Opinions wanted - best CNC machine for this part?

[Alby51088]

Hi All,
This is my first post and your opinions / help is wanted.

We are looking at a contract to manufacture approx. 500+ large sleeve's from low carbon / mild steel with the below dimensions.
At this stage the best raw material size our supplier has offered is (approx.) 380mm / 15" OD x 200mm / 8" ID x 280mm / 11" long so approx. 170kg / 375lb for each piece of raw material.

This will need to be machined to final size which has a flange at one end.
OD of Flange End = 350mm
OD of Bush Body = 280mm
ID of Bush = 220mm
Length of Bush = 266mm
There are also grooves in the bore that require machining along with bolt holes and threaded holes on the flange end so live tooling will be required. I have attached a basic sketch to give you an idea but cannot share official drawings.

My question is, based on your experience, what type of machine and which brand and model do you think would be best suited to the manufacture of these parts? Budget is +/- USD 200k.

• CNC Lathe with live tooling? If so, which brand & model?
• Vertical Lathe with live tooling? If so, which brand & model?
• Mill Turn? If so, which brand & model?

Please let me know your thoughts, every ones input is much appreciated. Cheers.

 

[triumph406]

CNC Lathe (large) something like a Mori Seiki SL6 comes to mind.

Holes done on a VMC

Those look to be large holes on the flange, I'd think would be time consuming with live tools. So that's why I would do the holes on a VMC.

-----------------------

I don't buy new machines. Around here SoCal, could be tooled up for $15-30k

 

[ManualEd]

For almost 200k lbs of steel, you could buy direct from a mill.
They could probably supply ID and OD with only 5mm on it.
If tolerance allows, chuck OD, finish ID, custom ID clamping that lets you finish OD complete in 1 op.

Any lathe with live tooling will make short work of it, so long as it fits in the work envelope.
$200k will be shy for a new 12" chuck machine with milling and the tools.
I don't think it would get you a VTL with live tools new or used.

If you can go used, ~$100k should get you a 2000's ish Mazak QTN350 M with some live tools in the turret.

A casting would be ~1/2 the material, and reduce machining time by 80%...

 

[Alby51088]

Thanks for the feedback @triumph406

For clarity, the holes on the flange are 8x 18mm drilled through and 4x M16 x 2.0 threaded. The holes on the sketch that I attached weren't drawn to scale.

If possible, we would like to do as much as possible in 1 setup and on 1 machine to maximize production efficiency.

There are also grease dams in the bore which aren't on the drawing, these are a R60 and go approx. 75% down the length of the bore, not right the way through. Please see attached snipped.

I hope that helps.

 

[Alby51088]

For almost 200k lbs of steel, you could buy direct from a mill.
They could probably supply ID and OD with only 5mm on it.
If tolerance allows, chuck OD, finish ID, custom ID clamping that lets you finish OD complete in 1 op.

Any lathe with live tooling will make short work of it, so long as it fits in the work envelope.
$200k will be shy for a new 12" chuck machine with milling and the tools.
I don't think it would get you a VTL with live tools new or used.

If you can go used, ~$100k should get you a 2000's ish Mazak QTN350 M with some live tools in the turret.

A casting would be ~1/2 the material, and reduce machining time by 80%...

Thanks for the feedback @ManualEd

Good points buying castings direct from a mill, will investigate if we can reduce the machining time as much as possible.

We could possibly go up around 250k-260k for the budget but obviously want the best bang for our buck without compromising quality or accuracy.

Accuracy is also critical, we need to have 0.025mm or 0.001" tolerance on these parts when they are finish machined.

 

[Overland]

0.001" tolerance on a bushing that size does not seem realistic to me. Why so tight ?
Bob

 

[BajaFire]

0.001" tolerance on a bushing that size does not seem realistic to me. Why so tight ?
Bob

Because that was the default tolerance in Solidworks for a three-place dimension

 

[ManualEd]

Thanks for the feedback @ManualEd

Good points buying castings direct from a mill, will investigate if we can reduce the machining time as much as possible.

