Speeds/feeds for 2mm mill in cast iron

[jaCK HobsonParticipant @jackhobson50760]

I wanted to cut some groves in 6″ dia cast iron plates like this:

I had a couple of small HSS end mills so thought that milling would be easiest for me.

Grooves are 1/16″ or 2mm, 0.5 mm deep. My mill goes up to 5000 rpm – this is the first time I used the high range, hurrah! It’s noisy at 5000rpm so I dropped speed down a bit.  I have power feed – I went about as slow as it will go. 1/16″ 2 flute lasted just over one plate maybe up to 4000 rpm. 2mm three flute maybe did one and two thirds of a plate maybe 2800 rpm. They snapped off when they got a bit dull. I used cutting fluid applied with brush.

What life should I expect from small cutters and what speeds/feeds would be best? To finish, I’ll be getting a carbide 2 flute and run it at 5000 unless advised otherwise.

[Bo’sunParticipant @bosun58570]

Just a though, but would a slitting saw work, with the job mounted on an angle plate?  A little clamp shuffling might be needed.

[bernard towersParticipant @bernardtowers37738]

Is it possible that using cutting fluid allowed swarf to get jammed under the cutter, shouldn’t you machine it dry and use a vacuum.

[Brian WoodParticipant @brianwood45127]

A better approach if you can manage it is to use a suitable width of slitting saw on a horizontal mill. Saw speed should be about 50 rpm with a good steady feed, cut each run in one pass.

Regards   Brian

Sorry, I see that route has already been mentioned

[RobinParticipant @robin]

Quick, somebody sell this man a shaper.

Some jobs simply cry out for one 🙂

best

Robin

[jaCK HobsonParticipant @jackhobson50760]

Shaper – you need a bigger one than I have. Slitting saw – reach is the problem… I’d certainly have to come at it from both ends. It is 30mm thick so I could just clamp it vertical in the vice, but still, not sure reach gets me to the middle.

Milling was the easy option for me – including workholding which is simples on a versatile vice. So what about feeds/speeds?

[BazyleParticipant @bazyle]

1/ machine cast iron dry and use a gentle air blast to clear swarf. The graphite and chippy nature of CI makes lubrication unnecessary.
2/ calculate the cutting depth of each blade on each revolution – you need to avoid rubbing so your slow feed at high rpm was blunting the cutter. 1 thou min per bite per blade every revolution.
3/ yes a high feed rate will put a lot of sideways strain on the small cutter so you will have to reduce the vertical depth.
4/ a better bet is to make an engraving V cutter as the form is designed for doing lots of thin lines.
5/ without a shaper you can still improvise by mounting the work on the lathe saddle and making a non rotating between centres boring bar to hold the cutter. Or on the mill table and non rotating cutter.

As you have proven by experiment that wasn’t the way to go.

[Thor 🇳🇴Participant @thor]

Hi Jack,

Your speeds seems to be OK. There is a nice calculator here. There is another calculator that gives both speeds and feeds here.
I always machine Cast Iron dry, Bernard’s suggestion of using vacuum is good.

Thor

[JasonBModerator @jasonb]

2-flute HSS use all your 5000rpm but you need a small chipload on a 2mm cutter so around 0.004mm which equates to a feed of 40mm/min which is prossibly slower than the power feed will run at. Cut the full 0.5mm depth in one go and do it dry with air or vac to clear swarf.

3-flute HSS 5000rpm but as they are a bit weaker 0.003mm chip load which gives feed of 45mm/min.

2 & 3-flute Carbide you will be limited to your 5000rpm max but chip load can be increased due to stronger tool say 0.006 so 90mm/min feed

[jaCK Hobson]

On jaCK Hobson Said:

Shaper – you need a bigger one than I have.

Is this a case of large material or small shaper?

