Saturday, July 31, 2021

Weekend Shop Update on the 1 by 1 - part 3

"When we last left the story..."  I prepared a machining fixture, temporarily mounted the two chunks of metal that will become the side plates and said that tool paths were the next big step.   

As I started working on the tool paths, I saw an area that concerned me.  I planned to cut the part by waterline machining, which is parallel paths around the part as if the part is surrounded by water which is lowered a little bit at a time.  If the part is a simple rectangular or square box, this is simple enough to do by hand.  You just give the program the coordinates of start and stop points and tell it to go from one to the other, lowering the cutter every pass around it.  In a part with complex surfaces like this one, it either becomes a very involved program with dozens or hundreds of points you have to find, or you use Computer Aided Manufacturing (CAM) software, which is what I did. 

The program I'm using is an old version of DeskProto, version 5. I bought this software about a decade ago, and while it has been updated several times, they appear to be offering what I bought as a free version now, and you pay to add capabilities in the SW.  I need to look at the free version and see if it's better than what I have.  I have to arm wrestle DeskProto to get it to do what I want; the problem is even when I do, I don't get exactly what I want.  This is a screen capture showing the tool paths before I save them to a file.  The green lines are what are called rapids, or rapid movements; G0 or G00 in Gcode; these are as fast as your machine can move.  The red lines are the regular movements with a controlled feed rate.

I end up editing the tool paths in a text editor to remove those loops around the raised center area; that top surface is Z=0 and that area is already flat.  Some of those paths would cut off my mounting bolts if I didn't do this.. Then I check it in GWizard Editor from to ensure it's cutting right. There still appears to be wasted motions that I'd like it to not make, but since I'm not trying to save every second of machine time, I won't try to edit them out.

This made me concentrate on that little triangular area in the lower right.  That's a large corner that's getting cut away, and what the image doesn't show is that the waterline paths will cut a slot in the aluminum there.  Eventually an inch deep and the 1/2" width of the cutter I'm using.  That concerned me because the cooling system I'm using, a misting coolant called a FogBuster, isn't going to get into a deep slot and blow the chips out like flood cooling will.  I decided to cut away that corner manually.  To do that, I had to figure out where to start and stop along that angular path.  Enter the design program again.

The only thing here that wasn't done by eye and saying "that looks close enough" was to draw the circles the size of the cutting tool (0.500") and pick places to put them.  The reason points 2 and 3 are farther off the edge than 1 and 2 is that I tested the points I had and the cutter didn't go past the edge of the blank.  I drew the rectangle wrong, so I moved 2 and 3 further along the angled path.  Then I wrote a GCode file that moves the cutter in numerical order, 1 to 4 and back to 1 and does that loop over and over.  That will cut away most of that big piece of waste, the only part of the blank to cut away. 

It didn't take long to notice that the cuts didn't seem to be as deep as the Mach 3 display (DRO) was saying as it was cutting.  When the file was done, instead of being all the way through the 1" thick piece, it was cut about a half inch deep. The cutter had driven the rest of the way up into the collet. I thought I had tightened that as tight as always. Oh, well...

I repositioned the cutter (a 1/2" carbide, 4-flute end mill), tightened very tightly and started the cut again. This time, it cut farther down, but still left a sizable ledge on the work - maybe .050 thick. I trimmed that back but every time I cut another pass, it didn't seem to cut any more of the edge away.  

Since the cut had pretty much achieved its purpose of trimming away most of that corner, I said it was close enough to done and decided to do the actual cut. I re-zeroed the cutter in the collet yet again and loaded the big Gcode file.  This file also left a thick ledge again.  You can see it in the red highlighted area, especially on the left.  That area on the right that looks thin with an irregular edge was from the cut to remove the metal in that area.

At this point, I took the carbide cutter out and replaced it with one of my older High Speed Steel (HSS) cutters that I had used several times before.  I suspected that the first cutter might be too small in diameter and that's why the collet couldn't grab it securely enough.  It's a cutter I got from some dood's table at Cabin Fever in '15, so maybe it was surplus because it was imperfect?  My mistake in retrospect was that I never stopped to analyze the problem and didn't really ask, "why is this a problem now and never has been before?"

I did the same exact file with the HSS cutter, spent about 10 minutes cutting air before it got to the bottom and it also left part of bottom too thick. By this time, it was late enough to shut down in the shop and I said I'd look closer at the cutter and collet today.

The cutter diameter was fine. The carbide cutter measured 0.4995 to my manual micrometer while the HSS cutter measured 0.4985. The diameter clearly wasn't the issue, so I cleaned out the collet with a paper "shop towel" (the blue paper kind) and some mineral spirits.  I don't know how it got oil in there, and I didn't see anything on the paper towel, but I put the carbide cutter back in the collet and did the last couple of passes around the side plate (I edited the file to remove everything above cutting to -0.950). This time, it left a thinner margin on the very left side of the blank, but it still had a visibly thicker area.  I re-checked the Z-axis and the cutter hadn't moved, so that meant the work must have moved due to the cutting forces. I lowered the last cut from the value the CAM set (-1.001) down to -1.004 and ran it again, this time resulting in a proper looking side plate.   I think the reason that previous try left some material on the left side is I inadvertently didn't position a backing plate under the left edge.

The end result of the trials.  There's a little metal around the bottom edge - or there appears to be some.  I think a little deburring will take care of that. On the table like this, there aren't many dimensions I can check but they all check to within about .002"with a tolerance of .005".  There's lots of adventures ahead with these two pieces; for starters I need to trim off the corresponding on the other side plate (visible at the right edge of the picture) and then do the big file of cuts on it.  That's just barely getting started.


  1. That corner makes me think "bandsaw".

    1. Bandsaw with a fixture to hold it in place at that angle so it can be held in the vise on the 4x6.

      Milling the corner off takes a couple of minutes, and I used the mill mostly to maintain the zero position on the plate they're mounted to rather than take them off an re-zero them. These two plates need to match each other precisely.

      The next operations are going to be clamping them to each other to drill and tap the five holes that will hold them together. Then there are very large cavities to mill out on both sides.

  2. Why would you bother to switch to G0/rapid mode when most of your moves are G1/linear or G2/G3 circular? I've done alot of CNC programming but not in a machining context. Seems to me that the G0s would just introduce unwanted vibration prior to cutting.

    1. Good point: I don't use G0. I don't think I really ever use it. That's the way the CAM program writes it. Part of the way I check the file is to go through it in a Gcode editor called GWizard Editor. I do a text editor-type Search and Replace all G0 statements with G1. On parts where the longest move is about 3" it's just not worth the vibration and banging.

    2. Makes sense. As I said, I'm not experienced with machining but I never understood the purpose behind the rapid mode. Always seemed like the each axis not synced up would be a little to unpredictable for my taste.