3D Printer Project: Fabrication #1

The first step in the fabrication of the printer is to create the Aluminum plates that everything mounts to:

The accuracy of these plates determine the precision of the overall system, thus precisely fabricating them is key.  However their size (roughly 20"x20") make them too large to fabricate in my Tormach. I considered alternate fabrication approaches such as plasma cutting, but ruled them out as too imprecise. Instead I chose to purchase a fixture table for my Tormach that allows me to precisely reposition the piece in a larger work envelope:

To use this I had to come up with a process to break a large part down into a series of smaller section cuts and ensure they all line up precisely.   Generally I use Sheetcam for 2D work like this, but I quickly discovered that you cannot currently specify a cutting region within Sheetcam.  So I had to figure out a way to precisely clip sections of the DXF file before loading it into Sheetcam.  Moreover, I had to decide how to align the zero positions of the cutting envelope (red), tooling plate (blue) and the material being cut:

CoreTop.png

I finally determined that I could create a sheet in Solidworks and specify a clipping box based upon exact offsets.  I sized the clipping window to be slightly smaller than the milling envelope of the machine.  Moreover I can control the relative position of the object relative to the clipping window by setting up smart dimensions between the object and the clipping window box.

I also created a reference point slightly outside of the clipping region in the lower left corner.  Since this point defines the lower left corner of the outputted DXF file, this becomes 0,0 in the sheet.  Now as long as I pick a 0,0 point on the tool table and ensure that the offsets to the two alignment holes match the measured offsets on the table I can guarantee that everything lines up correctly:

The raw DXF output looks like this:

Ok this is a great start, but now we have the issue that I don't actually want it to cut out all of these outside edges.  The two "clipped" edges need to be ignored.  Moreover the edges I want to cut do not form enclosed contours, so the interior/exterior function in Sheetcam would not function properly.  I decided to load the DXF file into Draftsight and do a bit of manual editing:

I did a couple of things to the file at this stage:  1) I moved the holes, alignment holes and edges to different layers, and 2) I boxed the outside edges.  By boxing the edges I created closed-loop paths.  The disadvantage of this approach is that it increases the cutting time, since it has to cut twice as much.  However the big advantage is that this allows me to use the path features in Sheetcam and adjust the cut path automatically based upon the tool diameter.  Moreover creating these boxes is quick and easy, since the lines I'm adding do not have to be precise.  Any other approach would have vastly increased my editing time at the benefit of run-time and would have increased the likelihood of errors.  Since the run-time was irrelevant for this prototype, I chose the former approach. 

I then outputted the modified DXF and loaded this into Sheetcam in the lower left quadrant.  Since I head already set the material size to match the cutting envelope of the machine, the 0,0 of the sheet and the table line up without any additional work:

From here creating the tool paths based upon the layers is easy-peasy.  No additional editing is needed:

I plan on trying to duplicate the process using Sprutcam at some point to see if  I can reduce the steps.  Theoretically Sprutcam allows you to define a cutting envelope as part of a larger piece. 

The only think left was to actually run the jobs.  I ran these in the following sequence:

  1. Top Left -  alignment hole & outer edge
  2. Top Right - outer edge
  3. (Flip front to back)
  4. Bottom Left - alignment hole & outer edge
  5. Bottom Right - outer edge
  6. (Rotate 90 degrees)
  7. Middle Left - outer edge
  8. (Flip left to right)
  9. Middle Right - outer edge

There were a number of subtle issues I had to deal with during the milling process itself.  The most significant of these was determining the proper placement for the clamps and the standoffs underneath.  I had some issues with vibrations at a couple of steps due to flex in the thinner joints as you will see in the video.  And I had to stop the process several times to move the standoffs to avoid the cutting path.  I verified that as long as I re-zeroed the machine after any emergency stops the alignment between cuts was maintained.  

Here's a short video I made of machining the top plate.  I'll probably post another one of the back plate in the next couple of days:

Next step is to mill the ways for the rails to rest on and drill the various holes.  This will follow basically the same process of alignment and repositioning to move the plates around on the tooling table.  

 

Posted on January 2, 2015 and filed under 3D Printers, Projects, CNC Machining.