NSW 'B' class mogul

[David]

In F360 it does have provision for programming the finishing pass(es) in a single toolpath, but it doesn't seem to have a setting for spindle speed, only feedrate. As I said I find it just as easy to duplicate the toolpath - one mouse click, remove all the multiple depth and stock-to-leave settings, set the feed/speed, and use that as the finishing pass. I think that's easier to understand than all the settings in the dialog box.

The other tricky thing is getting it to come into the cut the way you want. I had to use 'conventional milling' for one of these curved angles to get it to come in from the -Y edge of the stock because no matter what I did with entry positions on climb milling it just refused to enter anywhere that didn't require a plunge/pre-drill.

[Roger]

Feb 19, 2019 1:29:21 GMT David said:

In F360 it does have provision for programming the finishing pass(es) in a single toolpath, but it doesn't seem to have a setting for spindle speed, only feedrate. As I said I find it just as easy to duplicate the toolpath - one mouse click, remove all the multiple depth and stock-to-leave settings, set the feed/speed, and use that as the finishing pass. I think that's easier to understand than all the settings in the dialog box.

The other tricky thing is getting it to come into the cut the way you want. I had to use 'conventional milling' for one of these curved angles to get it to come in from the -Y edge of the stock because no matter what I did with entry positions on climb milling it just refused to enter anywhere that didn't require a plunge/pre-drill.

Although that calls it a finishing pass, it doesn't allow you to do the things that you want to do with one, ie use a different tool, at a different depth per cut.


Entry an exit can be tricky. Generally speaking, I always use a 3D entry along the tool path at around 3 degrees for roughing and leave say 0.2mm stock. Then I use a separate Finishing pass with a 2D entry, specifying a radius of 0.2mm in the X/Y plane and no linear extension so it drops neatly into the slot machined in the roughing operation.

Sometimes it tries to put the entry in a place where it can't create the arc, so it tries to plunge on a corner. In those cases, I use a linear X/Y entry that's 0.2mm long at an angle that puts it in the slot created by the roughing pass. Alibre CAM doesn't give you any clue as to what angle that might be, so you have to keep changing the angle until it finally shows you the entry tool path. Once you can see where that is, you can then adjust the angle to it plunges where you want.

I do it this way because it works for all types of work. The key thing it does is to allow you to machine into the top of whatever stock you're using, be that bar or sheet, and it doesn't matter how big the stock is. If you do it this way, you don't have to clear all of the stock or worry about plunging into it accidentally when roughing.

[David]

Yes, the duplicate toolpath for finishing in F360 is a more flexible method than using all their settings for the roughing pass, it allows you to change the tool etc. As long as you're happy to use the same type of operation which I am for 2D ops. 3D machining may be a different matter but I've only done that a couple of times and don't recall what I did.

I had to use a ramp for the first toolpath of these parts but after that I could come in from the stock edge. I've been programming both parts in a single program in case I do them for the other builders and was able to use the slot cut around the first angle as the entry position for the second.

[terrier060]

I must admit I do it all in one go with usually 2dinishing cuts. But for more complicated situations I separate the roughing and finishing. Then you can adjust feed and spindle speed and cutter if necessary.
Ed

[Roger]

Feb 20, 2019 21:30:51 GMT terrier060 said:

I must admit I do it all in one go with usually 2dinishing cuts. But for more complicated situations I separate the roughing and finishing. Then you can adjust feed and spindle speed and cutter if necessary.
Ed

Hi Ed,
This certainly works, but it takes a lot longer because you can't increase the depth of cut for the finishing pass. I go two to three times deeper for those, and usually double the feedrate too to it takes very little time to finish the part.

[David]

The boiler cladding is hopefully the worst job left on the loco, so I'd like to get it out of the way. I know some of you enjoy metal bashing but I loathe it.

I had a go at making the throatplate from 1mm CZ121 brass and that went about as well as I expected so a bit of time and money wasted. Other than the fact I'm hopeless at forming metal, I can't get the CZ108 brass Roger used unless I buy a full sheet or pay $100 AUD to get a 200mm sq sheet from a UK vendor. I'm not spending that just to bruise it with a hammer and have it not fit.