We should be told 🙂

best

Robin

[jaCK HobsonParticipant @jackhobson50760]

Thanks! I think I conclude, combining Jason’s 40mm/min and Bazyle ‘you need to avoid rubbing’ that a sensible compromise is to accept limited life of cutters in this scenario (if I want to get the job finished before I give up of boredom). I’ll try 2 flue carbide to finish off, dry. I really appreciate the ‘dry’ – cutting fluid everywhere is yuk.

With this project I got to use some features that finally justified my tool purchase – 5000rpm, and wet-grinding six largish surfaces.

[SillyOldDufferModerator @sillyoldduffer]

Duffers patent rule of thumb for mild-steel:

rpm = 10000 / dia in mm

So 10000/2 = 5000 rpm.

If cutter is carbide multiply by 1.5 = 7,500rpm

In this case, material is cast-iron so a further correction may be needed.   A little complicated because cast-iron is a family of alloys with different cutting properties, not a single standard metal.   Generally, I halve RPM when cutting cast iron, so:

7500/2 = 3750 rpm   Then I experiment, because faster is often better: Jason’s 5000rpm is perfectly reasonable.

Beware!  Cast-iron is frequently nasty, full of occlusions, and/or chilled super-hard by being hosed down in the foundry.  Machinability varies from wonderful to very poor depending on what you have.  Rule of thumb cutting calculations may not work out in practice because “cast-iron” is pretty random, especially if it was chilled, causing a hard skin of unknown depth.  A small diameter cutter could sail through it, or come quickly to grief.

Using a small diameter cutter on an unpredictable metal is high-risk.   The cutter might happily plough through before suddenly hitting an occlusion or hard spot, blunting the edge or suddenly increasing the side load to breaking point.   Rapid swarf clearance is important, because it adds to side-loading and causes blunting.   Only the operator can judge, and I’d expect to break a few cutters before finding a safe optimum.  A steady hand is important too – bumping is likely to break a small cutter.  (You can guess how I know!)

Jason recommends cutting full-depth in one go and he is a much more experienced and effective machinist than me.  However, another duffer rule of thumb is to cut no more than 20% of cutter diameter deep, which is 0.4mm.   Therefore I’d probably cut these grooves in two passes.   My 20% rule is conservative though, and not entirely sensible!  Although shallow cutting reduces the side-load, taking two passes blunts the cutter extra fast, which increases the side load.  The pros and cons aren’t black and white.

How long will the cutter last?   Roughly speaking, a lightly loaded HSS cutter machining mild-steel will last a couple of hours before it gets too blunt.   Driven hard, fast and deep, perhaps only 15 minutes.   Jason’s 40mm per minute feed-rate is about right, so the number of cutters needed can be estimated from the groove lengths, and assuming mid-range life of an hour.  Except 2mm diameter cutters are easily broken…

In short, a highish RPM with a slow steady feed-rate, in either one or two passes, varied as necessary by the operator depending on the nature of the cast-iron.  Could be straightforward, or tricky, or somewhere in the middle – I’d expect to break a few cutters finding out, because so much depends on the cast-iron’s properties, which might be lovely, horrible, or mixed.

Dave

 

[JasonBModerator @jasonb]

14-15K rpm would be a reasonable speed for 2mm carbide in CI but as said will be limited to the 5000rpm top speed of the SX3.5. Three times HSS speed is a common rule of thumb when going up to carbide.

While I would agree with the 1 thou (0.025mm) chip load for most cutters when you get down to the very small you have to take their strength into account and reduce the load on them hence the 0.003mm I suggested which is almost 1/10th the loading. Keep the 1 thou for 6mm and above dia cutters.

[Robin]

On Robin Said:

… Is this a case of large material or small shaper?

We should be told 🙂

Shaper with less than 6” stroke might be a reasonable guess

… although 3” stroke and a lot of faffing-about may suffice.

MichaelG.

[ChrisLHParticipant @chrislh]

For anyone who doesn’t have a compressor or a suitabe vacuum cleeaner I have found blowing down a large diameter drinking straw to be surprisingly effective in clearing swarf if ultimately rather tiring.

