Further Adventures with the Sieg KX3 & KX1

[Ian Johnson 1Participant @ianjohnson1]

I haven't used backlash compensation yet. On my Z axis I do have a few thou backlash so I was going to tighten things up ready for a bit of 3d milling, but you have made the Z axis looser? How does that work?

IanJ

[JasonBModerator @jasonb]

I think mine was a bit too tight to start with and was slightly jerky when jogging down, looks like I have got it about right now.

[JasonBModerator @jasonb]

I had an hour to spare so decided to carve out another casting, this time one of the end plates for the Wall engine, turning of the spigot that locates in the crankcase and boring for the bearing had already been done in the lathe so just the external shape to be done.

After adaptive clearing and pocketing with a 4mm 3-flute Carbide cutter for aluminium at 5000rpm, 300mm/min feed, 4mm high cut x 1mm stepover on the adaptive and 1mm x 1mm on the pocket ramping down into the recesses.

Then steep and Shallow while I still can with the boundary set within the inner diameter of the flange, 4mm ball nose 2-flute carbide at 5000rpm, 300mm/min feed 0.3mm stepover.

After that photo I also used the CNC to spot and drill the four 3mm holes. The flange had been left with 0.5mm remaining which I went back to the lathe to turn off.

[Ketan SwaliParticipant @ketanswali79440]

Posted by JasonB on 07/11/2020 18:43:28:

Thanks Ian, I did toy with the idea of making it as a brass fabrication, it was going to be split down the middle so that I could mill out half round curved passages and then soldered together adding the three separate flanges at the same time. However I really wanted to do it in Aluminium so used Alibre to section my drawn part and then plotted what angle and depth I needed to drill in from to get the holes to meet without going too far.

I'm very pleased with the finish, just a few minutes with a needle file to tidy the fillets where the pipe meets the flanges though I could claim I did some very fine TIG welding. I adjusted the Z=axis gib the other day making it slightly looser and now don't have to program in any backlash compensation as before there was obviously a bit of sticktion which was leaving a slight ridge where the 3D path went from up to down.

that looks very close to the edge where the two points meet. Glad you got away with it.

Ketan at ARC

[JasonBModerator @jasonb]

It's more than it looks. Due to the web and fillets between web and curved outer there is still some metal to play with. I did use the DRO to get the depths of the drilled holes rather than just the quill feed scale.

[JasonBModerator @jasonb]

A while ago I posted a photo of some engraving cutters that I had bought from Sorotec in Germany and have finally got round to trying them out. Although a bit deeper than your average engraving my need was for some letters to apply to the side of a model to represent the cast on wording that would have been done with pattern makers letters. I found a couple of offcuts of soft bending brass which is a bit stickier to machine than the normal harder brasses used for machining and engraving so a good test for the cutters and with a thickness of 1.1mm a lot deeper than you would normally use them at.

To hold the sheet material I soft soldered it onto an off cut of 1/4" brass originally intending to just have a try and then do al the wording from a single piece but as the first letter went well I just squeezed the rest onto two smaller scraps. Taking the 60deg cutter with a 0.5mm flat end and running at 5000rpm and with a modest feed of 60mm/min and ramping down into the work at 2degrees for a max depth per pass of 0.25mm the cutters took it in their stride and seemed to produce a reasonable chip with minimal burrs left on the soft brass so I'm quite pleased with the result. After melting the work from the backing the letters just pushed out with finger pressure and a quick rub on some Emery had them ready for the next step.

I have been upto other CNC things some of which can be found in this thread. where I'll post the finished article in the next day or so.

 

Edited By JasonB on 31/12/2020 19:01:47

[Ron LadenParticipant @ronladen17547]

Posted by JasonB on 07/11/2020 16:32:19:

Edited By JasonB on 07/11/2020 16:39:20

I almost missed this and was just about to say it looks very good but that does not do it justice, it is truly excellent and if ever a part machined from solid looked like a casting this is it.

Great stuff Jason.

[Simon CollierParticipant @simoncollier74340]

Amazing work. How many hours a week do you reckon you spend in the workshop and computer, ie, all ME activities Jason? I have a tremendously productive mate, who can build a standard gauge detailed tender engine in under two years, including boiler naturally, and it is simply because he puts in huge hours. No mystery.

[JasonBModerator @jasonb]

Thanks Ron, I'm pleased with how it turned out too.

