Further Adventures with the Sieg KX3 & KX1

[JasonBModerator @jasonb]

I covered the CAD side of these patterns in this thread but have gone into a bit more detail about the machining here

With all the CAD work done it was time to fire up F360 to do the CAM and generate the tool paths to machine the patterns. The actual CAM would have been quite simple just an adaptive path to remove most of the waste, a finishing pass on the mainly near vertical surfaces and then a couple of small horizontal paths to clean up the top of the core prints and the top of the bearing supports.

However as the pattern is close to 105mm tall I would have needed at least that amount of tool sticking out beyond the collet chuck if I was going to avoid crashing that into the work, F360 certainly turned the screen red with masses of collision warnings even when using an extended shank cutter with 30mm projection. The answer was to split the piece into several layers which could correspond to the layers of wood I would be using to build up the pattern from.

You can see down the left hand side I have a number of adaptive and then ramp paths which are numbered in the order they will be cut.

The actual order they are listed is to allow me to run the simulation on a "solid" block starting from the top and fooling F360 by having a very long cutting tool so it doe snot show any collisions. This shows it about to do the last ramp cut where the blue waste will be removed to leave the green finished surface below.

So time to put it into practice. As I don't have quick change tooling I opted to do all the adaptive cuts first with a 6mm 3-flute cutter just screwing each layer onto the one below. Then I took them all apart, changed to a 4-flute long shank 4mm ball nose cutter and worked my way up again, this time screwing and gluing the layers together.

First layer roughed out

Second layer screwed on and adaptive cut just started

Second layer complete

And the third showing the amount of chips each layer produced

All 5 layers roughed out

With them all taken apart and the tool changed it was time to start the finishing cuts

And all done

[JasonBModerator @jasonb]

The core box was not so deep and I was able to get away with using extended shank cutters without having to resort to multiple layers. To reduce the amount of cutting I built up the block from one full size base layer and then just added three strips at the ends and top. Similar roughing and finishing paths were again used with the same two tools. The last path was the drilling of two holes for location pegs to keep the two halves of the box lined up, I used an HSS brad point drill for this as they produce a nice clean entry hole

With the second half done which was basically a mirror image of the first a couple of 6mm steel dowels were put in the peg holes and I was pleased that the two halves pushed together nicely.

It was just after this that I got an e-mail from Graham suggesting that some writing should be added to the inside of the base so that was added to the CAD model and then the CAM done for that. As it was 30mm deep into the corebox my engraving cutters were not going to be long enough so I opted to use a 6mm spotting drill which had enough length to still be able to get a good grip of and a reasonably pointed end. The halves were clocked in again on the mill and the writing engraved – right way round on the core box = wrong way round on the sand core which should hopefully equal right way round on the casting.

All that remained was a very light sanding with 180g paper and a coat of paint, we have just been using grey rattle can primer which seems to work OK.

[JasonBModerator @jasonb]

A bit more pattern making completed today. The aim was to try and produce a flywheel pattern that had a similar look to the curved spoke flywheels used on National Gas Engines. I made this one out of aluminium so it would be a bit more robust than timber as the spokes are quite thin section towards the rim

Quite pleased with how it turned out

More details in the video. Ramon best look away as there are some fast feed rates upto 650mm/min and cutters spinning at 5000rpm

I was the first time I used the peristatic pump fed fog buster in anger and very pleased with how it performed giving just enough liquid to wet the tool and stop tip build up and meant I could leave the machine running unattended. I used about 40mls over the six hours of machining which did not leave me with a dripping pile of swarf.

[Ian Johnson 1Participant @ianjohnson1]

Excellent work as usual Jason, I do like the curved spokes. The adaptive cutting seems to work very well.

Do you have any more info on the fog buster set up? I haven't done anything with my KX1 for months, been doing a lot of house stuff. So its about time I dusted it down, and the fog buster would be perfect for future projects.

IanJ

[JasonBModerator @jasonb]

!an, have a look at this thread over on MEM started by Mike (Vixen) my design is on page 3.