[Robin]

On Robin Said:

On jaCK Hobson Said:

Shaper – you need a bigger one than I have.

Is this a case of large material or small shaper?

We should be told 🙂

best

Robin

I have one of those Adept hand cranked shapers. Nice tool to cuddle but I don’t use it much… not at all anymore.

[jaCK Hobson]

On jaCK Hobson Said:

I have one of those Adept hand cranked shapers. Nice tool to cuddle but I don’t use it much… not at all anymore.

This is perhaps not a good time to have money, this is a time to have things that will hold their value. Things like shapers 🙂

best

Robin

 

[Anonymous]

A decent grade carbide cutter should be able to do all three plates without replacement. I use K2 cutters from YG. These are South Korean professional, albeit bottom of the range, cutters.

For this job I would use a 2mm, 3 flute, stub cutter; 0.5mm DOC, 9500rpm and a chip load of 0.01mm/tooth, giving a feedrate of ~285mm/min. Running at 5000rpm would give a feedrate of 150mm/min.

Andrew

[David George 1Participant @davidgeorge1]

I have made similar plates which were used to lap the face of levers for aircraft controls. This was before CNC was around. To find hard spots they were surface ground and then laped on a granite surface plate with fine wet and dry paper and hard spots would usualy show up as shiny  spots or area’s and discarded. They were eventually cut on a horizontal mill with a slotting saw cutter.

David

[jaCK HobsonParticipant @jackhobson50760]

I was excited to open my package from ArcEuro containing new carbide 2mm stub 2 flute….. aaargh! The stub cutters have 3mm shank and I got a 6mm collet. Frustrating!

[Neil WyattModerator @neilwyatt]

As has been said above, speed isn’t critical although ‘as fast as possible’ probably isn’t bad advice for 2mm on a standard mill.

What is important is tooth load as too little will wear cutters rapidly leading and too much will snap cutters.

People have already suggested feed rates.

Neil

[jaCK HobsonParticipant @jackhobson50760]

I forgot I had an ER 32  – R8 chuck! Another tool justified, Hurrah! 5000rpm, carbide stub mill, dry…. smooth like butter (I listen to Kpop in the workshop). And the mill seems to have ‘worn in’ a bit at the 5000rpm now.

Now I just have hours of hand polishing to do.

[jaCK HobsonParticipant @jackhobson50760]

To (almost) finish off the story, I now have three lapping plates and surface plates. Now with a whole days experience, I’m not so keen on the grooved side – it can easily cause scratches, either because the grooves are difficult to clean and retain largest grit sizes, or because the edges can cause scratches.

The flat side is used to flatten a pitch lap. I can then get shiny glass with cerium oxide, but it is still a bit milky so I’ve got some learning to do still. And I don’t think the glass is coming out ‘optically flat’.

So the whole project – a fail so far… unless you count the learning…

[jaCK Hobson]

On jaCK Hobson Said:

I can then get shiny glass with cerium oxide, but it is still a bit milky so I’ve got some learning to do still. And I don’t think the glass is coming out ‘optically flat’.

Has the surface you’re polishing previously been ground flat?

Do you know what type of glass it is?

You may well be seeing ‘short finish’ where the glass between the grinding pits is shiny, but the pits remain – you should be able to see this with a loupe, etc.

There are two answers:

1) Polish some more, at the risk of losing the accuracy of the ground blank and rolling off the edges;

2) Re-grind to a finer grit. Ideally the blank should be ground finely enough that it has a waxy sheen before you start polishing.

How flat is ‘optically flat’? If you are looking for something that is better than a few fringes, then it is a bit of an art!

 

Good luck!

[jaCK HobsonParticipant @jackhobson50760]

I bought it as an optical flat off ebay. A bad purchase is at is scratched/worn beyond use.

Throwing good money after bad, I thought I’d have a go a repolishing and then seeing how flat it still is 🙂

I’ll try a lot more polishing. I don’t expect it will be very flat.

[Author]

Posts