Friday, February 26, 2016

Moving Along

While I'm waiting from my 6 day old concrete to cure, I'm pushing ahead with other projects.  The last (I hope) hardware I need for the antenna project is on order, and I've gone back to machining the parts for my G0704 Project.  Two of the three motor mounts, my X and Y axis mounts, are now complete.
You can't tell the scale, but these are each 2.5" on a side, and the holes in the corners are in the same place on both of them (they match the NEMA23 profile of the motor), drilled for a 10-32 socket head cap screw and counterbored to hold the cap head.  The other features are rather different between them, as you can see. 

Back in November, I posted a short example of getting one of these into CNC, but I didn't use the method outlined there of using a CAM program to automagically create my G-Code files.  I coded these by hand back in January.  It's pretty straightforward (although tedious) to do.  Basically, I got the motor mount drawings into my 3D design program (Rhino3D), the DVD I bought includes them in a standard format that Rhino can read, then got the dimensions for all the features.  This was basically the centers of all the holes to drill.

The first step was to create a G-Code file to drill the holes with a center drill to mark their locations.   G-Code files are plain ASCII, and the syntax is dirt simple.  Here's a sample piece of code.  It goes to two different holes and lowers the center drill, in a drill chuck, down low enough to mark the hole clearly:
G01 X 0.323 Y 0.323 Z 0.0250 F10
G01 X 0.323 Y 0.323 Z -0.1250 F1
G01 X 0.323 Y 0.323 Z 0.0250 F10
G01 X 2.177 Y 0.323  
G01 X 2.177 Y 0.323 Z -0.1250 F10
G01 X 2.177 Y 0.323 Z 0.0250 F10
This is far more than really needed to be written, but it's a text export from a spreadsheet (I use Apache Open Office because it's free and it does everything I've ever asked of Excel).  G01 X xxxx Yxxxx Zxxxx Fxxx  means Go to coordinates X Y and Z of the work at a feed rate of F (in inches per minute).  The first line will drive the cutter to the point (0.323, 0.323, 0.025) at 10 IPM.  All of these assume that the cutter was starting from a safe place, and it's my responsibility to make sure my machine won't cut itself or anything undesired.  Once the cutter is at that point, I lower it to 0.125 below the surface at 1 IPM, then I retract it at 10 IPM and go to the next point.  There's another GoTo command in G-code: G00.  G00 is a rapid GoTo, set as fast as the machine can move.  I could have easily made that third line read
G0 Z0.025
moved the F10 to the next line, and had the same effect while saving some space.  On my machine there isn't much practical difference between "as fast as you can go" and 10 IPM.

Once these holes are marked, I could have used the file to drill the holes to full depth, with breaks to change drill bits, or any degree of fancy I want.  I did those manually, in what's usually called immediate mode.  The machine controller has a command line, where I can enter strings of commands and repeat them with using a loaded file.  I wasn't sure how fast I could drill, so I experimented by hand and drilled the holes slowly, peck drilling "manually", then feeding faster, and finally in one continuous move with no pecking.  

The next step was to create a tool path to cut out the square hole in the middle.  The drawing called out a 1/8" radius, so if I moved a 1/4" cutter in a square with the end points 1/8" in from the edges of the square, it will cut it out with that radius with one tool.  I wrote a program assuming a hole big enough in the center to lower the cutter, the move to the edge, cut the four sides, lower the mill, cut the four sides, and then repeat until the cutter is below the bottom of the piece, cutting a little chunk of aluminum off.
G01 X 1.250 Y 1.250
G01 Z -0.0250 F1
G01 X 1.777 Y 1.250 F10 
G01 X 1.777 Y 1.777  
G01 X 0.717 Y 1.777  
G01 X 0.717 Y 0.717  
G01 X 1.777 Y 0.717  
G01 X 1.777 Y 1.250  
G01 X 1.777 Y 1.250 Z -0.0500 F1
G01 X 1.777 Y 1.777 F10  
In reality, you don't want to keep cutting until you make the last path around the square.  That piece in the middle is going to be held on by a progressively smaller and smaller piece of metal.  Generally speaking, it's going to get yanked out of place and jam up the machine rather than politely fall to the bottom, not affecting anything.  It could do Bad Things.  I stopped the cut on the last side and then took the piece out by hand.  Once it was out of the way, I resumed the cut and cleaned out the last of the metal in the hole. Here's a look at the last cut.  You can see where the bit cuts through the light web of aluminum and leaves air behind it.  This video stops before I stopped the machine to pop out that little cube with the big hole in it.  

I should probably powder coat these.  I'm not sure what color, but the only powders I have now are for fishing lures: white, chartreuse and an orange-red.  None of those seem quite right.


  1. Would it be worth it to plan leaving a small bridge in the metal at four or two cardinal points? Then the piece could be flexed free.

    Kind of like leaving the workpiece attached when using the cut off tool in the lathe to prevent damage when the piece is flung off by the final cut of the cut off tool.

    That would have been a lot of hand cranking on the mill for me. I like your way a lot better.

    Would you have to allow for a thickness change in powder coating, compared to no change if you dye the piece.

    1. When I use the CAM program, I will leave a web of metal in a few places to support the piece I'm cutting off. It's actually a built in feature in the program I use, DeskProto. When I code by hand it's harder to do, but it is the right way. Either wire cutters or a small saw, like a jeweler's saw, makes it an easy job.

      I don't have an answer to the coating thickness issue. Another thought I had was to take everything up to an anodizing place in town and finding out what they'd charge to do it for me. The surface prep isn't good enough right now. Basically, they should be polished to a high shine before anodizing. I'm not ready to take on anodizing as a hobby. At least not yet.

    2. Several years ago I was reading up on home anodizing on Calguns. I decided I did not want to do it at home.

      Could you do a CNC plotted engine turning? And then a dye?