3. Computer controlled cutting¶

This week i cut out a neat little sticker on one of our vinyl cutters and created a parametric construction kit that is going to come in handy in a future assignment, so stay tuned for that!
The construction kit was modeled entirely in Autodesk Fusion, to which i gave a brief introduction in last week’s assignment about Computer-aided design.
I also teamed up with Anna, Kerstin and Lars, the other students from HRW FabLab, to characterize our two lasercutters’ focus, power, speed, rate, kerf, joint clearance and types.
You can find this week’s group work page right here

Vinyl cutting a sticker¶

I started off by quickly designing this 10cm long ruler in Inkscape which pretty much only consists of rectangles and text/numbers

if you are following the process make sure that you set the stroke style of your design’s paths to Hairline so the vinyl cut software recognizes them properly
save your design as an .svg file and open it in your vinyl cutter’s software (in my case Cricut Design Space)

after opening a new project and uploading the .svg file i had to select all elements of my design and click on Flatten, otherwise the software would change their position for some reason

next i clicked on Make, connected the machine via USB, checked if everything was at the correct place and set up the cutting parameters for Adhesive Foil Vinyl with Pressure set to more to get a more reliable cut

i put my vinyl material on the sticky mat and put it in the machine

the only thing left to do was to press the flashing buttons and watch the cutter do its magic
after it had ejected the mat i cut the small section with my design out of the vinyl sheet and began removing the inner parts of the lines and numbers

i then stuck it face down onto some transfer tape

peeling off the outline and backside of the adhesive foil proved to be a little difficult because the insides of 4,6,8 and 9 did not want to stay in place
with a little patience and time i eventually got it right and all the relevant pieces stuck to the transfer tape

last i placed it all on the first page of my notebook and peeled off the transfer tape making sure that the numbers were complete

you can find the Ruler_Sticker.svg file in the Download section at the bottom of this page

Parametric modeling in Fusion¶

the first sketches for this week’s lasercut parts started on paper

my goal was to create a customizable system that can hold cups/bowls of varying sizes and be assembled in a grid pattern regardless of the elements’ sizes
the system’s design should be adjustable via parameters such as material thickness, hole diameter for cups or bowls and the lasercutter’s kerf
Fusion is the perfect software for something like this, feel free to follow along with this introduction to parametric design
in last week’s assignment i went over how to set up the software, start a basic sketch and showed what you can do with just one simple parameter
this week is going to be a little more complex than that but we’re still only scratching the surface of Fusion’s capabilities
i’m not going to show everything the Parameters function has to offer so if you want to learn more about the topic you can find Autodesk’s Parameters reference right here
let’s start by creating a simple sketch consisting of a square with a circle in the center and a small rectangle in the top left corner

as the blue lines indicate, the sketch is not yet fully defined meaning you can still drag the corners and points of the individual elements around
i selected two sides of the rectangle and marked them with an equal constraint in order to always have a perfect square

next i pressed D and clicked on one of the sqaure’s lines to give it a size
here i entered wSquare = 60mm which automatically creates a model parameter that i can (and will) change later on

i did the same thing for the circle, entering dCircle = 30mm

the last blue object in this sketch is the rectangle floating in the top left corner
i set the horizontal lines to wJoint = 20mm and the vertical ones to wMaterial but the rectangle can still be moved freely because it is not yet fully constrained

to change that all i needed to do was give it a fixed position by dimensioning its offset from a known fully constrained object such as the square
in order to do that simply press D and click on both the fully constrained object and the line you want to position
i set the top offset to wMaterial/2 (you can use mathematical equations in these boxes) and the side offset to wMaterial

now that everything is fully constrained, the previously blue lines have turned white and we can open up the parameters menu by heading to Modify -> Change Parameters

the following window should pop up

i just now realized that it could be helpful to have those parameters be User Parameters insted of Model Parameters so i did some restructuring
i basically had to delete the whole sketch, add User Parameters by clicking the little plus icon at the top of the parameters menu and redo the sketch with the new parameters
Same-same, but different…

to make the sketch robust to all possible changes, we’re going to need to do some Maths
or just copy what i did and live in blissful ignorance, your choice…

jointSpacing should be pretty self explanatory, it adds a margin to the sides of the joint’s width (which is four times the material thickness)
additionalJoints calculates how many additional joints besides the starting one will fit into the square
safetyMargin makes sure that the circle’s outline does not intersect with the joint’s slot
this all may look like witchcraft but trust me it is not, all it does is adjust the sketch automatically when changing the material thickness, the circle’s diameter or the kerf
the latter of which is the reason for all those .95mm values because i went back into the sketch and added or subtracted half of the lasercutter’s kerf from the relevant dimensions
let’s do a quick sanity check to see if everything works as expected

okay, that looks good to me, time to finish the sketch and go 3D
press E to start an extrude command, select both the inside of the square and the rectangle and set the distance to wMaterial

the sketch should have automatically been hidden after this command but we need to do another extrusion based on the joint slot so go ahead and click on the eye icon next to it

start another extrude command, select the joint slot, set the extent type to To Object and select the top side of the body to make a cutout that adjusts with the plate’s thickness
feel free to hide the sketch now and start a Rectangular Pattern command
for Object type select Features and select the last extrusion from the timeline