So I am planning to machine one from steel.



It is split in half to get it around the boiler barrel - it won't fit over the dome bush.

I've spent about 2 weeks measuring, drawing, modeling, programming, simulating, etc and had no end of crashes, broken tools, ploughed up clamps (despite the countless simulation runs) ... reprogramming, but finally got an MDF prototype out of the infernal machine. I've used a lot of MDF getting to here but at least it's cheap and quick to cut!

It is 12mm MDF with a 6mm radius on the front. The back (of the top at least) is hollowed out. The bottom just has a couple of cuts up the inside profile because I cannot get F360 to generate a sensible toolpath for the rest and have already spent more time on it than I'll need to clear it out manually.

I could really use some sort of fixture plate to set this up easily but I'm too cheap to buy or make one. Even steel is expensive around here and I hate to think how much a block of it would cost like Roger used when doing his formers. So I'm getting the material as square to the table as I can using an engineer's square and edge finding to get the reference point. Pretty slow and awkward. If I machine the outside edge, cutout for the barrel, and chamfer on one setup it doesn't matter if the inside clearing is a bit out of register.

I have 12mm steel and if that's not thick enough I'll have to come up with a plan B that hopefully doesn't cost too much.







It doesn't fit all that well, the cut-out for the barrel must need to be more generous on the bottom half. I was cutting it fine so that's probably ok.

The drawings show the boiler barrel cladding to be 139mm outside dia, which is 12mm greater than the actual barrel so there is some leeway. I've cut a hole 129mm and there really isn't much left at the thinnest point mid-barrel once the 6mm chamfer is on there.

I'm a bit confused how the 139mm fits with a maximum width of the firebox cladding of 143mm (given on the drawing) with any noticeable radius on the front of the throatplate cladding. I've gone to 144mm width because my boiler is wide and I think I've cut too much of the spectacle plate away. Barry obviously got it all to work because his looks good but I need to look at it again in person to see how he did it.

[JonL]

I'm sure it will come together to a standard which matches your excellent work so far. Good luck.

[Deleted]

I'm jealous David, I wish I was at the same stage, I love hitting metal with a 'hammer'... looking great as per usual sir.....

Pete

[David]

I went and spoke to the man who knows and (a) he reckons he would use the brass abomination (but he used to be a panel beater so knows a bit more about this metal forming rubbish than I do) and (b) pointed out a flaw in my machined cladding plan in as far as even if I managed to solder the boiler wrapper to the top half of the throatplate cladding (optimistic at best) it would be a neat trick getting the wrapper to sit nicely with the bottom half because it can't be soldered.

He's suggesting I fill the corners of the brass one with high temp soft solder and use a linisher to sort it out. He did one corner to demonstrate and that looks fine, but that's different to me doing it.

Then I have to make the bottom half of it look presentable and somewhere near to symmetrical.

But not today. Today (and yesterday) I've been arguing with F360 trying to get simple straight toolpaths out of it to machine some axleboxes from a bar of cast bronze. F360 - making the trivial impossible. I'd do them manually and it would be quicker but I need the practice on the infernal machine. I'll still do the bores manually because the Tormach only take up to a 3/8 drill and I don't have a boring bar for it. Boring a 19.05mm axle hole by moving the work in X/Y motions seems like a terrible idea.

[JonL]

I don't see you have much to lose to give it a try, worst case its a learning experience on something you were in two minds about using anyway. Either way, good luck!

[David]

Thanks Nobby. I'm going to try and salvage the brass one before going onto fresh material.

The good news is that (touching all possible pieces of wood) the simple first ops on the axleboxes went well. The sliding faces were between 0.02 and 0.04 over width after the first 0.25mm finishing pass. It was meant to be 0.15mm but the tool I used for roughing didn't cut where it was meant to. The finish looked a bit wobbly with a full depth finishing cut, it must have been near the top of the flutes of the endmill. I did a second one in two passes, half and full depth (6 & 12 mm), and that brought the width to 0.01mm under which I am very pleased with. This was a brand new 6mm endmill, 1500rpm, 60mm/min then 120mm/min feed, 0.15 to 0.25mm width-of-cut in bronze. These measurements are with Aldi guessing sticks so may not be correct.

