This assigment was divided into group- and indivual tasks:
- Group assigment, test following variables of your machine: (see documentation here: )
- runout
- alignment
- speeds
- feeds
- toolpaths
- Individual assigment:
- make (design+mill+assemble) something big
Learning outcomes
- Demonstrate 2D design development for CNC production
- Describe workflows for CNC production
In this week our task was to design something big. I had vision about the tree which would be cable organizer and holder for VR glasses in my classroom (KTK149).
Some examples from the past Fabacademy years
I got many ideas for my own implementation from the examples mentioned above. For example, I followed idea by Chunwei GE to make replica of Connox Tree Coat Stand in my design. Furthermore, I got ideas of joint from all of previous works and idea for stand from Peetu's work.
In this year we had to design "something big" by using OSB (Oriented Standard Board) as a material (thickness was 11mm)
I started from the same phase than Chunwei Ge. I used "Swedese - Tree Coat Stand" as a source of inspiration. However, because this stand was under "all rights reserved" copyright, I modified it a lot to create original artefact, which is as much as possible unique product. For example, I added and modified branches of the tree and designed different stand for it
Generally, my path to manufactured tree coat stand wasn't straight although I considered that this kind of design would be quite easy to design and manufacture. In this documentation you will see that I ended up into problems when creating tool paths, but finally learnt what was to reason for the difficulties
Editing original image in Gimp
First photo of tree coat stand was turned into black white version by using treshold tool (Colors > Threshold)
Then some parts of the tree rack were fixed by using paintbrush (see the photo). After that image was exported by using ctrl+e shortcut.
Next I opened bitmap image into Inskcape and used trace bitmap -tool (shortcut shift + alt + b) to create vector version of the three rack.
Tool did create new (vector) version of the three and after that bitmap version was deleted and vector version was saved to be used later on in the Fusion 360
Inserting SVG file into sketch
Adding SVG file into Fusion360 is easy task:
Settings for inserting SVG
Next it was possible to change orientation of the sketch of tree (it wasn't anymore svg) and scale it. I did scale it to 20x compared to import result
I had to make some changes to original designs:
In this phase I did modify top branch by deleting a part and fixing the rest, because it would be obstacle for joints
In this phase I did copy top branch to the left side of the trunk and then it was mirrored by using construction line in the middle of the tree as mirror line
In this phase I did create new trunk for the tree.
In this phase I did design platform to tree.
Last thing was to design slots to both tree trunks. The rack is designed so that two pieces will stand up in 90 degree angle attached into each other
Slot design was started by sketching vertical slot so, that lenght of the slot would half of the total height of the construction line in the middle of the tree (not visible anymore in this picture, see construction line e.g. in the phases C and D)
Workflow was as it follows:
Unfortunately, approach to use SVG as a starting point wasn't appropriate way to design object for computer controlled machining. Pretty soon I noticed that I can't configure manufacture settings in the Fusion 360 without different kinds of issues and warnings.
I was overwhelmed, because I thought that my design approach was pretty simple: I didn't have complicated slots, joints etc. only two pieces and two joints. So I error in generating passes was surprise. (NOTICE: manufacture settings are described just later on, this image is place here for illustrative purposes)
In order to continue, I did raise issue in Gitlab to get help from local instructor "eikka" with the problem. I saw him in FabLab face-to-face where he explained that my approach was "doomed", because SVGs have pretty often too detailed information and it's difficult to prepare for manufacturing in the fusion.
Because my design was simple, Eikka suggested that I would re-design it from the scratch. However, I decided to use my existing design as starting point - I just sketched new tree on top of the failed design by using normal sketching tools (mostly I used fit point spline tool for sketching new trees). However, I repeated phases above while creating slots, because those are so strict part of the tree instead of just copying those by sketching new sketch on top of those.
Picture below shows surface of the three, which were too much for Fusion360 manufacture settings
This picture (below) reveals radical change in the surface details after new design of the tree. I understand now why Fusion 360 manufacture configuration ended up into errors
If you have png/jpg image that you would like to use as basis for your design, don't use this "insert SVG" approach in the context where you are going to use 2D milling. Instead, it's suitable for 3D printing and similar purposes.
You can just import JPG or PNG directly to fusion and draw sketch on top of that. OR if you have already converted bitmap image into SVG then I recommend that you draw your sketch as a new sketch onto top of the inserted SVG.
Instead, if you have original vector graphics file (not converted from bitmap image), you can use that "insert svg" approach for 2D milling also, because then lines are "smooth"
I changed the mode to CAM (manufacture) to create tool paths for the CNC machine operation. First I chose Setup> New setup. I selected Orientation> X and Y axes, Origin> Model box point. I selected the lower left corner as origin.
