Further Adventures with the Sieg KX3 & KX1

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.

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

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

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

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

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

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

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

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

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

Jason, I dont want to detract from this thread but a couple of questions if I may. Does the Corian take paint ok and the adhesive type to be used with it.

Ron

yes it paints OK, the bed plate of this engine has held it's paint Ok for a number of years.

They make a specific colour matched epoxy adhesive for it but I have used superglue, JB Weld and various epoxys to stick it with and all seem to hold OK.

Just something simple of the KX-3 today in the form of a truely elliptical gland flange and a couple of 2mm holes. I used one of ARC's aluminium specific cutters as the uncoated carbide works well in other non ferrous materials too. Had to be sure my heights were right as there was not a lot of clearance between the collet and the underside of the flange particularly when the drill broke through.

Edited By JasonB on 21/04/2019 17:09:37

Had a go a 3D machining this evening, just a simple dome but quite pleased with it for a first attempt. Did adaptive clearing to get rid of most of the waste, then finish machined the 4 flat areas at the top of the square with a 6mm 3-flute cutter before changing to a 1/8" HSS ball nose to refine the dome.

Ball nose was a bit past its best so possibly explains the poor cuts towards the top and I did not spend long enough setting tool heights right so a bit overcut where the dome fillets out to the flat.

Looking good!

The poor finish on the top is more likely to be due to slow cutting speed. I assume that the hemisphere was finished using a series of concentric paths, each one moving out and down slightly. At the top the cutter is only working on the centre, so the cutting speed is small (zero at the centre of the cutter). For a given feedrate the chip load is then large and the tool may be more rubbing than cutting. As one moves out and down the cutter starts cutting more on the side so the cutting speed goes up and the chip load goes down, giving a better finish.

Depending upon the part geometry the issue can be overcome by tilting the part, or using a 5-axis CNC mill that adaptively tilts the tool so it's always cutting on the outer part of the ball.

Andrew

[This posting has been removed]

Thank's Andrew, you assumed correctly that the contour was a series of circular cuts and as you say the middle of the cutter will not be doing much at the top pf the dime. I remember Murray's post about tilting the work which worked well, not having even 4th let alone 5th axis the other option that may be more affordable would be to invest in a radius corner cutter or "Bull Nose" as the Americans call them which would get the speed at the cutting edge up. I may simulate that as F360 has those cutters already in the tool library. Only downside I can see in using them is you can't get into tight internal corners in the X-Y plane.

Barry, there are several options that I still need to get my head around depending on the orientation of the curves on the part where the path can be set to give a more suitable step over. I need to watch the video again and do a few more trials to see what works best.

For the clearing I used 0.5mm cuts and 1mm vertical steps, the final contour to the dome was done with 0.1mm steps. Purple is waste still to come off, set to leave 0.5mm which I assume its at teh thinnest points and that would be about 1.3 at its thickest.

[This posting has been removed]

Thanks again Barrie, I do seem to remember from the videos that you can pick certain areas of the contour and specify different speeds, cutting directions etc which is something I will have to study more. I also need to find where to change stepdown to step over. Will also look to reduce the roughing steps.

I just changed the tool to a 6.0mm dia 1.0mm corner radius one and ran the simulation. At my max speed of 5000rpm it gives a surface speed of 95m/min which is the full 6mm dia so allowing for the 1mm radius the cutting speed when the very bottom of the tool is being used at the top of the dome would be around 63m/min at 4mm diameter which is quite an improvement on the near zero speed of the 3mm round nose tool. I also has the bonus of being able to finish the flat areas in the corners and would not be too bad to do the initial roughing as well so no need to change tooling.

Blue line shows path of ctr of the tool which is now further from the finished surface so actual cutting speed is up.

One thing I've learned the hard way is to look at the movements of the tool during the sim and in the toolpath. Some yellow lines (Fusion360 specific) can be easy to miss and a tool might go tearing straight through a stud or clamp in the middle of the stock when you didn't think it would because it was just cutting around the outside.

I usually make the clearance heights a bit low to save on head movements, but obviously it's called clearance for a reason! Plus of course you can model your studs and fixtures etc.

As for writing g-code I was also put off by all the articles that went though manually coding parts, not to mention the cost. But in 8 months I've not written a line of g-code, and only altered them a few times.

I've not had the need to do much on the KX3 over the last couple of months but thought I had better blow the dust off it and see if it (and me) could handle something a bit more complicated. I have been drawing up a 24mm bore single cylinder 4 stroke with side rods loosly based on a design published in Practical Mechanics in 1938 with the intention of CNC machining the two crankcase halves.

So with a piece of 1" 6082 T6 aluminium mounted onto a holding block I loaded up the code and let rip.

The first 3 clips in the video show the 3D adaptive clearing which was done using one of ARC's 6mm 2-flute aluminium specific HSS cutters, I was in two minds whether to use this as I had noticed a bit of chatter when using it in the manual mill in the past particularly as I wanted 27mm sticking out of the collet so that would not crash into the work but after a chat with Ketan a while back I decided to give it a go. 5000rpm, 8.5mm height of cut (1/3rd stock height) 1mm depth of cut, feed rate of 300mm per min giving achip load of 0.03mm which was just right and did not need altering. 0.5mm material left for finishing

4th clip is the same as above except height is reduced as the surface was between the two 8.5mm increments, this is where a tiny amount of chatter could be heard on the lighter loaded cutter.

Clips 5-7 are the 3D contour which was used as the sides of the crankcase all have draft angle rather than vertical sides. I used a 2-flute carbide 6mm cutter with 1.0mm corner radius. Again run at 5000rpm, with a 0.5mm stepdown and the DOC was the 0.5mm that was left, feed 400mm/min. In hindsight a 4 flute cutter would have been better as the amount of swarf was not great so the 2-flutes extra clearing capacity was not needed and then I could have fed faster.

Clip 8 Spotting the bolt holes with a 5mm HSS spotting drill at 5000rpm

Lastly drilling the 3mm holes with a Dormer A002 split point drill at 5000rpm and using a pecking cycle to clear the swarf.

Well that saved some work Jason, looks good. How long did the programme take, is it a quick process, I can appreciate the more complex the longer the programming.

Ron

Edited By Ron Laden on 04/07/2019 19:37:16