Simon, probably best I don't add up all the hours

[JasonBModerator @jasonb]

I decided to make a couple of Flywheels from Cast Iron for my Heinrici model, It was a good chance to try out the air coolant setup that I have been meaning to fit for a while. You can see the swarf build up on the ledges during the adaptive cuts as I was not able to manually clear it while taking the various video clips. But if you can bring yourself to watch through to the 5min mark you will see I have finally rigged up some air which is just enough to clear the swarf ahead of the cutter. The first side I stood over the machine clearing swarf more so on the adaptive than the finish but decided I did not want to waste another 3hrs each side. The second side and second flywheel were left unattended except for doing the tool change trusting F360 to have spat out the right code as each side and each flywheel was slightly different and all went well.

Ketan at ARC suggested that I use an air tool lubricator as I did not want to soak the place in coolant as this is what John Stevenson had set up ARCs own machines and his four Sieg CNC mills with. I'll only be using liquid when cutting aluminium but it certainly worked well doing the CI dry. Only a small amount of air is needed – the regulator was almost turned off and the swarf does not get spread all over the place staying in the "trough" that the KX3 comes with. I'll make the fitting a bit more permanent once I have tried it with liquid and then look at getting a quieter compressor as my old Machine Mart one is louder than the mill. The Loc Line is acting as a means to position the air only as I have run a 4mm OD PVC line inside that with a small brass outlet drilled 1.5mm to get the velocity up and it will save a build up of fluid in the Loc Line before it comes out the end.

[Ian Johnson 1Participant @ianjohnson1]

Good stuff Jason, turned out great as usual, I'm getting to like the adaptive machining it doesn't seem to put as much stress on the tool, and your air blower works well, I've got a small 9ltr shhh ultra quiet compressor from Machine Mart, bit expensive but does the job very well and it is really quiet, I have got an air gun to blow the chips away but it just blows them all over the place! So your low pressure set up is something to consider.

IanJ

[JasonBModerator @jasonb]

Apart from when I was adjusting the flow and got a bit too much and sent a bit of swarf flying I was more than happy with how little got spread about and was really no more than may have ended up there anyway.

This is the swarf in the trough and the small amount on the bench next to the machine after doing both sides of one flywheel. I have teed off the air so I can still have the air gun if needed.

[Ian Johnson 1Participant @ianjohnson1]

I've not done a lot of CNC work on my KX1 recently, but I am making a little tailstock for the 4th axis, just in case I want to do some gear cutting on a mandrel or something that requires supporting.

This is a little M6 brass thumb screw for the tailstock. I prefer a spline (or grooves) rather than a knurl, I think it looks better and gives better grip.

So if you want a bit of CNC action here's a link to a short YouTube video of machining the splines on the KX1, using my handwritten program for 18 splines. Works quite well!

If the link doesn't work here is a photo instead (with the 4th axis in the background)

IanJ

Edited By JasonB on 14/02/2021 07:04:39

[JasonBModerator @jasonb]

Good use of the corner of the cutter, gives a higher cutting speed than a Vee tool.

[Ron LadenParticipant @ronladen17547]

Ian, I must be missing something but the end mill will cut a 90 degree V wouldn't it but the V,s in the final picture look less than 90..? or at least that's how it looks.

Ron

[ZanParticipant @zan]

Interesting stuff Jason, always fascinating to see your efforts , you are teaching us all so much with your experience. Keep it coming!

how exactly did you align each side of the flywheel when flipping it over? I’m intending to do something similar, and considered a pin in the central bore then another removable one to mate with one face of the 1” dia holes you produced

did you use the “ tool stay down” feature ( can’t remember the exact wording} when doing the initial adaptive clearance?

[Ian Johnson 1Participant @ianjohnson1]

Posted by Ron Laden on 14/02/2021 07:29:55:

Ian, I must be missing something but the end mill will cut a 90 degree V wouldn't it but the V,s in the final picture look less than 90..? or at least that's how it looks.

Ron

You are right Ron, the V is not perfect, I aligned the cutter edge to 45 degrees from the centre of the job, moved the Y and Z axis equally and was out by a few thou! I think the Z axis zeroed itself, or I pressed zero by mistake and I over corrected the error.

[Ron LadenParticipant @ronladen17547]

Hi Ian

At least I know I,m not seeing things, not that it matters of course the thumb screw looks fine. I like that idea grooves rather than knurling, I need a pair for something thats coming up and I dont have a knurling tool so will give that a go.

Ron

[JasonBModerator @jasonb]

Thanks Zan, if you have a look at my post dated 17th Jan on this page you can see my setup of a piece of crankshaft material held in a collet to locate X&Y, blocks to locate in Z and the last photo shows the mark on the rim which was lined up with a pointer held in the spindle.

