Further Adventures with the Sieg KX3 & KX1

In my early days of CNC I started off by touching off each tool and noting the offset. However, that got tedious rather quickly, especially when I forgot to type in the offset when changing tools.

I now use a master tool and an electronic tool height setter. The master tool (tool 0) is simply a length of silver steel with a rounded end, on the left in this picture:

The sequence is:

• Touch off the master tool on the table and zero Z
• Use the electronic tool height gauge to measure each tool against the master tool and automatically fill the tool table. Measuring each tool is a one button push on the screen
• Touch off the master tool on the fixture or work, depending upon where the zero height reference was set in CAM
• Set X & Y zeros
• Start machining!

Andrew

I like that method Andrew, usually I take the Z offset from the longest tool, but having one dedicated master tool is a good idea. The only problem I can see is a restriction on Z height on my KX1. Are you using Path Pilot they look like Tormach tool holders?

Ian

Andrew, do you touch off the master tool on the table or the height setter? Presumably the latter if the heights of the other tools are measured using the setter? Is your master tool solid or is the tip isolated?

I am indeed using PathPilot and the toolholders are Tormach, although I use them on the Bridgeport as well.

The concept of tool 0 came from a professional CNC book. One advantage is that the master tool is longer than most real tools so less chance of a crash. But of course it's bad if you have limited Z. Tormach now advise using the spindle nose as a reference. In theory that should be "slightly" more accurate as one is removing one variable, the interface between the toolholder and spindle nose. But in practice it's a PITA as the spindle nose is large, you can't see what's going on and it's no good for recessed reference planes. So I've stuck with a master tool.

Andrew

I touch off on the table. The electronic tool height setter is from Tormach and is integrated into the software. So the system knows that the tool setter is 80mm high and takes that into account automatically. The master tool is solid, no electronics involved. I simply ramp down slowly until a fag paper is trapped.

Andrew

My method is old hat but doesn't require special tools or programs, just enter the tool offset in the toolchange line in the program,

**LINK**

Emgee

Thanks guys, one more question: when a job is running is it possible to adjust the tool speed and feed rate or does the job have to stop to re-visit whats programmed.

Mach3 allows you to override feed in 10% steps and speed can also be overridden both while the machine is running using the up and down arrows in the two boxes bottom right

Edited By JasonB on 10/04/2019 19:20:55

Yes, but I've never used the facility. One might do an aircut at slower speed if clearance on clamps, for instance, is tight. But once a program is cutting metal let it get on with it. Unlike manual milling you make a decision as to speeds and feeds and let the program run. And then go and do something else. For CNC milling you need a better understanding of speeds, feeds, widths and depths of cut than for manual milling. Which is why the "all you do is press a button" brigade are wrong.

Andrew

I tend to be a bit wimpish with feeds and often find myself turning the feed up once a cut has started when it's evident that it's too slow.

The adventure continues with this part which will be the bottom mounting flange of the cylinder.

First operation was to run the code which put the four 3mm holes into an oversize piece of 1/4" flat steel bar. I then put an offcut of aluminium into the vice and ran the code again but this time with a 2.5mm drill, the holes were then hand tapped and the two screwed together without removing the aluminium tooling plate from the vice.

With a 6mm dia 3-flute carbide cutter I first ran an adaptive clearing cut around the outside followed but a final contouring cut to finished size. I started off quite tame at 3000rpm and 150mm/min feed but found that could be upped as the flat bar cut a lot better than the steel plate I was cutting the other day.

The next part of the code had the adaptive clearing to form the 4 raised bosses, this again had been programmed as above but found I could go faster and ended up at 3900rpm and 225mm/min feed.

Again Youtube has added some high frequency noise but you can see the first cut around the outside where the DOC varies as I only rough centered the work followed by 3 clips of the top clearing at various stages.

Looking good Jason I will have to admit my ignorance though...adaptive clearing cuts...?

Ron

[This posting has been removed]

That's a pretty good summary. Took me quite a while to realise I was better off running fast with small cutters on the CNC mill rather than trying to hog out with large cutters at slow speed.

In the video the tool seems to spend an inordinate time cutting air. I suspect a climb mill only button has been selected? I normailly use climb milling for a finishing cut but for roughing out I select both, so you get the zig-zag cutting.

Andrew

Thanks for the explanation Barry and also to Andrew for his input.

From posting on another forum I have found out that I had the return movements set the same as the cutting feed which slowed things down quite a lot.

After reading your replys I have looked and found where I can set the tool to cut in normal, climb or both directions and changing to both has again reduced the time according to the simulator. I had just been using climb cutting.

For Ron these are screen shots of the simulator, the blue line represents the axis of the spindle and you can see that the tool steps over 1.5mm for each pass which is what I was doing in the video. The yellow lines ae where the tool returns to the start of a cut so time wasted

This screen shot is with the cutter set to cut both ways so less time not removing metal on the return movements, blue in climb cutting, yellow conventional direction.

Edited By JasonB on 14/04/2019 10:36:45

Thanks guys , interesting stuff.

Ron

Good explanation of adaptive machining thanks Barrie. I am using Vectric Vcarve and don't think they have an adaptive strategy, unless I'm not looking hard enough?

And I too have also come to the conclusion that small cutters and more faster cuts are the best way to tackle CNC milling, less stress on the machine, especially on a little hobby mill. Apart from a fly cutter and edge finder, I very rarely use any cutter over 6mm dia now, there is no need to!

Ian

To finish the sandwich construction of the engine base some form of filling was needed and as I have quite a few off cuts of Corian I decided to use that rather than metal.

The sequence was much the same as the top and bottom plates but I tried out peck drilling for the 3mm holes as they were quite a bit deeper than before, I could have gone faster with the retract speed and not lifted so far out of the work, drill was running at 5000rpm.

I used a chip breaker feed for the larger holes, you can't see it that well on the video but can hear when the drill pauses the feed which if I was drilling steel or Ali would shorten the swarf, dropped down to 1000rpm on the 6mm and 7.8mm holes.

Finally machining the contour where you can see the tool ramp down and then start cutting in 2mm deep passes before it starts to get lost in the swarf which is when I stopped filiming and got the vacuum running. The 3-flute Carbide cutter romped through this at 5000rpm and 350mm/min feed.

It's coming together nicely Jason. Good idea to use Corian as a filler, I don't suppose it matters what its made of, as long as it does the job and looks good when finished.

Had to Google Corian, never used it before, looks like good stuff. Messy though!

Ian

I'm sure you've said somewhere Jason, but what CAM program do you use please?