Then I started to make toolpaths for cutting. I selected 2D> 2D contour, because I didn't have any pockets and other complicated designs. In Geometry section, I selected all the lines which I wanted to cut on the bottom surface.
In Tool section, I chose FabLab tool library and added 8mm flat bit
I marked Tabs to add tabs on the edges of pieces to avoid the pieces moving or small pieces flying away. It takes some effort to remove tabs. Considering both enough strength to keep object staying and less effort to remove them after contouring, I set tab width 8mm, height 2mm and distance 64mm
In Height section, I chose Model top as top height, and selected model bottom as bottom height. I checked the bottom height is -11mm.
In Passes section, I selected Multiple Depth which the bit creates the depth not at once but goes multiple times till it reaches the depth. I selected 3 mm as maximum step-down and marked Use even steps. So the machine calculates how deep the bit cut out depending on material thickness and maximum depth. I also removed the mark on Stock to leave which leaves some extra material to finishing or sanding. I wanted to cut all the material up to the design so I removed the mark.
In Linking section, I removed the marks on Leads & Transitions which means the bit starts milling on the starting point which is defined in the design without any extra cut before or after. It is useful for cutting metal. Metal is hard so the bit cannot cut in the virtical way, but it cuts in horizontal way. The bit comes from outside of the metal stock (Lead-in) and mills metal in horizontal way. But I used soft material, wood, I don't needed lead-in and lead-out, so I removed these marks.
Finally, I went Action > Simulation to see tool paths
In order to get tools paths as NC code, I added FabLabNC postprocessor to Fusion 360 CAM (for detailed instructions, navigate here).
Workflow for getting NC toolpaths:
NC code ready for machining
I used Rensi E2-1234 CNC router. Eino Antikainen, Fab Academy 2017 alumni, showed me how to operate the CNC machine and was present during the machining.
OSB board was fixed into machining board by using six screws (all corners and center edges of the OBS board)
First, main power was switched on from the control cabinet and Rensi was started by pressing green power button. Yet, control computer was also started and NC Studio program was opened, which is used to control the NC Router
Next, I did pick up milling bit to be attached into machine. (8mm flat bit). To be able to change bit, rensi machining arm was moved to it's mechanical origins. To do this, NcStudio awas used to set the machine Back to Mechanical Origin in All axes. After this the position of the armn was moved closer to edge of bed from the NcStudio.
In order to replace milling bit: 1) I did loose two screws which control the position of the sawdust removal equipment and slowly lowered tube and other parts to the table: 2) then I used two wrenches to loosen the nut and carefully removed holder nut with milling bit (don't allow it to drop to the table) [in the image milling bit is not installed]
Next I set the 8mm flat bit on the bit holder nut and attached it to the machine. Check the bit diameter and use correct holder. Note that diameter of head and bottom are different. Holder diameter need to fit with diameter of bottom of the tool. When you attach the bit on the holder, length of the bit out from the holder should be longer than cutting depth.
In this phase, I did clear existing data from the software (right click > clear). Then I opened the file (File > Open and Load). I clicked simulation to see how it will be machined
Then I did define origin points for X and Y axis. Rensi router has two methods for moving the router: 1) move router with XYZ arrows on the screen of the NcStudio. (if you press ctrl at the same time, router moves faster). When the appropriate X and Y axis positions are found, click X and Y origins from the software; 2) Hand wheel (separate device), which needs to be enabled from the NcStudio (HW/handwheel, manual section in the software). By using this rotating dial, it’s possible to specify appropriate position for axis and then click X and Y origins from the software.
I used to software arrow to move rensi router to close to the bottom-left corner and then calibrated X and Y axis origins to be in that place.
Z-axis can be calibrated by using sensor “mobile calibrator”. In practice, machine will lower z-axis until bit will touch the sensor. In the practice: I placed the mobile calibrator under the bit and kept holding with a hand. Then I selected Operation> Mobile calibrator. When these steps are done, Rensi will auto-calibrate the Z origin.
Place the mobile calibrator under the bit and keep holding with a hand. Select Operation> Mobile calibrator. Z axis moves lower to the mobile calibrator and software calibrate the Z origin.
I set Feedrate (mm/min) 80% and spindle (r/min) 70% and clicked start in NcStudio
If machine is operated in a wrong way, vibration will cause damages to the CNC machine. So be careful not to operate the machine with too much spindle and Feedrate. If these values are too high, the milling sounds gets higher. Attention should be put on listening to the high pitch sounds and avoiding to operate the machine with too much force.
After the parts were cut, I used knife to remove parts. Because trees were attached to the board with tabs, it required a little bit of force. Afterall, result was bit unfinished. I needed to use file to make joints and surface smoother.
Finally! Ready! Tree is assembled
