The Sequel - Oh Blimey I bought a CNC Lathe (Beaver TC 20)

[djc]

...a close fitting plug in the holes...

And the very closest fitting plug possible might be to drill the long 6mm hole first, as a first operation on the raw stock, and the larger holes afterwards.

In the same vein, it might be possible to machine the perimeter of the stock so that the 6mm drill enters perpendicular to the surface, and then later on make the curve.

[awemawson]

Yes that would be best, but it very significantly adds to the indexing / locating issue which is bad enough already.

The stock is circular so your second idea can't unfortunately be applied.

Holding this thing so that it can accurately be inverted is still defeating me - certain features on both side MUST align, but machining both sides removes any location aids. The central through hole gives me an accurate bore that I can pick up with my Heidehain probe, but the rotational positioning is a hard nut to crack. I may have to machine a flat on the side but I am trying to avoid that. There are through holes for bolting to the spindle which are an obvious feature to use but they don't exist until the second side is machined.

I've decided that I'm going to leave both the male and female tapers unmachined, then set it up in the four jaw on the manual lathe and machine the female A2-6 recess. It then can be mounted on the target spindle on the CNC lathe and the A2-5 male taper machined.

[djc]

Holding this thing so that it can accurately be inverted is still defeating me - certain features on both side MUST align, but machining both sides removes any location aids.

There must surely be space somewhere on it for two 3mm dia. through holes which can go into a sub-plate for locating dowels when you invert it. Even without a sub plate, you can indicate it back in off the dowel pins and a straight edge. Plug the holes when finished.

No space or do not want holes? Weld/glue/soft/silver solder two lugs to the outside of the stock and put the location holes in them. Remove lugs when finished on mill and before transfer to lathe.

[awemawson]

I'll try and post up some 3D images tomorrow if I get a chance (grand daughter in tow at the moment !)

[awemawson]

OK Here we go - I've removed the A2-6 (female) and A2-5 (male) tapers and replaced them by a parallel sided bore and boss respectively as I intend to machine the A2-6 female taper on the manual lathe when the CNC bit has been finished, then fix it on the target spindle nose of the CNC lathe to machine the A2-5 male nose taper.

I think that CNC milling the A2-6 side has to be the first operation, as it provides the widest support when inverted to machine the A2-5 side.

So I think the operations are probably:

A/ Machine the A2-6 side

B/ Machine a spoil board flat and level with suitable holes for location pins

C/ Invert the adaptor A2-5 side uppermost on the location pins, clamp down

D/ Accurately locate centre of adaptor with Heidenhain probe

E/ CNC machine the A2-5 side

F/ Set up in 4-jaw in manual lathe and machine A2-6 female taper to (already ground) test gauge

F/ Mount on CNC lathe nose and machine A2-5 male boss testing to fit on actual collet chuck that all this fuss has been about (!)

NB the EN24T stock that I am using is 170 mm - adaptor max diameter is 165 mm so not much wiggle room.

[djc]

So I think the operations are probably.../

Sorry to keep posting on this.

I hope I am not teaching you to suck eggs, but when you invert it, depending on which axis you flip it about, either 12 and 6 will remain the same and 3 and 9 will be mirrored or the other way around. Clearly the code for the second side has to match what happens to the part.

In the sequence of operations, I do not think you included the long 6mm holes. Maybe it is 'G' or later. If it is, is there anything you can do before 'G' to assist it (e.g. small witness mark for clocking/angle of drilled hole - but maybe extended pins in the larger holes that the 6mm intersects could be used on the edge of a square to set verticality)?

[awemawson]

Absolutely no problem re more comments, the more input on this the better as far as I'm concerned !

Some time ago, and probably a page or two back up the thread, I cut a disk of thin plywood and glued prints of the A2-6 and A2-5 drawings on each side to ABSOLUTELY check that I had the correct orientations and handedness, as the original drawings that I was getting dimensions from were confusing to say the least, and I was deriving female cavities from drawings of male bosses.

(It's illustrated in reply #1008 above)

Unless I can come up with a foolproof method of being able to demount and remount the part in the correct radial orientation I fear that the long 6 mm holes will have to be done just before turning the A2-6 female taper on the manual lathe.

