Tools used

• large (2x3 meters) self-made CNC

Software Used

• Solid Works
• ArtCAM
• Mach3
• Fusion360
• Dog-bone Plug-in for Fusion

1. Group Assignment:
   Test run-out alignment, speeds, feeds, and tool-paths for your machine. Go to group assignment page


2. Introduction:
   
   I will be designing and cutting a table for the tree-house. I based my work from a sketch of table done by Anaig a volunteer in the FabFarm.



Rendered table.



table finished.

3. Specifications
   • Material: Birch plywood
   • Mill bit used: 3.175 diamond shape


4. In order to manufacture the table, I will first be using multiple CAD and CAM software. I will start designing with Solidworks then move to Fusion 360 to create the dog-bones, then with exported .dxf file I will move to ArtCAM and create the CAM files, well lets see all these steps bellow:
   
   
   1. I started by scanning the Anaig's sketches.

   

   Anaig's sketch

   

   Anaig's sketch
   2. In Solidworks I started a sketch and then Went to Tools>>Sketch Tools>>Sketch Picture

      

   3. Next I scaled the picture by:
      1. clicking on the ruler and dragging it to a known dimension
      2. I dragged the tip of the ruler to the limit of the known dimension on the picture
      3. I inserted the dimension of the know dimension of the picture
      4. I confirmed the input.

      

      This procedure insures the picture is with the correct scale and alignment.

      

   4. from there I extruded and repeated the steps above for each part then I created an assembly of the table.

      

   5. After being satisfied with the design I proceeded to create dog-bones in Fusion 360. That is done using a plugin called well guess what? Dog-bone!

      

      The Add-in Dog-bone can be simply placed on Windows in the folder "~/AppData/Roaming/Autodesk/Autodesk Fusion 360/API/AddIns/" under its own directory and it will be started at every startup of fusion.

   6. To apply the dog-bone in a design made in Solidworks I first imported the design to Fusion 360 then copied the solid with ctrl+c

      

   7. Next I created a new design
      1. by clicking in the plus sign
      2. right click the workspace
      3. click paste new

      

   8. That automatically opens a dialog box that I just clicked ok.

      

   9. Last is to use the Dog-bone add-in itself.
      1. click the home icon
      2. chose the view
      3. click on the Dog-bone add-in icon
      4. click on the face selector
      5. click on the face you want to add dog-bones
      6. fill in the dimension of the dog-bone, in my case 3.175mm or 0.125 inches which is the size of the mill bit I am going to use
      7. chose the style of the dog-bone
      8. press ok.

      

   10. The result are several dog-ones created at once. Very practical.

       

       

   11. I need to export a .dxf in Fusion360 in other to create a CAM file in ArtCAM.
       1. Click on the surface
       2. Click on create sketch

       

   12. click finish sketch

       

   13. 1. right click on the sketch
       2. Click on save as DXF

       

   14. Finally chose a name and save and I am ready to move to ArtCAM

       

   15. Open Autodesk ArtCAM and then:
       1. Click New Model
       2. Chose the size of the stock
       3. chose the unit
       4. click ok

       

   16. Next it's importing the previously created vector:
       1. Click Vector
       2. Import
       3. Chose the file
       4. press open

       

   17. The previous steps will show a preview of the import then do:
       1. Confirm unit
       2. chose automatically rejoin vectors
       3. press ok

       

   18. Do the steps above as many times as needed so you import all the vectors you want to create the CAM for.

       

   19. I offset all vectors by 0.1mm to compensate for the imperfections of my CNC. That allows for higher tolerance.

   

   20. Next I like sometimes to organize the vector wasting as little stock as possible. That can be automatically done with the nesting tool:
       1. On the vector menu click nest, this will open a dialog
       2. you can inform here the milling tool to be used, in my case 3.175
       3. also inform the angle increments in witch you will allow the software to rotate the parts, in my case I chose 45 degrees.