I've spotted the axle bores and left the job in the machine with the machine on until tomorrow. I can't finish the bores in the CNC machine but I need to decide whether to drill out to 3/8 while in the current setup or do the whole thing on the manual mill. Then I need to run a 6mm endmill between each box to separate them. I cannot get F360 to do this after hours of arguing with it. I might have to do it manually too. Then clear off the significant amount of stock left underneath. By that time I'll have a few days into these 6 axleboxes and I'm not sure I trust my F360 skills with that operation.

Another problem I have is setting tool length offsets. The height gauge sold by Tormach to measure this is atrocious - the repeatability is about 0.1mm on a good day. To get this one right I used the Tormach guesser on the finishing tool to get it close then did an actual touch off on part of the waste stock and adjusted the DRO meaning the roughing tool will now be wrong. It was off by a long way.

How do you other CNC guys do your offsets? Set up a piece of scrap and touch off all the tools in one session to get it done?

[uuu]

I set all the tools needed for a job at the start. Mach3 uses Tool 0 as the master tool, and all others are offsets from it. So if machining a second piece, I only need to check Tool 0 and the others will fall into line.

I don't touch to set the tool. I bring it close, then slowly withdraw whilst holding a precision 6mm roller gently against the side of the tool. As it comes near to sliding under, I slow the rate of withdrawal right down, then stop when the roller pops underneath. Then I set Z to 6mm

Wilf

[Roger]

Mar 8, 2019 9:37:07 GMT David said:

Thanks Nobby. I'm going to try and salvage the brass one before going onto fresh material.

The good news is that (touching all possible pieces of wood) the simple first ops on the axleboxes went well. The sliding faces were between 0.02 and 0.04 over width after the first 0.25mm finishing pass. It was meant to be 0.15mm but the tool I used for roughing didn't cut where it was meant to. The finish looked a bit wobbly with a full depth finishing cut, it must have been near the top of the flutes of the endmill. I did a second one in two passes, half and full depth (6 & 12 mm), and that brought the width to 0.01mm under which I am very pleased with. This was a brand new 6mm endmill, 1500rpm, 60mm/min then 120mm/min feed, 0.15 to 0.25mm width-of-cut in bronze. These measurements are with Aldi guessing sticks so may not be correct.

I've spotted the axle bores and left the job in the machine with the machine on until tomorrow. I can't finish the bores in the CNC machine but I need to decide whether to drill out to 3/8 while in the current setup or do the whole thing on the manual mill. Then I need to run a 6mm endmill between each box to separate them. I cannot get F360 to do this after hours of arguing with it. I might have to do it manually too. Then clear off the significant amount of stock left underneath. By that time I'll have a few days into these 6 axleboxes and I'm not sure I trust my F360 skills with that operation.

Another problem I have is setting tool length offsets. The height gauge sold by Tormach to measure this is atrocious - the repeatability is about 0.1mm on a good day. To get this one right I used the Tormach guesser on the finishing tool to get it close then did an actual touch off on part of the waste stock and adjusted the DRO meaning the roughing tool will now be wrong. It was off by a long way.

How do you other CNC guys do your offsets? Set up a piece of scrap and touch off all the tools in one session to get it done?

I don't use offsets because the quill is used to set them on my CNC. However, professional machines have a touch pad that you can put the tool down on. Ideally, that would be permanently attached so that it wasn't influenced by taking it on and off the machine. You can buy dial clock version from eBay or adapt a plunger clock with a flat end and mount it on a fixture that sits on the machine bed.
Before you use this method, I'd want to check to see how accurately the machine homes in the Z-axis. My guess is that it isn't very accurate. That's because I don't believe they have a precision switch that's used for homing the machine. Professional machines use an encoder with a special Home pulse that sets this, it's not done from a switch. I'm sure there are ingenious ways of improving the accuracy of homing though if you want to turn that into a mini project of its own.