I cast another machinable wax billet this afternoon, and will have a full 'dry run' using it before attacking the EN24T.

I had thought that it would be easy to place a nice thick alloy spoil board under the part, drill two of the 6 holes that pass through the adaptor all the way into the spoil board and use them for locating pins, but sorting out clamping in that scenario is not straight forwards. Bolting the spoil board using the mills Tee slots is easy, but then re-clamping the inverted part that is impaled by the two locating pins becomes an issue. Clamps can only be on its sides as the entire top is being machined. Side bearing clamps will tend to dislodge it. I'm sure that there's a way but it's escaping me at the moment.

[djc]

...spoil board...

What I was afraid of with the flipping is that the operator would physically flip it in the X-axis and the CAM jockey would flip it in the Y-axis. The drawings on the part are good as long as both sides have high noon clearly marked on them.

It came to me in my sleep that you can use the T-slot as your spoil board. Make two T-nut blanks, three times the normal length. Drill and tap the first and last third of the length for grub screws to jack them into place against the slot bottom. Loctite the sides if paranoid. Location pin goes in the middle third. Relieve the underside of the middle third a little for breathing space when through drilling and reaming and for swarf clearance. Ideally, blow out drillings before reaming.

On the clamping, the old planer-era books show clamps that are like a standard milling machine strap clamp but with a pin sticking horizontally out of their nose. So the 6mm holes you need in the side of the stock could be spotted/counterbored maybe 1/4" and clamps with pins used in them. Spotting the holes slightly bigger allows wiggle room before final drilling and also gives a flat surface for the long hole to start on.

Found one: http://www.cartertools.com/spill.html

[awemawson]

Another one who solves issues in bed !!! Now that's certainly an idea to consider. I also was cogitating last night :

Suppose I plasma cut a thick flange that will loosely encircle the billet, with hold down holes that are a loose fit to bolts into the spoil board and sidewise pressing bolts that allow the inverted billet to sit impaled by the locating pin and clamp up tight as the flange and not the billet will be moved. Then when those are tight the hold down bolts into the spoil board can be torqued down and theoretically all parties are happy.

So this morning I did a quick cad drawing and cut a flange. The sidewise clamps are the current slight issue. I am limited to a total height of 25 mm or it will be clobbered by the milling operation, the easiest option is to weld pairs of M10 nuts on - flange is 6 mm nuts are 17 mm, 6 + 17 = 23 mm so low enough.

(picture actually shows M12 nuts and bolt 6+19 = 25 so too high)

[awemawson]

So I've just done an experimental weld of two M10 nuts onto a bit of 6 mm scrap plate to prove that it's possible and that the threads stay usable.

I'm glad to say that they do - I'd expected to have to run a tap through the pair but although they are a bit stiff when both engaged, they are usable. No doubt the heating / cooling of the welding has drawn the two tighter together on the thread but at least it shows that the method IS possible.

Saves making 8 steel blocks to weld on !

[awemawson]

Well despite having visitors for lunch I managed to finish the 'billet clamp'. Time will tell if it is strong enough but I think gentle cutting is the order of the day.

Were I doing it again I'd place the nuts closer together along the length of the bolts. As they are a standard M10 tap isn't long enough to pass through both to clean up the threads - only one was in desperate need and I had to grind back the shank of a bottoming tap for it to pass through nut 1 and clean up nut 2 !

[djc]

That clamping spider is very good. It will surely be useful to you in future as well and easy to add to if you have some horrible irregular part.

Allthread coupling nuts might be good to use for this as well. I have some M10 ones that are 13mm A/F so if these are common, that might help where space is short.

I think you are OK, but it is worth double checking that if the horizontal clamping bolt or lock nut ends up with its points vertical, it still meets the height restriction. Or use cap screws as the mock up.

[tom osselton]

That’s a nice clamp idea.

[awemawson]

I had one M10 coupler in stock and although the local Screwfix had them and was open Bank Holiday Monday we were suffering the annual London to Hastings 1000 motor bike run on the A21 outside the farm gate I didn’t fancy my chances! So I stuck to the double nut solution 😀

[Pete.]