We could possibly go up around 250k-260k for the budget but obviously want the best bang for our buck without compromising quality or accuracy.

Accuracy is also critical, we need to have 0.025mm or 0.001" tolerance on these parts when they are finish machined

You could order a mill run of tube/pipe way closer to size than your supplier is offering is what I meant.
If the customer allows a casting, domestic Places can do a really nice job.

.001” tolerance will be easy for the machines, not so easy for the material.
It will move more than that from stresses so you’ll have to rough everything, do all your funky features, then finish.

A live tooled lathe that size will have no trouble with 18mm holes Or the 16mm tapped holes.
I have a 90s Mazak sqt15ms and run a 1” insert drill at 1400rpm/.0025”/rev.

 

[Donkey Hotey]

You should have mentioned your location prominently in the first post. Advice you're getting is probably based on the market in the US. I have zero insight into the local buying conditions for new or used machinery in Sydney. Used machines will come down to what might become available on your local market. New will depend on who sells local to you. Do you have some machines in mind?

 

[triumph406]

Thanks for the feedback @triumph406

For clarity, the holes on the flange are 8x 18mm drilled through and 4x M16 x 2.0 threaded. The holes on the sketch that I attached weren't drawn to scale.

If possible, we would like to do as much as possible in 1 setup and on 1 machine to maximize production efficiency.

There are also grease dams in the bore which aren't on the drawing, these are a R60 and go approx. 75% down the length of the bore, not right the way through. Please see attached snipped.

I hope that helps.

In your first picture the holes look a lot larger in proportion to the flange. So 18mm drilled and M16 tap no problem for a live tooled lathe.

 

[Alby51088]

0.001" tolerance on a bushing that size does not seem realistic to me. Why so tight ?
Bob

That's the machining tolerance on these highly critical parts. What machining tolerance would you suggest?

 

[Alby51088]

Because that was the default tolerance in Solidworks for a three-place dimension

No, that's not the reason at all. I didn't even realize that was the default tolerance in SolidWorks tbh.

 

[Alby51088]

You could order a mill run of tube/pipe way closer to size than your supplier is offering is what I meant.
If the customer allows a casting, domestic Places can do a really nice job.

.001” tolerance will be easy for the machines, not so easy for the material.
It will move more than that from stresses so you’ll have to rough everything, do all your funky features, then finish.

A live tooled lathe that size will have no trouble with 18mm holes Or the 16mm tapped holes.
I have a 90s Mazak sqt15ms and run a 1” insert drill at 1400rpm/.0025”/rev.

@ManualEd I really appreciate the feedback, thanks!

Yes, due to the stress movements we were going to rough everything, do all the features, then finish machine ID and OD last.

Thanks again.

 

[Alby51088]

You should have mentioned your location prominently in the first post. Advice you're getting is probably based on the market in the US. I have zero insight into the local buying conditions for new or used machinery in Sydney. Used machines will come down to what might become available on your local market. New will depend on who sells local to you. Do you have some machines in mind?

I was wanted advice and opinions about the type of machine best suited to this job so I'm happy to get advice based on the US market and experience.

Machines that have been suggested, i.e. Mazak, have a distributor down here so I will look into them and what their after sales service is like.

To be honest, one of the main questions I have thought of during this thread is vertical or horizontal going to be the better way to go? The answer to that then narrows down the machine make and model.

Based on your experience and the US market, what would your suggestions be?

 

[triumph406]

That's the machining tolerance on these highly critical parts. What machining tolerance would you suggest?

Well it depends on what the parts are doing, what the tolerances are of mating parts etc etc.

.025mm/.001" on a part that size is very tight. Your going to have to be carefull how you inspect, and hope the customer QA inspects at the same room temp, and is competant enough to be able to take proper measurements. Don't assume they can.
I'd have customer QA come out and do final inspection/acceptance at my shop.

if the tolerances were +/-.005" then I'd feel better about making those parts.

