Bristol Mercury revisited

[mike mott]

Mike was the cutting done with cnc or by the hand dials? impressive bit of machine work.

Mike

[Vixen]

Mike

Other than the tailstock on the lathe, I do not have any other hand wheels, all my machines are CNC.

I guess if I had been turning the hand wheels by hand, I would have felt the cut and would not have over driven that unfortunate ball cutter.

Mike

[john mills]

was that a carbide ball nose end mill and what speed and feed were you you able to drive it at.
and are you able to use coolant  ?are you able to use coolant at high pressure and good flow.
It is always satisfying to see these shapes form when cutting on cnc machines.
I am following your projects with great interest .it must of been interesting to see factories processes making the
full size engine parts , the way they went about the machining at that time.

John   

[Jasonb]

Off to a good start Mike.

Have you thought about using corner radius cutters rather than ball nose ? They keep the cutting speeds about the same and you get better chip clearance, would also have left the tops of the lugs flat. I have always preferred them on the manual mill as they remove metal far quicker so seemed obvious to use them on the CNC

[AVTUR]

Mike

How long did it take you to machine the Hub Barrel?

I know you use CNC but if I was doing, not having CNC, it would take me a month of Sunday’s.

AVTUR

[Vixen]

John,

You are correct, it is a four flute carbide ball nose end mill. I have never learnt how to get the best from carbide tooling, so I prefer HSS. Perhaps that's because I do not have a high speed spindle or any form of pumped coolant to cool, lubricate and flush the chips. I usually cut dry, using low pressure air, a paint brush or the occasional squirt of WD40. My carbide cutters do not seem to stay sharp for very long and then they become prone to pick up and cold welding. My feed and speed rates are probably too conservative.  I still have lots to learn.

Model engineers often have to carve/create the external 3 dimensional shapes to represent a casting or forged item, It's a problem the original manufacturer never faces.

I have a very old book which shows how Bristol's manufactured the Mercury engines back in the 1930's. The factory was filled with large, carefully selected, single purpose machines, set up to do one and only one process; for all their working life. They had a dedicated cylinder boring machines with a dedicated operators. Their sole purpose was to produce accurate 5.75" bores in the cylinder forgings, week after week, month after month. I am sure they got realy good at it, with all that practice.

Next to the cylinder boring station was the lathe like machine which cut the cooling fins. Another robust single purpose machine which cut all 15 cooling fin slots in one go, using a long bank of 15 parting tools, it looked like a huge hair comb. Next door to that, was the multi spindle drilling machine which simultaneously drilled the 8 bolt holes in the base flange.

Thats a far cry from our small multipurpose hobby machines which are expected to do everything, milling, drilling, gear cutting and much more.

Jason,

If I were to do that machining operation again (heaven forbid), I would do it completely differently. I needed the 4 mm cutter to form the corner radius for the six lugs. I should then have changed to a larger diameter cutter to do the upper part. A larger, two or three flute cutter would have better chip clearance than the tiny 4 mm ball nose cutter. In hindsight I would also have changed the feed/ speeds for the upper part of the Hub Barrel.

I have never seen (except in one of your videos) a corner radius cutter, I have certainly never used one. I can see the obvious advantages you describe. What is the correct name for these cutters and where do you buy them from? I am guilty of always trying to make do with what's to hand rather than shelling out lots of money on new kit.

Another problem I encountered was with my CAM program. For some unexplained reason (probably operator error) it decided to produce a conventional milling toolpath for a few of the contours and the preferred climb milling for the majority. The tool melt down occurred during one of the  conventional direction contours. I would have corrected the toolpath direction if I were to make another one.

Contouring with a ball nose mill will always be a roughing process requiring hand finishing to achieve the casting/ forging look.

ATUR,

The real cost in time was in producing the toolpath program, that took several days of work. Each Hub Barrel half was machined in about four or five hours. Doing that much toolpath work for single item is not very cost effective. It would be a small price to pay for a large batch of identical parts, but for a one off prototype, no. It's still quicker (and safer) than doing it all by hand.

Mike

[sco]

Corner rounding end mill:

https://www.cutwel.co.uk/milling/milling-cutters/hss-co8-milling-cutters/4-flute-hss-co8-corner-rounding-end-mill-weldon-e2498-series

Following this project quietly...

Simon.

[Vixen]

Hello Simon,

I have some of these concave corner rounding end mills. They are intended for breaking/ radiusing the edges of flat plate work.

Unfortunately they will not do as a substitute/ replacement for a ball nose end mill. For that we need a convex radius, like a conventional end mill with the corners ground off.