next click on the select box next to Axes and select an axis that is parallel to the slot

unfortunately i seem to have modeled into the negative direction according to Fusion’s coordinates but oh well…
all this means is that i have to enter negative values for the spacing distance
make sure to set Distribution to Spacing, the Quantity for Axis 1 to additionalJoints + 2 and the Distance for Axis 1 to -jointSpacing
also set the second Axis’ Quantity to 1 and you should be looking at something like This

start a Mirror command, set the Object Type to Features, select the rectangular pattern as well as the previous extrusion from the timeline and set the Mirror Plane accordingly

time to revisit the Parameters menu and change some stuff to see the magic happen

onto the next piece of the puzzle - connectable snap fit legs
i want all the plates to stand on their own feet with the ability to link up with adjacent ones
hide the body for now (mind the context) and create a new sketch
i added a new parameter defining the leg’s height and drew a center rectangle with the dimensions (hLeg + kerf / 2) x (wJoint + kerf / 2)
starting from the top left i created a smaller rectangle with half of the material thickness as its width and constrained it to reach to the center point this will later be a slot to make sure the snap fit elements have enough room to bend
those snap fit elements need some kind of feature that holds them in place so i drew a semi-circle with a radius of wMaterial / 2 starting from the top left corner
next i added a feature in the shape of a thick L that extends by wMaterial to the left of the bottom left corner
its top is set to be wMaterial from the semi-circle’s bottom point
i left a gap of wMaterial / 2 between the flexible pin and the L shape
last i created a center line from top to bottom and opened the Mirror command to bring all of those features to the other side

one symmetrical extrusion command with a width of wMaterial later i was left with the first snap fit leg

i think i am going to use an additional piece with a lap joint to create a + shape and give more stability to the legs
while i am at it am going to create a wider lap joint piece to connect the legs of two adjacent elements
i went back into the sketch to add a rectangular slot from the middle to the bottom with a width of wMaterial / 2
the extrusion does not automatically adjust for newly added profiles if they are in a previously selected region so i had to go back into the extrusion command and deselect those manually

after that i added a 1mm chamfer to the bottom edges of the new slot to have an easier time during assembly later on

at this point i realized that the slot does not have to be that long, it should rather end in the middle between the element’s center and bottom, so i went back again to change its height to hLeg / 4 + kerf / 2
this of course broke the extrusion command again which in turn broke the chamfer command…

for the connection/stability parts i once again started by drawing a rectangle with (hLeg + kerf / 2) x (wJoint + kerf / 2) as its size
i actually only need half of the height but in my head it makes more sense to have the overall height as a reference
i started drawing another rectangle from the center and pulled it down, making its dimensions (hLeg / 4 + kerf / 2) x (wMaterial + kerf / 2)
next i extended the sketch to cover both the single stability element as well as the connection piece in one drawing
the slot rectangle simply had to be copied to the side with a distance of wMaterial - kerf / 2 and so did the space to the side of the slot

after that i extruded both parts as new bodies

as a finishing touch i added some more chamfers and gave the whole design a wooden appearance

the next thing to do would be to prepare .dxf files for the lasercutter
Fusion is kind of weird when it comes to exporting .dxf files, you can rightclick a sketch and select Export DXF but this would also export all of your construction lines that you definitely do not want to have in your files for lasercutting
to circumvent this i installed a neat little plugin called DXF for Laser by Ross Korsky, which you can find here
simply login with your Fusion account, install the plugin and restart Fusion
the Create dropdown now has a new command at the bottom

this tool lets you select the face of the object you want to export with a built in kerf parameter
in this case, since kerf already is a parameter within all the calculations and sketches i set it to 0

click ok, give the file a name and save it to your location of choice
check the Download section at the bottom of this page to find the parametric_construction_kit.f3d file

Laser cutting¶

i imported some of the files into RDWorks, our Laser’s Software and arranged them so they would not leave as much unused material

after that i set up the cutting parameters and made sure to include two different colors with the same settings
basically you want to do the inner cuts (red) first to prevent the part from moving

for some reason the button to upload your files to the machine is labeled Download in the lower righthand corner, so after figuring that out i clicked it and started setting up the lasercutter
i placed some 6mm poplar wood on the bed and moved the lasercutter’s head over it
next i let the machine run an auto focus command

after selecting my file from the file menu i looked for a fitting spot and set the origin point with a small gap to the side walls

the last things to do were to close the lasercutter, make sure the laser is activated, hit the reset button and press start

when starting any kind of lasercutting job it is vitally important to check if the air filtration system is working
equally important is to never leave the machine when a job is running, the material can catch on fire quite easily, so please be careful and always monitor what your machine is doing
when the job was finished i let the filtration system do its thing for another minute or two and then went to retrieve my first tests
while the pieces looked good enough, the joints weren’t quite there yet

the snap fit joint …snapped immediately and the lap joint was too loose, so back to the drawingboard it goes

the snap(-ping) joint’s problems might actually come from the wood’s grain direction, so i am going to simply turn the part by 90° and see if that fixes things

nope…
back in Fusion i gave the snap joint’s pins a little more length and put a chamfer in their bottom corners
in addition to that i changed the pin’s top from a semi-circle to a more conical shape and gave them a few fillets