I'd no bid at +/-.001"

There are Engineers out there who will specify tolerances with no thought to what the part is doing, and no idea what the implications are of those tight tolerances.

------------------------------------------

And of course on top of your machine budget you need to have very competant operators. Not sure whether what it's like in OZ in respect to good competant machinists.
That's one reason I'd go the Lathe/VMC route, then the live tooled lathe route.

Last place I worked (Southern Cal) 9 out of 10 new hires didn't make it to the end of the first week, quite a few didn't make it their first lunch break.

 

[BajaFire]

No, that's not the reason at all. I didn't even realize that was the default tolerance in SolidWorks tbh.

That was just me being a smart aleck.

Me not being a smart aleck: I'm not sure what exactly you mean by:

Accuracy is also critical, we need to have 0.025mm or 0.001" tolerance on these parts when they are finish machined.

Is this +/-.001, +.001/.000? Those are two VERY different numbers. Also, I assume you have diameter of the bore in mind here, right? The non-essential features have much more generous tolerances on their diameters/lengths?

Grab your copy of the Machinery's Handbook. There's a whole section on Fits and Tolerances (right after the section on proof-reading drawings) that is very helpful. you just find your size range for the feature, move to the appropriate fit class (Driving, Clearance, Location, etc.), and presto you have your tolerance.

Edit: Also, you have grease dams (like this is some kind of bearing), but the parts are made from CRS (per post #1)...how does that work?

 

[EmGo]

A casting would be ~1/2 the material, and reduce machining time by 80%...

I've had unhappy experience with sand cast steel but if they have it near you, centrifugal castings would really be the way to go on these. The density and homowhateverness is about as good as bar, but much less material to remove. They should be able to spin your flanged shape even, which would save you tons of time and material.

If you start out near finished shape, then plus-minus one might not be so bad. You could get by with a much lighter (read "modern") lathe that way, too.

I'd hone and grind, but I'm kinda sick in the head

btw, people should not use the word "tolerance". This ain't the NAACP. What do you mean, EXACTLY ? plus or minus half is not the same as +/- one. Totally different animal.

 

[triumph406]

I'd hone and grind, but I'm kinda sick in the head

Big parts, either going to need a vertical hone or a large horizontal hone. Would have to be honed before the grease dams are put in. Time consuming too depending on how much material is left on the bore.

Big parts to grind too. I have a pathological dislike for grinding (was the scene of one of my more memorable f'ups starting out in the UK)

Yes you are a sick puppy! Got any pictures of long legged girls running a hone or grinder? Unfortuantly I'm working tonight. Need something to cheer me up.

 

[EmGo]

Big parts, either going to need a vertical hone or a large horizontal hone.

Yeah but easier than holding a thou on those parts ... I did a few hundred similar inserts but about half that size, carburized so had to id (two opposed keyways, can't hone) and od grind after, pretty easy to hold those sizes grinding, but most people don't like grinding. I love id grinding, it's almost my favorite thing ....

Got any pictures of long legged girls running a hone or grinder? Unfortuantly I'm working tonight. Need something to cheer me up.

Sorry, best I can do on short notice, but you'd maybe let her work in your shop ? If she brought her own surface grinder ?



A little more leg but she's just selling, not running it. Domestic tool and cutter grinder, similar to Anca or Walter ...



Would you buy a grinder from this person ? Top of the hill chongqing city, open every day ten to midnight ! Come one, come all, get your order in now, won't last long at these prices !

p.s., spin casting, for sure. Even if he had to import them, knocking out all that material is ridiculous.

I dunno, looking at the size .... maybe. Sure would save floor space. And yeah, screw it with the live tooling on parts like this.

 

[???]

Based on your experience and the US market, what would your suggestions be?

There is no similarity between the Australian and US markets. There’s a reason we don’t have a manufacturing sector anymore. Just trying to buy a machine here is an absolute mission. Good luck dealing with the local Mazak agent, this is from direct experience dealing with them.

I agree with EG about grinding. Easy to hold those tolerances.