Ron, if you have a spotting drill that can also be used as a Vee cutter held vertically above the work's ctr line. Another option is to hold the work with it's axis vertically and plunge down with a small diameter cutter to take out half circles.

[Ian Johnson 1Participant @ianjohnson1]

Posted by JasonB on 14/02/2021 07:05:19:

Good use of the corner of the cutter, gives a higher cutting speed than a Vee tool.

Thanks Jason I think it produces a decent V shape, but like Ron pointed out it can look a bit 'off' if not set up correctly, it will produce a 'L' shape, although it will still be 90 degrees. I have made a few knobs and wheels with this method, mainly to get used to using the 4th axis.

IanJ

[Ron LadenParticipant @ronladen17547]

Posted by JasonB on 14/02/2021 16:16:04:

Ron, if you have a spotting drill that can also be used as a Vee cutter held vertically above the work's ctr line. Another option is to hold the work with it's axis vertically and plunge down with a small diameter cutter to take out half circles.

Thanks Jason, I do have a couple of spotting drills but never thought of using them as Vee cutters, makes sense when you look at the business end of a spotting drill. It also seems obvious to hold the work vertical and plunge cut the half circles, only thing is it wasnt obvious to me until you told me..lol.

[ZanParticipant @zan]

Hi Jason, I’m trying to do a small flywheel in 360 3” dia. I see in your video that the cutter goes round edges of the drilled holes and does not air cut . The cam cannot see these holes and thinks it’s a solid material so will try to cur them, not a problem nut all adds to the machining time. This would be easy in the ventricles 2d (which I now no longer use. Having to manually create contours) by just adding another circle on the face of the stock
as it’s impossible to add a hole in the blank in the design model where there’s no material, so there’s no hole edge to pick up how did you convince the cam to go round your holes???

Next Now that steep and shallow has gone from the free 360 version, what’s the best 3D cutting type. This is the first 3D Iv attempted, and all the path options in 360 seem to be very similar I have seen you using scallop, and contour I think so which is the best, I did see the discussion with regard to matching the tee piece

ps I did actually add a tube feature with a very thin wall , this seemed to work, but it’s very crude and I was wondering how you produced this bit of magic! The trouble with 360 is the bewildering no of options which can be confusing when it’s only used about once a week. It always seems to take so long to create the 3D design and cam strategy

thanks. Graham

Edited By Zan on 18/04/2021 10:26:56

[JasonBModerator @jasonb]

Hi Zan, The correct waty to do it would be to draw as separate part that is the shape of what comes off the lathe and mill/drill and use that when you are doing the setup by selecting "from solid" rather than box or cylinder but as I do it a bit differently.

This is the part as it was ready to put on the CNC, the OD and sides have been machines, the width of the hub has been machined and the 6 holes drilled

Part as imported into F360

So the setup I used was a fixed size cylinder dimensioned as the actual finished turned size. I then did an adaptive cut to emulate the turning of the raised hub with 0.5mm radial stock left but zero axial stock left as I had machined the side of the rim to finished size.

I then did another adaptive cut selecting a large diameter cutter and left some radial and axial stock, by playing about with cutter/stock you can get a hole about the size you have actually drilled.

From there I did the actual adaptive cut I intended to use making sure to select "from Previous" in the ticked "rest machining" section of the geometry. I used a 6mm cutter for this 1mm max load, 4mm max stepdown 0.8mm fine stepdown.

Then the finishing cut was all done using scallop marking the turned surfaces as ones to be avoided.

When you come to do the post process you don't do it for the first two but just start with the 6mm adaptive and it thinks the earlier two have been done on the CNC not separately.

It takes longer to explain than actually do. Hopefully if you click here it will open up my CAM file in F360 so you can run the simulation and look at the various paths. There are two setups as the other side of the flywheel is slightly different so one setup for each side.

[ZanParticipant @zan]

Ah so you don’t actually “drill” in the cam bit but use a virtual large milling tool in the triangular pocket which is too big to get into the corners ( which is used to fool the cam). I think the rest machining is designed to take out missing parts which the bigger.  Cutters can’t get into not used that yet, so many complex things in 360.  Not seen or used the “from previous “ more investigation,
thanks for that explanation. I’ll look at it on the desktop later
Thanks

 

ps keep your exploits coming!

Edited By Zan on 18/04/2021 19:43:33

[JasonBModerator @jasonb]

Yes there is a lot in F360 still to find but quite enjoyable to play around and see what it can do.

Should be another adventure soon, the cylinder for the parts I was making the crankcase and manifold for on the previous page is just about complete.

[Author]

Posts