find both the Travelcase.f3d and the Lasercutter_Hinge.f3d Fusion files in the Download section at the bottom of this page

Designing and printing a chainmail spinning top¶

Michael Bennemann, a student from 2023’s FabAcademy and colleague of mine showed me a really cool test print for metal powderbed fusion 3D printers. A small spinning top where the outer mass that keeps the thing spinning was made out of a kind of NASA chainmail equivalent. Ever since our lab got a TRUMPF TruPrint 1000 metal 3D printer i wanted to try and print such a spinning top. Only barrier (besides the machine not working) was that i had no 3D models of this and had to design them myself. I’ll be honest, designing this in Fusion is not easy so if you know of any design tools that would make quicker work of it, please let me know. Anyways here is my design process:

you are going to need two offset planes that are 3mms from the XY plane and a plane that goes through the Y axis at a 120° angle

on the bottom plane start a sketch and draw a hexagon with a width of 7mm and include lines from the center to the middle of the side lines, these are going to be helpful later when we start creating patterns of the chainmail element

start another sketch on the top most plane and project the hexagon by pressing P and selecting the whole outline with a double click on any of its lines

next start a sketch on the angled plane and connect a both of the hexagons’s points that intersect the plane with an arc, add a tangent line of arbitrary length to both ends

head to the CONSTRUCT menu and create a Plane Along Path
select the arc and drag the plane to its end or simply type 1 in the box labeled Distance

another plane, another sketch… draw a center circle with a diameter of 1mm

start a Sweep command from the CREATE menu and select the circle as a profile, for the path select the arc from before

create a new plane the goes through the “tangent line of arbitrary length” at a 60° angle

this is the part where it can get kind of tricky, project the center point of last sketch’s circle as well as the Z axis into the next sketch and start a spline
it should begin at said center point and end somewhere on the projected Z axis
click on the spline to reveal its handles and select the one from the start, add a horizontal constraint so the spline is properly aligned with the arc from before

while still in the sketch go into the top view and roughly align the spline’s end point with the origin

start a sweep with the circle and the new spline but make sure you set it to output a new body instead of joining it to the existing one

mirror it along the first angled plane and also make sure that it generates a new body

we haven’t created a new plane in quite a while so let’s quickly construct one that is at a 30° angle from the Y axis, thus making it perpendicular to the first angled one

i am getting dizzy writing this but mirror the recently mirrored object along the new plane, again creating a new body

now it is finally time to join them with the combine command and probably create a brand new pasta shape in the process
if you are not quite satisfied with the shape remember that the spline is still adjustable

next start a circular pattern, select the combined body and arrange it 6 times around the Z axis, make sure to select join this time

to add a little more rigidity you can add a circle to the origin and extrude a pillar out of it

after that create an offset plane from the XY plane, in the Extent dropdown select To Object and click on a fitting point like this one

do the same thing for the top and split the body with the new planes

select the excess parts and remove them just as a little cleanup

since i have no idea about the engineering behind building spinning tops i used this image from Gigazine’s article about the ForeverSpin 2.0 as a reference

simply head to the INSERT menu and select Canvas
Fusion will ask you to select an image and the plane or face you want to put it on, i had to adjust its position a little to lign up its center with the origin point

rightclick the reference image in the browser and select Calibrate

your cursor will become a + sign with which you can select two spots on the image and enter a distance between them in order to scale the entire thing

this unfortunately moved the image in a weird way so i had to realign its center with the origin

the chainmail element seems kind of big doesn’t it?
i scaled up the image one more time and added a pillar to the bottom of the element, which is going to be used as a support structure

remember when we created the first sketch and i told you we would use some lines for patterning purposes later down the line?
reenable the first sketch and start a rectangular pattern
select the chainmail element and for the axes select both lines from the sketch
set the distribution type to Spacing and create a symmetrical 9x9 grid with 9mm distance
check the Suppression box and deselect the elements you don’t need for a hexagonal pattern

now that there are so many different bodies with roughly the same name you should consider creating subfolders to keep your browser organized

start a new sketch on the YZ plane
project the bottom of the center support pillar and from there draw a line straight up (i went with a length of 62mm)
at the bottom create a circle that will form the tip of the spinning top
now start a spline that goes from one side of the circle to the top of the line, roughly following the contour of the reference image

start a Revolve command with the face that the center line, circle and spline created
make sure that you create a new body

some of the loops from the moving parts are stuck inside the main body so they wouldn’t be able to move freely

fine tune the spline so there is no connection anymore
combine the main body and the inner circle elements

the last thing to do is remove the unnecessary support pillars
a quick and dirty way is to simply select them and hit the DEL key but i’d suggest using the Remove Face tool instead

and there it is, the spinning top model is done

usually you would now go ahead and right click the body you want to export as a 3D model for slicing and printing purposes but since there are so many elements that are not directly connected we need to right click the entire component and select Save as mesh

my weapon of choice for this print is going to be the Bambu Lab X1 Carbon with a 0.2mm stainless steel nozzle, you can read more about the machine on our group page
since this is going to be more of a torture test for the printer i am really just freestyling the settings in Orca Slicer, a popular fork of Bambu Lab’s Bambu Studio
if you didn’t know, a slicer is a piece of software that takes a 3D model and turns it into code the machine can read and execute

3D Scanning with the Einscan Pro 2X Plus¶

Downloads¶

Spinning_Coin.f3d

Travelcase.f3d

Lasercutter_Hinge.f3d