Now that I know it works I will tidy it up and put in a small box plus I either need to source a synthetic cutting fluid or buy in a supply of silicon tube for the pump. Probably the fluid as although there was no fog the fumes from the paraffin did build up.

[Ian Johnson 1Participant @ianjohnson1]

That's a neat set up, I think I've got a little peristaltic pump from an ink jet printer somewhere, might be able to use that? No doubt it will all grind to halt when I delve into the electrical bits!!!

[Ron LadenParticipant @ronladen17547]

Excellent Jason, how did you get the spokes from a square section to a round one. Was it part machining, part handwork..?

Ron

[JasonBModerator @jasonb]

Thanks Ron. It's all done by machining save you a quick going over with 180g emery once the two halves are together just to remove the very fine machining marks.

The video only shows the initial part of the process which is an "adaptive" cut. This is done at a maximum depth set my me in this case approx half the metal thickness which removes the bulk of the material and then it goes around the shape in progressively shallower cuts again with a set depth to each which in this case was 4.5mm for the deep one then 0.5mm shallower for each of the finer steps. This leave s a sort of contoured surface a bit like looking at the lines on a map

I then switched to a 4mm dia ball nose 4-flute cutter and used several different types of tool path. The first is what is called a "ramp" where the tool follows around the shape gradually getting lower as it goes, again this can be set and I had it at 0.2mm spacing per pass. This is the vertical depth which works well on the more vertical surfaces such as the hub and sides of the spokes but not so well on the more horizontal such as the top edges of the spokes as you can hopefully see see (click image to get it larger)

The final couple of paths were a "pencil" which cleans up the internal fillets and then a "scallop" to tidy up the tops of the spokes, this moves the tool a set distance along the surface per pass rather than a set vertical or horizontal amount.

These final ramp, scallop, pencil are what really determines how smooth a finish you get but it is a toss up between smoothness and run time as the closer together the cuts are the smoother the surface but if you half the distance you approx double the machining time. A larger dia ball nosed cutter will help smooth things out but can only be used if you have larger internal fillets so would not have fitted on this job.

[Ron LadenParticipant @ronladen17547]

Wow Jason that is impressive, I did wonder that with it been CNC it may have all been cut and shaped on the machine. Interesting seeing the cut lines on the larger image and where the spokes meet the hub and outer wheel.

Great stuff.

[Ron LadenParticipant @ronladen17547]

Out of interest Jason how long did the two halves take to machine. Obviously a lot of cutting but the time is of no consequence when you arrive at such a great result.

[JasonBModerator @jasonb]

Ron, the computer says 2hrs 39mins per side but it is actually a bit longer than that as the free version of F360 slows the rapid moves down to the feed rate but with a bit of tweaking that can be kept to a minimum so say another 10mins there. There are also a couple of tool changes where the height of the tool needs to be set together with the initial mounting of the work so I would say 3hrs per side

Luckily I can leave the machine to do its own thing for most of that time and do something else, just popping in when I know a tool change is due and the odd check to just make sure all is well.

[Ron LadenParticipant @ronladen17547]

Thats also impressive Jason, 3 hours per side I was thinking it would have been much longer. How do the cutters fare are they still good after 6 hours I was thinking thats quite a lot of work but for a quality tool maybe not. Do you tend to use carbide more than HSS or is it a mix depending on the job.

[JasonBModerator @jasonb]

Cutters had done quite a lot of work before this and will do quite a bit more. All carbide for the milling cutters on the CNC for me the main reason being that it would slow the job down a lot if I went with HSS with the bonus that the carbide stays sharper for longer

[JasonBModerator @jasonb]

The little Otto flame sucker that I'm working on has a form of scotch yoke that is pivoted at one end and connects to the conrod big end at the other. I had sent Graham Corry a basic sketch of this with the critical sizes from which he made a pattern and had some cast in brass with the intention to have the crank run against the brass slot. Having subsequently seem images of Tom's larger size replica I decided to go down that route which has split bearings for the crankshaft and to get them into place the bottom of the Yoke is a separate part.

I did a few alterations to my initial model while bearing in mind how I might machine the part and also ways to hold it and came up with this.

