Best machining process

O.K. Jason … I probably got it all wrong

I will keep out of it for now

MichaelG.

Michael has started a demarcation dispute - getting it all wrong is my job!

Dave

Similar to Peter Cook,s suggestion.

1. make an arbor with a 25mm stub to mount the job. There should be a shoulder on the arbor which will keep the workpiece running true so there is no side to side wobble. The shoulder should be 10mm or so i.e. the o.d. around 45mm. The arbor should be turned in one set up so the shoulder and 25mm stub are true make the stub 0.5 mm shorter than the workpiece say 11.5mm, I would under cut the shoulder so only the outter 5mm supports the workpiece. Tap the the end of the stub 8mm or similar. Make a second ‘washer same dia as the shoulder with the centre hole clearance on your chosen clamping thread. Ideally undercut one side like the shoulder. Set this aside.

2. Find the centre of the the square/ rectangle and centre pop or spot drill it this will help in setting up. Remove any burrs from the edge to aid seating and chuck he square workpiece in the 4 jaw. Use the centre mark to centre the job. Bore the 25mm hole; centre drill then use the largest drill your lathe can safely handle, there is no point in doing excessive step drilling when you will be boring the hole to dia. as this will correct any error from the last drilling op.

3. knock off the corners by whatever method suits but don’t get it hot as the job might distort.

4. Re Chuck the arbor and get it running true on the stub dia. and shoulder face. Mount the job and clamp it up, get it running as true as you can i.e. minimise the side to side wobble.

5. Remove the corners, take it slow and watch out as the corners are near invisible when spinning. I would use an HSS tool as carbide won’t like the interrupted cuts. You can swap to carbide once it’s round if needed.

as for the grub screw it sounds like you are drilling radially, that’s going to be tricky to tap and I am not convinced that is a great method given the ratio of the disc dia. to its thickness.

Hope this helps.

Tony

I would not like to part off a bit of 304 stainless, even having industrial parting tools. The parting depth would have to be an inch. Tapping that alloy could go badly wrong also. The tapping would be subject to the length of the tap, the outer half of the hole might have to be clearance for the tap shank. Drilling the hole could be problematic, because of the alloy, I would drill the larger diameter halfway through first and then finish with the tapping size hole, not the other way around.

If the raw material is 75 x 80 x 12, by the time that it has been faced, it won't be 12 mm thick.

By working from corner to corner, the centre point can be found.

Assuming that your 4 jaw can accommodate the 75 x 80 mount it and face one side.

Note the comments about using sharp tools, correctly set,. to minimise risk of work hardening.

Centre drill

Drill

Bore to a suitable size, < 25 mm.

Turn up an arbor size and size with the bored hole. (Centre drill the arbor ready for later )

This would be a good time to saw off the as much of the corners as possible.

Mount the stainless on the arbor, machined face to the shoulder on the arbor. Loctite for added security?

Mount in the 4 jaw, and centre accurately. Use the Two Centres method.

Machine the outer to produce the 75 mm diameter.. Being an interrupted cut, take things gently!

You can use the arbor as a chucking piece to drill and tap for the M5 grubscrew. Drill through at 4.20 mm

Open up the outer hole to 5.5 mm x 15 - 20 mm deep.(20mm will leave 5mm of thread )

Tap the M5 thread.

Deburr the bore.

Hopefully, job done.

HTH

Howard

Thank you for all that hepful advice. It sounds like the "treppanning" process is not going to work, or is going to prove troublesome and difficult. Although I see that you can buy special "face grooving" tools for this (e.g. https://www.sandvik.coromant.com/en-gb/products/pages/face-grooving-tools.aspx). Does anyone have any epxerience using these?

So my process now (based closely on JasonB's suggestions) is:
1. Cut the stainles steel rectangle to a rough circle using a hacksaw. Whether this just means cutting off the 4 corners, or doing more cutting probably depends on whether I can reassemble and get working my power hacksaw.
2. Grip it in the 4-jaw chuck, and cut the outer 6mm to 76mm dia using an HSS tool.
3. Reverse it in the chuck (maybe change to the 3-jaw) and cut the other 6mm to 76mm dia.
4. Still holding it in the chuck, drill and bore the 25mm hole.
5. Hold by the hole in the three jaw chuck with the internal jaws and turn the outside circumference to 75mm dia.
5. Face both sides and the circumference.
6. Drill and tap the radial hole. I understand that I can't tap 25mm deep. I was thinking of just tapping it as deep as I could, and then "extending" the grub screw with a rod say 4mm dia ground to a conical point. This can just be loose inside the hole.
7. Finish with emery or similar. Make a 25mm arbour if necessary to protect my fingers

Other issues. If 304 is not the best grade to use, what is best? Yes, it does need to be stainless.
Yes, what I have is a piece of 12mm x 75mm bar. I know that facing it will end up with it less than 12mm thick. I was just going to take off enough to get a flat surface. The eventual thickness is not very critical.

Thank you - Rowan

I am confused by the metal description. 75 x 80 x12 mm BAR?

