What's new
What's new
By:
Advanced search…

Help Required - Machining Bronze - Ballpark Speed and Feed

H

HarryKSW

Plastic
Joined
May 30, 2013
Location
Fife, UK
I have been asked to quote on some large (Ø36.7" OD x Ø33" ID x 130" Long) bronze liners by our customer, this is not a common material to us and not much experience in machining and I am wondering if someone could point me in the right direction for typical cutting speed and feed.

Customer is looking for 2 quotes, one from Grade BS EN 1982-2008 CC492K and one from ASTM B271 Grade 92200, I have no idea if any discernible difference between the two from a machining standpoint.

Not a huge amount of material coming off (around 0.2" per side)but due to the size of the parts I`d appreciate any advice you can offer.

Thanks

Harry
 
HarryKSW said:
I have been asked to quote on some large (Ø36.7" OD x Ø33" ID x 130" Long) bronze liners by our customer, this is not a common material to us and not much experience in machining and I am wondering if someone could point me in the right direction for typical cutting speed and feed.

Customer is looking for 2 quotes, one from Grade BS EN 1982-2008 CC492K and one from ASTM B271 Grade 92200, I have no idea if any discernible difference between the two from a machining standpoint.

Not a huge amount of material coming off (around 0.2" per side)but due to the size of the parts I`d appreciate any advice you can offer.

Thanks

Harry
Click to expand...

Holy carp, those are big parts, and will be terribly expensive - you will NOT want to scrap one of those!

You need to know how these were made, they're most likely cast, and if in sand, you'll have to consider inclusions and the risk of gas bubbles. Might want some indemnification from the client that you're not on the hook if a tool catches and digs in due to either of those. And then there's stress relief, before machining, and after material's removed. And maybe a fifth for you when the parts ship...

Even fixturing will be a big deal, making sure you're not going to toss the part out of your lathe, or have it distort from gravity or clamping. Will you be doing vertical turning, or horizontal?

There must be a red metals trade association in the UK that can offer technical advice, I would ask them about the materials and "gotchas" when working with either of them.

I'd love to hear how this works out for you if you take the job.
 
Thanks Milland for the reply, the parts are centrifugally cast I believe and will be pre machined prior to arriving with us. We just get the fun job of finishing.

Parts will be Horizontally Turned on our Goratu Geminis lathe. We do similar shaped parts often for other customers in Steel & Inconel so fixturing should be taken care of, Distortion always a potential risk so treated with kid gloves.

I have another google search to see if any technical support around regarding the machinability of the parts. Thanks for your help so far
 
Bronze will be heavier and less stiff than either steel or Inconel, would be less of a worry if cutting vertically.

Cast Metals Federation | The Best in British Casting seems to be a UK society that could offer technical information on the materials you're dealing with. Or you could ask your client which foundry they'll be using, then contact their metallurgist. He or she should have suggestions regarding the materials.

And yes, I should have guessed the parts would be centrifugally cast. I blame lack of sleep for my forgetfulness...
 
Not going to look up those types, but for the record I have at least machined a half dozen or so types of bronze and it is very abrasive and eats tooling I remember the feeds and speeds I used were around those used for 316 stainless. Sorry but I cannot recall the types. I did not make giant parts, 2" diameter or less and 6" or less long. I also remember the round cast material being severely out of round and tapered with a lot of surface scale and voids. Good luck, you didn't say how many. Be careful, this is an easy one to shoot yourself in the foot on.
 
I'm not looking up the composition either.. But if its got aluminum in it, its going to be NASTY ABRASIVE..
If its got nickel, its going to be even worse...

Many moons ago, ran some ali-bronze castings. Wide open holes, but they were reamed since the size fell
in between drill sizes.. Wasn't checking them.. Got to the end of the run and checked.. The REAMED hole
size was .015" under the drill size.. It just wore the drill and the reamer away..

SHARP tools, any type of a land or hone, and things are going to get ugly fast... You can get up there
in speed with SHARP carbide, but HSS, you have to be careful, like I already said, it just wears it away.
Alloy steel speeds seem to work OK with HSS..
 
Those are both leaded copper-tin gunmetal bronzes.

I have much more experience with the tougher bronzes, nickel aluminium bronze, ampco etc.

