Further Adventures with the Sieg KX3 & KX1

[Andrew JohnstonParticipant @andrewjohnston13878]

Posted by John Haine on 10/04/2019 15:10:05:

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 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

[EmgeeParticipant @emgee]

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

[Ron LadenParticipant @ronladen17547]

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.

[JasonBModerator @jasonb]

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

[Andrew JohnstonParticipant @andrewjohnston13878]

Posted by Ron Laden on 10/04/2019 19:16:11:

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.

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

[John HaineParticipant @johnhaine32865]

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.

[JasonBModerator @jasonb]

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.

Final job was to skim the bottom off, final size will be done after silver soldering the assembly together.

Intention is to have a 20mm block between the bosses so a quick test with an ARC 10-20-40 block to see what the fit is like

Can't get much better than this

[Ron LadenParticipant @ronladen17547]

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

Ron

[Former MemberParticipant @formermember32069]

[This posting has been removed]

[Andrew JohnstonParticipant @andrewjohnston13878]

Posted by Barrie Lever on 14/04/2019 09:38:01:

Modern CNC machining (HSM) seems to be favouring taking lighter cuts on the side of the tool and with very high feed rates. Rather than old manual techniques which I think tended to go for big stepovers.

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

[JasonBModerator @jasonb]

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

[Ron LadenParticipant @ronladen17547]

Thanks guys , interesting stuff.

Ron

[Ian Johnson 1Participant @ianjohnson1]

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

[JasonBModerator @jasonb]

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.

I did not use any tabs this time as the material was thicker than needed, bottom milled off afterwards.

Quite pleased with the cut edge, no sign of cutter marks when held upto the light, this was a full depth finishing pass

I used a 50mm face cutter to thin the work down to 10mm moving the clamps to complete the ends, only downside to working with Corian is the mess.

I'll bond it all together with JB Weld but that won't be until the bearing supports have been fabricated and silver soldered to the top plate but could not resist a quick trial assembly.

[Ian Johnson 1Participant @ianjohnson1]

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

[John HaineParticipant @johnhaine32865]

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

[JasonBModerator @jasonb]

Sorry john missed your post yesterday, Drawn in Alibre then CAM in F360 using an exported STEP file.

A post on another forum brought up the subject of the "Star Wheel" used on the Alyn Foundry "Sphinx" engine which is an alternative to timing gears and operated the exhaust valve on alternate strokes. A casting is supplied but the latest batch are not upto the usual standards that Alyn were well known for so I happened to mention that if my casting was not usable then it would be something worth trying to cut on the CNC. Well that was all it took to get me trying it out.

Video firstly shows the adaptive clearing, I speeded things up 20% after filming so that was a 6mm Carbide 3-flute cutter at 3600rpm, 150mm/min, full 8mm height cut with a conservative 0.25mm DOC. I went with Andrews suggestion of cutting both ways which reduced the time quite a bit. It was cutting very nicely and I did not bother with brushing on anymore suds which only seemed to make the swarf stick to the work.

There is then a clip of a 4mm dia cutter clearing further into the internal corners which went well but during the final contouring cuts it went pop which almost made me go poop. It was a cheapie and at a cut height of 2D I was probably asking for trouble. I had drawn in a corner radius of 2.1mm but that probably should have been more.

Video ends having reverted back to the 6mm cutter for the final contour cuts which I slowed down so that it would not chatter in the corners.

 

This pic shows the star wheel after the first clearance cuts, you can see the faceting of the curves.

 

 

This is after all the milling where the curves flow better. Interesting to see the three height bands left by the tool, although it has not done much they show the wear from the 2.5mm plate, the 1/4" flat bar and the best finish at the top which can be seen better in the video is unused edge.

 

 

All that remained was to file out the internal corners, casting for the hell of it!

 

 

Edited By JasonB on 18/04/2019 15:22:36

[John HaineParticipant @johnhaine32865]

Thanks Jason. I guess that it could also all have been done in F360?

[JasonBModerator @jasonb]

Yes, it is just that I have Alibre and am used to using it so quicker for me to use that for the drawing.

[John HaineParticipant @johnhaine32865]

I think I will have to take the plunge into F360…

[JasonBModerator @jasonb]

I was always put off CNC by all the talk of G-code but have found F360 quite a straight forward way to go about it and have not had to actually write any code as the program does that all for you, I did just have to make a couple of slight changes but that was easy enough to pick up. First in the series here

I had previously only dabbled with the drawing side of F360 but after watching the 5 or 6 videos about CAM by Lars soon picked up what I need to know for now. The simulator for CAM is good for me as you can see what the machine will (hopefully) do from the comfort of your chair and make any alterations then immediately see their effects on the screen.

Edited By JasonB on 18/04/2019 18:39:49

[Ron LadenParticipant @ronladen17547]

The star wheel is impressive Jason, chalk and cheese when you compare it to the raw casting. I know they say you can set a CNC job running and go off and do something else but I think I would just stand there and watch it.

I looked up the Corian which is new to me, I should imagine its quite rigid and I can think of a few uses for it. Is it a heavy material and also is it possible to buy small sheets and different thickness.

Ron

[John HaineParticipant @johnhaine32865]

Corian aimed at kitchen fitters, best to approach one for offcuts, or try eBay.

[JasonBModerator @jasonb]

Ron the Corian is in deed quite rigid something along the lines of a cured resin and will tend to crack or snap if you hit a piece unlike a lot of other softer plastics, also quite heavy compared with other plastic.

As John says most commonly found in use as kitchen and bathroom countertops where 12mm thick sheet is bonded to an MDF subframe and additional material bonded to the front to give the look of a thicker material. I usually get a few offcut swhen I have these things fabricated but e-bay has quite a bit as it is use din other crafts like pen and wood turning.

I did this box top with an offcut

This was made to my templates and matches the counter tops

Nice integral basin in this bathroom that I did

Can also be made to look like thick stone slabs for counter and shelf

[Ron LadenParticipant @ronladen17547]

Thanks for the Corian info Jason I will see if I can get hold of some. Seeing the pictures of your work the wife said WOW and did I think I could talk you into doing a makeover on our bathroom….lol

[Author]

Posts