So if you can't do it that way, you're stuck with setting the tools off the machine in some kind of fixture, but you need a top notch height gauge and a good reference surface to get it really accurate. I don't think Tormach have really thought this through. Talking to them about backlash compensation convinces me they haven't really got a handle on precision machining.

[David]

Thanks Wilf. I might try your method using an old 6mm endmill shank rather than cutting the stock.

I think Tormach talks about a tool 0 scheme too but I didn't understand it. The one time I tried to follow it I crashed a tool straight into my vise jaws. The tool table in Path Pilot seems to be tool lengths from the end of the spindle which makes sense to me. I think Tormach considers tool 0 to be the empty spindle so they do happen to be relative measurements to that, but given you can measure them off the machine I think of them as absolute.

I assumed Tormach just used microswitches for the limit switches and I'll never get around to checking it's repeatability. How does an encoder get a special pulse in one place?

I see AvE has one of those tool setting devices on his new CNC mill and it looks very convenient. I'm extremely tempted to try and build a simple tool height setter as seen on YouTube - they seem no more than a switch completing a circuit between the spindle and a pin inside the control box, but I never finish those little side projects.

I'm trying to convince myself to buy Cliff's touch probe for edge finding. I reckon it would be little short of a necessity if the machine ever got used more than once a month.

[Roger]

Hi David,
I think Tormach use the limit switches for the reference position too, which is not clever. Microswitches don't repeat accurately enough to be able to machine a job in two sessions after turning off the machine. Commercial machines use linear or rotary encoders to measure where they are, unlike open loop systems like Tormach use where they take it on trust that it's gone where it's been told to move to.
Those encoders have three channels. The A and B channels are out of phase square waves so you can count the pulses and know the direction of movement. The third channel has a single pulse, repeating once per revolution on rotary encoders, or every so often on linear ones. The end switch on the machine just tells the control that it's ready to start looking for the first reference pulse it sees in the direction homing has been set for. This guarantees it will always find the precise same position every time it's homed, to the precision of the scales used.

[David]

I spent last night making some leaf spring brackets for the a couple of other guys making the same loco. Still another set to go. It was only the double-sided piece that was done, the other was done back when I did mine. I reprogrammed these parts to use full depth of cut (10mm) where possible with 0.5mm width of cut. It went well but my lovely 6mm carbide cutter is now throwing up burrs and giving a bad finish after this lot. It went through 10 brass axleboxes and came out almost like new but even free cutting steel has an impact. I got a good lot of parts out of it though and it will still be good on the manual mill.



Tonight I programmed, then redraw because the sketches in the model got stuffed up, and reprogrammed the reversing screw handle.That took a lot longer than the cutting did. It's cast iron because that's the only ferrous material I had of large enough diameter. I'm happy with that though because I'm guessing the real one was too back in the early 20th century and it's so easy to cut too. I'm quite pleased with how it turned out. The square pocket was done with a 1.5mm endmill after drilling right through 4mm. The spokes had 4mm holes drilled in their outer corners which was used as the entry for a 4mm endmill, depth of cut 1mm at a time. Then it was flipped over and the 5mm bore opened out with the endmill to meet the square pocket. It fits the reversing screw but I need to make a mandrel to hold it so I can machine the still solid side back on the lathe, and I also need to give a bit of a scallop to the spoke where they meet the hub and rim. In hindsight that would have been better done before I started, plus more of the thicknessing. I rushed into action without enough planning as usual because I wanted something to show at our scale running weekend tomorrow. At least I know the CNC program is good if I need to do it again.

[stevep]

Generally speaking, any tool used on steel is then useless for any brass-type material.

I even keep separate files for steel and brass.

[simplyloco]

Mar 29, 2019 17:03:32 GMT stevep said:

SNIP

I even keep separate files for steel and brass.

Me too: five very nice Swiss 8" ones plus a set of needle files!
John

[uuu]

Yellow cable ties on the brass files. Cut them off when they're ready to be relegated to steel.

Wilf

[stevep]

I like that idea, Wilf.