Further Adventures with the Sieg KX3 & KX1

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.

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

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.

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

Ron

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

IanJ

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

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

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.

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

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

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.

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

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

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.

Somewhere on this forum there's a thread where the use of taps for thread milling was discussed with several contributions from John Stevenson, though I can't readily find it. I did contribute myself and John was very helpful. For my M14x1 internal thread I use two cutters (different trials). One was an M8x1 tap, with all the rows of teeth ground away except one and the tip ground square. That worked well but is limited to conventional milling down into the hole, and unless you also grind away all the teeth but one it will only do one pitch. A single point cutter (like my internal threading lathe tool I discussed) can start at the bottom of the hole and spiral out, climb milling all the way which is quieter and gives a better finish. To generate the code I used a little program provided by Chestnut Pens which Richard kindly modified to allow the use of a tap.

was this it ?

Aha! Thanks Jason, well found.

From one of my earlier posts in that thread:

After some though I decided that the helix angle of the tap isn't really a problem. You have to remember that the tap is significantly smaller than the hole you are threading. Yes, in principle as the tap rotates the helix may cause some rubbing, but both the smaller tap radius and its form relief are quickly taking the cutter surface away from the work, as it were.

Edited By John Haine on 15/05/2023 09:51:56

Well this will be the last adventure on this version of the forum.

A name plate that will be bent and then let into a recess on a cylindrical part to represent cast letters. They are raised and tapered though hard to tell if they are raise dor cut into the metal from the photo

Plate is 50mm x 32mm letters 3.5mm tall and stand 0.4mm out of the background. Apart from the contour cut around the edge all was done with a 60deg engraving cutter with 0.3mm end width, 0.15mm stepover running at 5000rpm and a feed of 200mm/min. I left it running while I went out to do other things as the run time was just short of 4 hours to get through the 83,000 lines of code.

The machining marks that are just visible on the background cannot be felt and will have disappeared by the time I have silver soldere dit into place, cleaned things up and probably bead blastsed for good measuer.

How long did that take to do Jason?

There is a big clue in my post