Wary that cutting a big notch out of the lower edge could make the steel go banana shaped I cut off a short length of 10mm x 100mm black hot rolled steel which should have less internal stresses than bright bar. After milling down to the required 8mm thick by taking 0.5mm cuts off alternate faces to keep the cuts balanced I drilled and reamed for the two 4mm holes and also stitch drilled out most of the waste material from the slot.

A couple of quick hacksaw cuts and the remaining waste dropped out so that the slot could be milled to the final 50mm x 10mm size and a pair of holes tapped M3 for the bottom plate retaining bolts.

Another piece of steel milled to 3mm x 8mm section with a couple of clearance holes completed the work on the manual machines.

The CNC is the best tool for the job on a part like this where there are curved features running into straight and angled ones so a session on Fusion 360 soon gave me a USB stick with all the tool paths needed, 5 per side which were:

1. Adaptive cut to remove most of the waste using a 4mm dia 4-flute R1 cutter at 5000rpm and 500mm/min feed
2. Ramp cut to finish the vertical and curved surfaces using a 3mm dia 4-flute carbide ball nose cutter at the same speeds and feeds. This was also used for the remaining cuts
3. Horizontal cut to finish the face of the webs and the "D" shaped big end boss
4. Scallop cut to refine the near horizontal parts of the three round bosses
5. Pencil cut which refined the internal fillets particularly where the three bosses meet the main body.

With the KX3 fired up the first thing to do was drill and ream for two location pegs in a bit of scrap aluminium which would locate in the two hole sin the yoke. I also tapped a couple of M3 holes to take screws to clamp down a top hat section clamping block.

It was then just a case of clicking "GO" and then getting on with something else, just popping back to change the tool and start the next tool path. Also just had to turn the yoke over half way through so the opposite side could be machined.

quite pleased with how it turned out. There is one small flaw in the steel that you may just ne able to see about mid way along the top flange between the oiler boss and big end boss. I could hear it as the tool passed but not really see what was causing the change in tone until the part was out of the machine as it was towards the rear when being cut.

Finally a couple of close ups of the tool marks left by the ball nose cutter as it stepped over 0.2mm between each pass of the horizontal path, they are more visual that physical as I can only just about feel them with a finger nail but as this was probably a casting or possibly a forging it will be fine after final fettling.

[Ron LadenParticipant @ronladen17547]

I know its CNC Jason but the parts you produce with it are seriously impressive and never cease to amaze me.

Ron

[Ian Johnson 1Participant @ianjohnson1]

Very impressive results Jason, never be able to tell the difference between a casting when painted

IanJ

[JasonBModerator @jasonb]

Well it's been a while but a couple of castings from the patterns shown on the previous page arrived today. Look to be quite good with little flash and the two halves seem to line up well. hopefully they will have soft centres.

I did have to get them out of the unexpectedly heavy parcel quickly to avoid the risk of cross contamination from the other well matureed castings with that special coating that made up the other 80% of the contents

[JasonBModerator @jasonb]

I've been wanting to try thread milling for a while and the need finally came up so time for a new adventure.

The part in question is a gland nut that fits onto the end of a steam engine cylinder to seal the piston rather than it having piston rings. The lower lip just needs to clear the 19mm dia piston and the thread I chose was M22 x 0.5mm and needs to go as close as possible to the lip.

 

I made use of a bar end of 1" brass and milled the top flat enough using the jog function as a glorified power feed control and then use the CAM in F360 to produce the code to firstly rough out the two bores leaving 0.3mm of material which was then taken to finished size in to passes of 0.2 and then 0.3mm.

A change of tool to a single tooth,5 flute thread mill took care of the thread, I ha dread of possible tool deflection so took light 0.1mm steps and a spring pass.

Quite happy with how it came out so will be using it again particularly as one cutter can do several pitches and almost unlimited diameters

 

Edited By JasonB on 11/05/2023 12:25:24

[John HaineParticipant @johnhaine32865]

Jason, thread milling is cool! I have use two tools, one a modified M8x1 tap, the other a standard small insert tip inside threading tool I got from JB a few years back. Conveniently that has a cylindrical shank with a flat and takes the insert with the cutting edge exactly on axis. The one made from a tap has to be used in conventional milling mode but the other was quite happy climb milling from the bottom of the bore. I cut an M14x1mm thread in one pass to fit the Unimat spindle and the fit was perfect.