 

I had one M10 coupler in stock and although the local Screwfix had them and was open Bank Holiday Monday we were suffering the annual London to Hastings 1000 motor bike run on the A21 outside the farm gate I didn’t fancy my chances! So I stuck to the double nut solution 😀

Lightweight

I went past your gate twice runing an errand to St Leonards. I would have stopped in but I was meeting someone and too pressed for time.

There were a lot of bikes though.

[awemawson]

Miserable fellow - you could have picked up my M10 couplers from Screwfix AND had a cup of tea 

[awemawson]

At long last I've been able to get a bit of time to return to this project. Life (or rather death) had got in the way. Sadly one of my long term flat tenants died suddenly leaving rather a mess to sort out, shame as he was a nice chap and very reliable (but his next of kin is in Panama!) and another problem tenant left again leaving a horrible mess. It all takes time, and not an inconsiderable amount of dosh to sort out.

However today I did actually manage to knock up a little G code program to surface the 'spoil board' and then sort out the CNC mill to mount it and machine it. The material is some very gummy aluminium alloy that I can't seem to get a good surface on, but that's OK it isn't particularly critical so long as it is flat.

The spoil board at 300 x 330 mm is pretty much the largest object that I can mount and work on with a 50 mm face mill without running into the limits set on the machine. In deed to find the centre I would normally use the Heidenhain probe, picking up each edge, lie to it to say that it was circular, and use the centre as X=0 Y=0, but the probe can't go far enough past the edge to work, so it was an eyeball job!

I used my Mitee-Bit clamps to edge hold it as the machining had to run off all edges, but first I hand filed the 'nasties' that have accumulated over the years, removed the heavy Kurt vice, and had a detour / diversion mining in the swarf to rescue the Allen Key and Tee nut that I managed to drop in there This plate was a test sample I was given literally decades ago and it has at times had to live outside

No more  playtime as it's guest check out / check in time

[awemawson]

I managed to get a little more done this afternoon between tasks.

The spoil plate needs a circle of eight M10 x 1.5 mm holes drilled and tapped to marry up with the matching circle of 15 mm holes in the billet clamp flange. So a bit of transferring co-ordinates from the flange drawing, specifying an 8.5 mm drill and M10 spiral flute tap in the tool crib, then actually mounting them and measuring their Z off sets before . . . Pressing the button 

It's always a bit bottom clenching waiting for the machine to smash your tools to shreds and ruin your work up to date, but no - it all worked without dramas and the billet clamping flange is loosely mounted.

The M10 hold down bolts are in 15 mm holes in the flange which I hope gives me sufficient wiggle room to get things aligned when I have to invert the billet having machined one side - time only will tell !

I may cut another machinable wax as a test before doing the EN19T billet - haven't decided yet

. . . back on duty now . . .

[awemawson]

It occurred to me that if I were to loose the X=0 Y=0 setting on the machine that determine the centre of the circle for those bolt holes it wouldn't be easy to re-establish it - unlikely as the machine control maintains them, but better safe than sorry so I need a feature that I can get the probe at (as the plate edges are too close to limits for the probe to work)

So this mornings fill in job while waiting for the postman was a nice and simple task - bore a 25 mm hole 20 mm deep accurately on the centre as previously established

Apart from checking that the loaded 22 mm slot drill WAS centre cutting, and that it's Z offset was correct - dead easy. So now if we have a power glitch etc I can get back to where we are now. Probably always sensible to incorporate some such feature in a part - even a spoil board !

[awemawson]

I've Fallen Down Another Rabbit Hole

Today's 'simple'  job was to turn a plug to go in the 25 mm hole in the spoil board incorporating a 10 mm upwards facing spigot, then fair face one face of the EN19T billet and centre drill and ream a 10 mm hole for the spigot. So the first action was to confirm that the hole in the spoil board WAS accurately 25 mm. A rough check with digital verniers lead me to question it.

So I dug out my 'Insize Digital Bore Gauge', a nice bit of kit that I've never used as someone had dismantled the probe end and not put it back together properly. A bit of intelligent 'looksee' showed that they'd fiddled with the range setting - easily corrected with a pair of miniature spanners. Checking against slip gauges showed that it was working fine .Note the picture with the gauge blocks shows it reading 4 microns undersize - that's just me not having zeroed it.