Still looking

Mike

[john mills]

I  have used and programmed old machines that i too used low speeds 3600 top speed and mortar feeds and ordinary coolant but mostly worked on tough tool steel .latter i run and programmed a smaller light weight machine with had a 10000 rpm spindle ,Ifound it worked best with light cuts and high speed 4mm would have been at full speed possibly 1meter minute feed but i think the coolant supply at good pressure  got to the cutting edge and that made it work.
Only thing i would do is rough with bigger tools possibly 10mm ball nose and use the smaller cutter for the finish.
that depends on the cad cam program you have and at slow speeds it could take a lot of time.
I have thought dedicated machines and opperator as you have said would be the way it would have to be done
with the tools available at that time .it must of been a job doing the same thing all the time but that was the way it was done.I worked with some one that did the same job for the war years re boring or sizing ford v8 con rods .
 

[Vixen]

Hello John,

Better CAM software would certainly help in producing the toolpaths for different size cutters. I only have rather basic 2.5D CAD and CAM software, which can be slow work.

I considered a modern CAD/CAM package. Fusion 360 is well respected and (currently) free to the hobby user. But when I looked into it, I discovered the actual cost, to me, would be too high. First would be the cost of a modern, fast computer; which would throw me back into the clutches of Bill Gates and his over bloated WIN 10 nonsense. The second cost would be the time, lots of time, it would take to become  fast and proficient with the 3D CAD part and more time to become familiar and efficient with the CAM part of the package. Unfortunately time is one commodity us old guys do not have much left.

So I guess I will stick with my tried and trusted ancient 2.5D software, even though it's limited compared the clever stuff of a 3D package.

Mike

[sco]

Hello Simon,

I have some of these concave corner rounding end mills. They are intended for breaking/ radiousing the edges of flat plate work.

Unfortunately they will not do as a substitute/ replacement for a ball nose end mill. For that we need a convex radius, like a conventional end mill with the corners ground off.

Still looking

Mike

Sorry I completely misunderstood what you were trying to achieve 

When I put 'corner radius cutter' into Google I only get the concave type - do you mean a lollipop cutter?

Simon.

[Jasonb]

Model engineers often have to carve/create the external 3 dimensional shapes to represent a casting or forged item, It's a problem the original manufacturer never faces.

Well maybe not in metal but the pattern maker had to!

The 4mm dia would not be a problem with say a 4mm x 1.0R cutter, I have mostly used 6mm dia but have used a 4mm on smaller parts where the internal corners needed the smaller fillet.

In the UK they are called Corner Radius Endmills but in the US they are known as Bull nose (not ball), Fusion has they already loaded in the tool libruary so easy enough to just pic the size and make any adjustments if it is not quite right or their speeds are too high. I have been using the ones from APT which are reasonable quality far eastern https://www.shop-apt.co.uk/corner-radius-end-mills-4-flute-altin-coated-carbide-45hrc.html

Even though coated I have not had build up problems brushing on a little paraffin and using air, going to rig something more permanent up soon.

I think I would have roughed with a square cornered aluminium specific cutter, then contoured with a 6mm x 1.0R and Fusion has the option to then go back and machine bits that the 6mm cutter could not get to with a smaller 4mm x 1.0R cutter, it will also work out a shallow stepdown on the flatter parts and more on near vertical ones.

I've just been playing with some insert tooling that would be good if you did not need such a small dia cutter and may use that a bit more for roughing out at 25mm dia and 5000rpm you can get the right sort of cutting speeds for aluminium and feed to suit. You can get the inserts with different corner radii just like the lathe inserts. 0.8R as standard.

If you want to send me a part file I'd be intereted to see what Fusion makes of it.

[Jo]

...we need a convex radius, like a conventional end mill with the corners ground off.

Still looking

I have a cutter grinder, you are welcome to use it Mike. It does what it says on the tin in the name   

Jo

[Vixen]

Jason, Jo

Thanks for the link to the APT website for the Bull nose cutters. The corner radius (radii) are typically quite small , looks like the radii are intended as a protection for the cutting tip rather than for 3D contouring. I did see some 3mm R cutters which may prove useful.

I have recently bought a 12mm single insert end mill. It may be worthwhile for me to explore the availability of different tip radii and experiment a bit. However, I suspect they will all be small radii.

Alternatively I can take up Jo's kind offer and simply grind a larger radius on the outside of a conventional end mill. I believe a larger radius will produce the smoothest curved surfaces. So I now have plenty of options to consider.

Your description of the Fusion CAM package certainly shows what I am missing with my antiquated CAM software. For me it's a long slow process to generate a single version of a 3D toolpath. Multiple cutters as well as roughing and finishing passes are simply out of the question. Thanks for the offer to run a part file through Fusion, but that presents another problem; my drawings are all in 2D.

It's not the sophistication of the machine and software that matters, much depends on the man behind the machine. Even a basic machine and basic software can produce good results

Mike

[mike mott]

Even a basic machine and basic software can produce good results

Mike, Thanks for your answer regarding your tooling and I have to agree with your last comment. that said it can be very challenging.

Mike