[JasonBModerator @jasonb]

Thanks John, a couple of others have said they use reground "normal" taps which I'll bear in mind.

The female thread was only half the part and I really needed the male to make sure it all went together so I threaded a short length of bar with a test thread on the lathe and it screwed on very nicely. I made use of that test thread to hold the part while the remaining turning was done. Using one wheel only of teh diamond knurl gives a reasonable looking "rope" knurl

Happy with that I cut the thread proper on the piece of thick wall tube that will become the engine's cylinder. I'm running in reverse and cutting from the run out in groove towards the right which allows cutting at a decent speed.

And how it goes together with the cylinder support plate, I'll bore it out tomorrow and the thread will be nice and concentric to the bore.
 

Edit, looks like the forums reduction of image size make sit a bit hard to see the 0,5mm pitch thread so here is another shot, click to get it even bigger

 

Edited By JasonB on 12/05/2023 18:48:26

[NealebParticipant @nealeb]

I like the idea of thread milling but put off by the cost of cutters! The idea of a modified tap sounds interesting but how is it modified? My understanding of a thread mill is that it is "flat", and even a multi-tooth cutter (to get proper thread crest rounding) looks like a set of circular cutters stacked. A tap, of course, has a helical thread. Do you grind off almost everything to leave the equivalent of a single-tooth cutter?

Itching to have a go now…

(Shouldn't say multi-tooth, I realise, but I mean a cutter which cuts several adjacent threads at the same time. I see these listed in the catalogues)

Edited By Nealeb on 13/05/2023 08:53:06

[JasonBModerator @jasonb]

Yes you grind off everything except one cutting edge soo feed rate is a bit slower than the one I use das that has 5 cutting edges.

You can also get the "single tooth" style in full form so don't have to us the multi tooth ones.

[EmgeeParticipant @emgee]

Jason

I think those single point cutters are only suitable for a dedicated pitch but can do fine or coarse thread and as you say any diameter. Info below from the linked page,

These thread mills are suitable for machining internal metric coarse and fine threads with the same pitch using the same cutter.

Emgee

[Martin ConnellyParticipant @martinconnelly55370]

I found somewhere a figure for the minimum diameter of the thread being cut compared to the diameter of the cutting tool for straight threading tools with no helix angle. I think the tool had to be 60% of the thread diameter to ensure the thread was not overcut due to the tool helix angle (0° ) being different to the thread helix, the thread helix angle reducing as diameter increased. This means that if, for example, you wanted to make a 1mm pitch thread from a Ø6mm thread milling cutter the thread being produced would have to be 10mm diameter at least. A play with 3D CAD would confirm if this is the correct percentage. For purchased single pitch cutters I think the manufacturers will have a data sheet stating the limits of what can be done with each tool. I have also used a manufacturer's web site (Vargus) to create G code for one of their cutters, put in your parameters and it will either say no way or produce G code.

When you make a tool from a tap there is the added problem that the tap is at a fixed helix angle and the material behind the cutting edge is not necessarily going to have the same back clearance as a tool manufactured for the job. You would have to remove a fair amount of material from behind the cutting edge to ensure there was sufficient clearance or only use it on quite large diameters to ensure there was no rubbing or overcutting of the thread. Once again 3D CAD could be used to check for interference.

Martin C

Smiley removed

Edited By Martin Connelly on 13/05/2023 12:59:03

[JasonBModerator @jasonb]

Emgee, yes the full form ones will only suit a particular pitch as they have the correct radius for that given pitch exactly the same as full form threading inserts used on a lathe.

I was using a partial form so able to do any pitch within the range again like partial form threading inserts

this is what I used which will do 0.5 to 1.0mm pitch and anything in between, you need to make a slight allowance for the more pointed profile of the cutter when doing the larger pitch.

[Author]

Posts