Best machining process

I have to make a disc 75mm in diameter, 12mm thick, with a 25mm hole in the middle. The dimensions (apart from the 25mm hole) are not critical. It needs an M5 tapped radial hole to take a grub screw to locate it on the shaft that goes through the central hole. I have a piece of 304 75mm x 12mm x 80mm stainless bar to make this from. Here is the process that I'm thinking of:
1. Mount the rectangular piece of stainless in the 4-jaw chuck, if necessary with some pieces of shim under it so that there is some space underneath to cut into in the next step. Drill a central hole up to 12mm dia in stages (e.g. 4mm, 8mm, 12mm).
2. Increase the size of the hole to 25mm using a boring tool.
3. Take the part out of the 4-jaw chuck and mount it in the three jaw chuck with the internal jaws.
4. Cut into the part from the side at 75mm dia using a parting type tool with extra clearance on the outside edge to allow for the curvature of the groove being cut.
5. Either cut right through the part from one side, or reverse it in the chuck half way through and cut from the other side.
6. Face both sides and the outer circumference of the part.
7. Give it a satin effect by holding silicon carbide smoothing paper against it as it rotates. It has to look nice.
8. Drill the radial hole using the pillar drill.
9. Tap the hole M5.

Is this a good process? Please say if this process won't work for any reason, or could be improved in any way.
Can I buy the tools needed to do this? Where from? Presumably they should ideally be carbide? Or do I need to make them myself from HSS? If so, any hint on correctly grinding the tools?

Thank you - Rowan

I think the trepanning process (step 4) is going to be difficult - especially in stainless and gripped on a 25mm hole in the internal Jaws. It's also not going to help with the final precision of the 25mm bore. I would

1) Make a short arbour from bar you have available. Put a flat on it.

2) Mark the centre of the bar and drill the hole to suit the arbour.

3) Drill & tap from one of the 75mm sides for the grubscrew

4) Rough out the circle with a bandsaw (or hacksaw!)

5) Mount the rough circle on the arbour using the grubscrew and turn the outside to 75mm

5) Remove the arbour, mount the disk in the chuck (3 or 4 jaw depending on the precision of centrality you need)

6) Face.

7) Flip and face then bore central hole to size.

Edited By Peter Cook 6 on 10/09/2022 20:41:34

I would saw off the 4 corners

Hold in 4 jaw and turn to 76mm dia for half the 12mm thickness.

Change to 3-jaw and hold by the 76mm dia to taken the remaining 6mm of material to the same 76mm dia over the full 12mm thickness

Drill and bore the hole

Hold by hole to take the last 1mm off diameter to your final 75mm

Drill and tap for grub screw

Remount in chuck or on a bit of 25mm bar so your fingers are away from the jaws and finish with scotchbrite or Emery

Edited By JasonB on 10/09/2022 20:52:04

Redacted!

Andrew

Edited By Andrew Johnston on 10/09/2022 21:18:04

I would:

• cutoff (3) corners so that the part fits in a 3 jaw chuck. Draw a circle and use that as a guide
• drill a 24 or 24.8 mm hole. Be gentle, the work holding isn't that good.
• turn or ream the hole to 25 mm
• face both sides gently.
• Make an 25 mm arbor to hold the part
• Turn the outer diameter
• Drill and tap the hole for the grub screw.
• Check the length of your tap before you start. 25 mm is on the limit. If you bore the hole thicker over a length of 10 mm, a standard 5mm tap will do

If you have a mill, you could also make the 25 mm hole on the mill.

If you face your 12 mm part, it won't be 12 mm thick after facing.

If this is your first exercise in stainless, take some practise cuts at this diameter on another piece of the same type.

If you use the jaws to hold the 25 mm hole, check if the hole fits the jaw. My 80 mm chuck can hold 23 mm on the outside of the jaws.

if you hold the part in the jaws, check if the jaws don't hit the lathe when turning.

Edited By Huub on 10/09/2022 23:39:19

Buy a custom water jet cut disc from one of the eBay suppliers and then machine the important dimensions. So much easier and probably no more expensive.

.

Very ‘forward thinking’ for someone with your alias

MichaelG.​​

I thought he already had the bit of flat material?

If buying something in a slice off a 3" dia bar say 15mm long would allow you to finish to 12mm thickness and 75mm dia.

Also if the job allows then buy 303 round bar as it's easier to work than 304

The first paragraph states " I have a piece of 304 75mm x 12mm x 80mm stainless bar to make this from". Why buy a second and waste the first piece ?

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

Simply because 304 is an unpleasant materiel to machine.

.

… and it’s 12mm thick

[ which is fine if you want the practice, but … ]

MichaelG.

Edited By Michael Gilligan on 11/09/2022 09:12:30

Maybe because Old School has been around the course before ?

Don't follow Michael. The OP says he wants the finished part 12mm thick which is why I left facing out of my method. Though from his own method it sounds like if a bit under that would be OK

Rowan, as Chris Evans said your choice of material is not great. 304 stainless is an awful choice for a novice to machine.

Does the part particularaly need to be stainless or is it just that you happened to have some so decided to use it?

25mm from OD to ID is far too deep to tap for a grubscrew, most especially in stainless of any sort.

I would drill about 9mm diameter x 15dp from the periphery, then tap the final 10mm depth M5. With stainless , I'd also drill above nominal tapping size, say 4,5mm.

If there are potential balance issues (eg. high RPM), I'd do the same from both sides.

By no means an expert, but what about using a rotary table on a mill, or CNC to do the job? I normally make things out of acrylic and other plastics (mainly because I can get offcuts FOC from my ex place of work!) My Siieg SX2.7 makes short work of maching 12mm aluminium bar, and my little 3018 CNC router cuts plastics up to 19mm easily, just takes a while.

My apologies, Jason …

I mis-remembered the opening post, and thought Rowan wanted 10mm

Anyway : If the faces on his slice are sawn, not machined, I still think he would struggle.

MichaelG.

Edited By Michael Gilligan on 11/09/2022 11:10:42

Although 304 machines reasonably well when cutting, it work-hardens in a blink if the tool fails to cut for any reason; blunt tool, rubbing, depth-of-cut, feed-rate or rpm too slow etc. Trepanning is high-risk for all of these, and 12mm being a deep cut will multiply the problem.

A fair amount of skill is needed to cut 304 and similar stainless steels without work hardening them. My first attempt to drill stainless was a disaster because I started with a blunt old twist-drill in a hand-powered drill. It work-hardened amazingly, and the hand-drill wouldn't touch it. Then it instantly blunted a new TiN coated brand-name drill driven by a power drill. Another new drill moved slightly to fresh metal, went through easily. No problem if 304 cuts first time, nightmare if it work-hardens. The difficult part is keeping the cut going.

Dave

Michael, I was assuming it was a bit of 75 x 12 bar as that is a stock size and OP says it is bar but if a rough sawn block it could well end up at 10mm

I did not put the reasons for my suggestion last night as I was wanting to get to watch something at 9.00 on the TV. My thinking is that by holding in the 4-jaw to get the part down to 76mm dia (will have a couple of small flats) is that it will be the most rigid setup for dealing with the interrupted cuts. If held on an arbor or by the bore with the 3-jaw it could well slip or at the least chatter.