OK measure the bore in question gave me 24.894 or about 100 micron undersize - but why ?

At first I was sure that the 22 mm slot drill that I had used must be undersize as I've never had reason to question the accuracy of the Beaver Partsmater positioning system. A crude and rough check with a digital vernier seemed to confirm this but it's very difficult to get it bang on the maximum diameter of a two flute cutter - or at least I find it difficult.

So time to bring out the big guns - the PCM Toolset Tool Setter - BUT the extreme cutting edges of the two flutes at the tip were pretty well bang on at 11.007 mm and 11.020 mm.

Remember that the program orbits this 22 mm cutter to form the 25 mm bore -an undersized cutter will give an undersized bore and vice versa. If anything this cutter is very marginally oversized at 22.027 or 27 microns too fat.

So where is the error? Well I don't know, hence the rabbit hole comment, I need to find the source of this error before I proceed any further, so I think that I need to do more tests with other cutters and see what errors I get.

It can't be an undersized cutter as I've measured it

It can't be a bent spindle or holder as that would make oversized holes

The program doesn't leave a finish allowance so that's not it

Here is the program in Heidenhain conversational language

0 BEGIN PGM 14 MM
1 L Z0 R0 F15000 M91
2 TOOL CALL 10 Z S1455
3 L X0. Y0. R0 F15000 M6
4 L X-0.23 Y0. R F M3
5 L R F M8
6 L Z2.54 R F15000 M
7 L Z-20.0 R F192 M
8 L X-0.829 Y-0.781 R F384 M
9 CC X-0.074 Y-0.74
10 C X-0.15 Y-1.493 DR+ R F192 M
11 CC X0. Y0.
12 C X-0.15 Y-1.493 DR+ R  M
13 CC X0. Y0.
14 C X1.5 Y0.034 DR+ R  M
15 CC X0.744 Y0.017
16 C X0.842 Y0.767 DR+ R  M
17 L X0.018 Y0.229 R F384 M
18 L Z25.4 R F15000 M
19 L Z0 R0 F15000 M91
20 L R F M2
21 END PGM 14 MM

So please if anyone has any suggestions I would very much like to hear them.

[awemawson]

I 'think' that I can eliminate movement error in the Beaver Partsmaster because the 'error'  in bore diameter is exactly the same in X as in Y, but just for elimination purposes I set up a test.

Mounting a long travel digital plunger gauge magnetically on a set of hold down clamps firmly bolted to the bed I brought the collet of the spindle up against the plunger, over travelled a bit to compress it, and zeroed the gauge. Then I set the TNC355 controller to move 20 mm in the X axis and noted the indication - 20.002 mm and those 2 microns at the end are probably introduced error as I pressed the zero button.

So I believe that eliminates movement and scaling errors in the TNC355 controller and Beaver servo system.

So what the heck is doing it ?

Any suggestions would be very welcome !

[djc]

Your disappointing end product is the result of running one cutter once through a program. I think you might need a larger sample size to draw any conclusions and eliminate the problem.

Use the same cutter in the same material and do it again. See if anything changes. Blue up the sides of the hole and run the program again (effectively cutting air) and see if any of the blue is removed or the hole changes diameter. It might just be deflection, which could be removed by a spring pass. Try the same hole with a 6mm cutter, with a different number of flutes. Experiment with tool offsets to see if they change anything. Try the same cutter and program on a different material (change feeds as necessary) to see if anything changes. Do a series of five holes from a cold start and see if anything changes - maybe the machine needs to warm up.

Is it climb cutting or conventional cutting on the final orbit? Is there any issue with coolant? A 22mm cutter in a 25mm hole does not leave much space for chips - maybe air blast them out as they form.

[awemawson]

DJC thank you for your comments and suggestions.

I had already run the program a second time to see if a clean up cut was needed. (It is climb milling)

To eliminate cutter flexing (or maybe identify) I had decided to run the program again with the feed rates drastically reduced from the recommended levels, and went through the program first thing this morning editing them down to just 10% and had just run it when I read your comment!