Does it need facing, Plenty of flat and round bar used as is and finished with a "brushed stainless" look straight onto the mill surface which sounds like to look the OP is after

It's certainly the way most architectural stainless fabrications are done such as handrails, brackets, furniture, etc.

If it is flat plate, I would produce the bore first and make an arbor to hold it, as already mentioned. When it is on the arbor, just touch a tool tip against the side to make a mark slightly bigger than the finished diameter and remove it from the arbor and hacksaw just outside the mark for a rough diameter. Then refit to the arbor and turn the OD. The dimensions mentioned leave no allowance for finished size or thickness.

303 stainless is the best/easiest to machine, doesn't work/heat harden easily. 304 is a pain the only real advantage it has is weldability which you don't need.

As I said earlier 75 x 12 is a stock size flat bar in stainless, cut to 80mm long

303 is easier to come by in round bar rather than flat bar or plate so also as mentioned earlier get a piece cut to say 15mm long from 3" (76mm) dia round bar and you will have enough metal to machine to the exact size of 75mm dia x 12mm thick. Someone like M-machine will be able to supply that.

Edited By JasonB on 11/09/2022 18:06:43

As a thought to the difficulties of tapping the deep hole for the grub screw, why not drill full depth tapping size, then only tap the first 7-10mm, just deep enough for the grub screw to be below outer surface. then use a small brass rod to make up the difference in depth. This way you don't need to tap the stainless so far. Brass will also help prevent scuffing the shaft it is going onto.

Thank you for all that hepful advice. It sounds like the "treppanning" process is not going to work, or is going to prove troublesome and difficult. Although I see that you can buy special "face grooving" tools for this (e.g. https://www.sandvik.coromant.com/en-gb/products/pages/face-grooving-tools.aspx). Does anyone have any epxerience using these?

So my process now (based closely on JasonB's suggestions) is:
1. Cut the stainles steel rectangle to a rough circle using a hacksaw. Whether this just means cutting off the 4 corners, or doing more cutting probably depends on whether I can reassemble and get working my power hacksaw.
2. Grip it in the 4-jaw chuck, and cut the outer 6mm to 76mm dia using an HSS tool.
3. Reverse it in the chuck (maybe change to the 3-jaw) and cut the other 6mm to 76mm dia.
4. Still holding it in the chuck, drill and bore the 25mm hole.
5. Hold by the hole in the three jaw chuck with the internal jaws and turn the outside circumference to 75mm dia.
5. Face both sides and the circumference.
6. Drill and tap the radial hole. I understand that I can't tap 25mm deep. I was thinking of just tapping it as deep as I could, and then "extending" the grub screw with a rod say 4mm dia ground to a conical point. This can just be loose inside the hole.
7. Finish with emery or similar. Make a 25mm arbour if necessary to protect my fingers

Other issues. If 304 is not the best grade to use, what is best? Yes, it does need to be stainless.
Yes, what I have is an 80mm long piece of 12mm x 75mm bar. I know that facing it will end up with it less than 12mm thick. I was just going to take off enough to get a flat surface. The eventual thickness is not very critical.

Thank you - Rowan

Plate is flat like a wall, and bar is cylindrical like a tree trunk.

The process that Martin suggested is almost exactly what I was thinking of (except that I was going to use steel rod rather than brass - I'm not too concerned about marking the shaft).

Thanks - Rowan

According to Google many suppliers use the term "bar" to mean a flat fairly narrow strip. Anyway, that's what I meant.

Thanks - Rowan

I used Jason's method to turn the flywheel or a ST engine, but I took it right down to finished size from the start. Saw the corners off (or angle grinder), grip in 4 jaw, set face to run true, turn half length of OD and bore the centre. Turn round in 4 jaw, set face and bore true, finish turn OD. A 4 jaw is much better for this kind of thing, it gets a much better grip for one thing. Gripping a rough sawn lump in a 3 jaw is chuck abuse. You can't see the join on my flywheels. If the OD has to be dead on then finish on a mandrel, but that is something else to make and it doesn't help rigidity.

If using angle grinder be sure to wear PPE and make sure the lump is well clamped down. The only time I managed to inflict a minor injury with an angle grinder they rushed me to the front at A&E as soon as I mentioned how it happened, they see very severe injuries. As it was I only had a deepish cut caused by picking the piece up without gloves before I'd deburred it

Other issues. If 304 is not the best grade to use, what is best? Yes, it does need to be stainless.

I have only machined 304 on my (CNC) lathe and it took some time to get the job done properly.

From what I have read on the internet, 303 is better for machining on a manual lathe. 304 is more corrosion protective.
The 400 series are easier to machine but are not as "stainless" as the 300 series
The L (leaded) series 304L, etc are better for welding.

I would go for 416 or 304.
You need sharp tools. If you use HSS tools, resharpen them often.

Edited By Huub on 12/09/2022 15:00:42

So what do you call a length of rectanglular section?

Most people would use "flat bar" or "#x# bar" or just "flat" and would not call it plate