       

   21. I like to organize the vectors into layers, in this case I will create an outside layer and an inside layer so when creating the tool-path this will be easier.
       1. With the vectors ungrouped select the vector you want first, in my case I selected the vector to be cut outside
       2. click move vectors to
       3. new layer or to a layer previously created.

       

   22. Here I rename the layers to Outside and inside.

       

   23. In the following steps we are creating the tool-path:
       1. Click on the tool-path in the menu
       2. New 2D Tool-path
       3. Profile

       

   24. Since we already have separated the vector in different layers now this will come handy.
       1. Select inside operation
       2. select inside layer
       3. select the depth, in my case thew stock is 19mm
       4. Under profiling tool click in click to Select, this will open a dialog where you can choose the milling bit to be used.
       5. Chose the tool, in my case I chose a 3.176 diamond mill bit
       6. click select
       7. you can then add the type of ramp to be used, I want to try the smooth one.

       

   25. Next Step is to finalize the tool-path, scrool down to show more options and:
       1. Chose Material thickness, in my case 19mm
       2. Define the Material Z Zero, I like to define it on the top of the stock
       3. Confirm the bottom offset that should be 19mm
       4. click ok
       5. Do the same procedure over and over for each tool-path

       

   26. Now we are saving the tool-path, start by clicking in the blue floppy-disk icon this will open a dialog.
       1. You can the view the tool paths you created calculated earlier:
       2. move the tool-paths to the windows on the right to include them in one file
       3. here you can confirm all files on the right side
       4. Chose the folder location
       5. Chose here the post processor to be used, in my case I choose the Mach3 post processor.
       6. Click on save.

       

   27. One thing I almost forgot is to create holes in the G-code. I do that by placing these circles around where the the tool-path in various parts of the job in oder to later screw and fix the stock on the bed, the advantage is I am sure the tool=path is not going to collide with the fixtures of the stock, in this case the screws.

   

5. Now lets Manufacture it with Mach3 on windows XP :-) with the CNC I build while in the Fabacademy. Although its operational I decided not to document it as a final project but thats another story.
   
   
   1. With Mach3 opened:
      1. Click on File
      2. Then load G-code

      

   2. Chose your g-code file and open it

      

   3. The previous step will load the G-code
      1. G code will be shown on the left window
      2. next I like to click on jog follow this will allow you to visualize where your tool is in relation to the G-code, this way you can safely check and simulate the paths before actually running the code. Use arrows to move within X and Y axis and PgUp and PgDn to move the Z axis
      3. by clicking on Zero X, Y and Z when you are over the place in the stock you want to be 0,0,0 will set the soft 0 to where the tool has been moved.

      

   4. I started the job first securing the stock, for that I have the cnc make holes around the design with the g-code "holes.tap" contained in this zip file.

      Holes being made for the stock to be screwed down into to the sacrificial bed.

   5. Here you can see the screwing of the stock. I like to use a torx screw, the can be reused several times and are always reliable. Thanks for Jarek from FabLab Nomads for the tip.

   

   6. After the holes are made and the stock is secure, the internal holes are cut.

   7. After internal cuts are done then the external cuts are done. the step down is 4mm on all cuts.

   8. I believe the quality of the cuts are quite ok for this birch plywood. The dog-bones are visible and with little finishing the parts are going to be ready for assembly.

      

   9. Here you can see the quality control, a team of four including me is filing the finger joints so they smoothly attach one another.

      

   10. I use here an orbital sander. I started with sandpaper 100 grit and moved to 220 and then 500, after that I spayed some water to lift the fibers and sanded again before applying beeswax mixed with isopropil alcohol .

       

   11. Here I test the assembly, everything fits, I fit and then remove the pieces hammering with a white rubber mallet.

       

   12. Now with all pieces sanded and waxed I fit one to another.

   13. Here you can see the tight tolerances of this finger joint, the reduce even more the gaps I used a mixture of glue and saw dust I generated while sanding the surfaces.

       

   14. Detail of the curves

       

   15. Another detail of the filleted sides. The fillet was done manually with a router tool.

       

   16. And Voile, the final result!