The results are rather surprising (to me at least) as best as I can measure it at the moment is am getting:

Diameter in X Axis 24.914 so Delta X = 86 microns

Diameter in Y Axis 24.934 so Delta Y = 66 microns

So two odd things - firstly that material IS still being removed and secondly that there is a small discrepancy between X and Y

As the spoil plate is now fixed and centred I'm loath to dismount it for too many more experiments. I'll carry on with the machining of the adaptor as the critical dimensions will be finished machined on the lathe rather than the mill, and return to experiment when that is done.

But I will do a further run of the exceedingly slow feed rate version and see if  anything changes !


(Later Note: second run of 'slow feed' program removed approx 10 microns from both X & Y diameters ending up as  X=24.922 Y= 24.944)

I guess at this feed rate there is a bit of rubbing going on - cutter feels dead sharp but I don't have another 22 mm finish end mill, just roughing ones, as a substitute.

[awemawson]

OK OK enough of this messing about with oddities - time to get some work done !

So I turned up a stepped plug for the hole in the spoil plate, aiming for the mid point of the two measured diameters of 24.930 and 24.948 being 24.939 guessing that this should give me a fairly light press fit, which seems to be the case. Used a bit of unknown scrap that was an absolute joy to turn - I suspect that it's EN24T. Then I gave it a nominal 10 mm spigot 10 mm long - I aimed for 9.99 to go in a 10 mm reamed hole and actually achieved target!

Next to sort out the billet. It is a nominal 170 mm 60 mm sawn off the bar, so both faces were not necessarily parallel or square. Mounting it in the three jaw with jaws reversed I pressed it firmly home with the tailstock while tightening it - don't want that chunk leaping about the workshop - and hand spun it to estimate how far out the exposed face was. Answer, a tad over 1 mm. I skimmed it down by 1.1 mm which just left witness marks barely visible, then took a final cut of 50 microns to a fair finish.

Reversing it I hoped that the newly exposed face would be running reasonably true, and as expected I only had to take 150 microns off to achieve a fair finish loosing all the saw marks.

Then it was just a case of centre drilling, drilling out to 9.9 mm with jobbers drills, and passing a hand reamer though (supported by a tailstock centre) to finish at bang on 10 mm. The plug spigot fitted nicely. I took the precaution of drilling all the way through the billet so that were the spigot to bind I can knock it out. This plug / spigot jobby is sacrificial - it will be machined away as the adaptor is milled and I will probably have to drill and tap it to remove it finally from the spoil board!

[awemawson]

So at long last I've started machining the EN19T billet for the collet chuck to spindle adapter.

I've been holding off waiting for a 22 mm long series end cutting end mill to arrive,  but I got feed up waiting, and re-jigged the program to use a 25 mm NON end cutting 6 flute end mill instead - this involved ramping down into pockets rather than plunging. I still used a 22 mm end cutting roughing mill to start off the pockets then the 25 mm for finishing.

However despite being very careful to set suitable speeds and feeds, (even to the extent of confirming the actual hardness of the billet) after a short bit of cutting disaster struck, the roughing cutter stalled the spindle and the spoil plate was pulled off the bed of the machine when I raised the spindle 

Very close examination of the roughing cutter, which is a Sherwood Tools HSCO one, showed a tiny chip off one of the end teeth but no further damage so I really don't know why it happened. Flood cooling was washing chips away as they formed, but something jammed. It's not nice stuff to mill, EN19T, though I must say that it turned OK when I faced it.

As I had a reamed 10 mm hole in the spoil plate I was able to re-align it and re-fix it. Alignment being with two precision dowel pins, one the the spoil plate and the other in a collet, with a precision 10 mm brass collar between them. (Tap the plate about until the collar slides down!)

Having done this I was back in business, but I took the precaution of halving the feeds but I did use the same (one tooth chipped) ripper cutter - heck it has four other teeth 

After that things went OK but rather slowly due to the low feed rate.

It's a compromise - too fast too high a chip load and danger of breaking, too slow and danger of rubbing and not cutting, (and this material work hardens).

Anyway, the billet is now ready to be inverted for the other side to be milled, but that's a job for another day.