These two both should be easy going by comparison.

Positive geometry cermets work well in bronze, generally. In the tough bronzes that I am used to, I use Sandvik grade 5015 in ccmt and dcmt and normally run about 90m/min and around .15mm/r. I expect you can get away with more in either of these grades, but that should serve as a starting point.
 
If it's the easier machining bronze, a little trick when turning it so that you don't get sprayed with chips is to use a small paint brush 1" wide or so and rubberband it to the tool so that it deflects the chips.
 
With as nasty of round cast bronze I have seen in 2" sizes with out of roundness, tapers, scale and voids I wonder what the hell 3 foot rounds would look like. Since quoted material tolerances open up more as they get bigger this is a scary proposition. If the OP gets this job and runs it I would love an update with pictures.
 
Mtndew said:
If it's the easier machining bronze, a little trick when turning it so that you don't get sprayed with chips is to use a small paint brush 1" wide or so and rubberband it to the tool so that it deflects the chips.
Click to expand...

Is that considering the size he is machining?
 
Thanks all for the advice, just bidding on it at present so will err cautiously and if it comes off I`ll let you know how I got on
 
HarryKSW said:
I have been asked to quote on some large (Ø36.7" OD x Ø33" ID x 130" Long) bronze liners by our customer, this is not a common material to us and not much experience in machining and I am wondering if someone could point me in the right direction for typical cutting speed and feed.

Customer is looking for 2 quotes, one from Grade BS EN 1982-2008 CC492K and one from ASTM B271 Grade 92200, I have no idea if any discernible difference between the two from a machining standpoint.

Not a huge amount of material coming off (around 0.2" per side)but due to the size of the parts I`d appreciate any advice you can offer.

Thanks

Harry
Click to expand...

.
.
usually cutting tool manufacturer will list recommended max with their particular inserts on various materials. tool holders vibrate and machine hp limits and various things like tolerances influence feeds and speeds
....i have seen same tool run fine at 60 ipm feed no problems but will have a lot of problems even only going 20 ipm if part vibrating or coming up against hp limits
.
also have seen finishing issues and holding tolerances. machine issues and tool holders used obviously effect things, a 20" long tool holder is run different than a 4" long tool holder
 
i have machined many big parts where when i removed a 1/2 ton of chips on top of part it would bow up cause well i removed a 1/2 ton that was on top of the part
.
tolerances can effect decisions on how part is machined
 
By my maths, at the 0.15 mm / rev feed suggested by by gregormarwick you are looking at approaching 35 miles worth of cut per pass! Given the propensity of bronze finish and size to go to hell in a hand basket in nothing flat once the edge has gone off the tool you need to think seriously about how long the tool can be expected to last.

On a job like that you can bet your bottom bippy that the gremlins have everything nicely arranged for the tool to crap out half way through the finish cut.

Probably equivalent to one pass over a thousand or two of the common sizes, say inch or two diameter, of bronze bushes that I tend to see (and avoid where possible).

Clive
 
Clive603 said:
By my maths, at the 0.15 mm / rev feed suggested by by gregormarwick you are looking at approaching 35 miles worth of cut per pass! Given the propensity of bronze finish and size to go to hell in a hand basket in nothing flat once the edge has gone off the tool you need to think seriously about how long the tool can be expected to last.

On a job like that you can bet your bottom bippy that the gremlins have everything nicely arranged for the tool to crap out half way through the finish cut.

Probably equivalent to one pass over a thousand or two of the common sizes, say inch or two diameter, of bronze bushes that I tend to see (and avoid where possible).

Clive
Click to expand...
.
many big thick inserts can handle higher feeds .010 to .020 ipt not unusual for roughing passes. but obviously not going to machine 10 hours on one insert
 
Rotguss in my language, red cast. I love it, chips spray off so nicely. You want to find the highest possible surface speed and a rather aggressive feed at a relatively shallow cut. Negative rake geometry, no sharp tool. Only the final two passes with sharp steels. Stress relief may force you to let parts sit for a day or two before next cut. I’d start with 200 m/min or 656 ft/min and increase to 250 or 820 respectively. According to Nickel content speed comes down by 20 percent. Avoid to cut too slowly under any circumstances, the aluminum will then spit in your soup.
 
You must log in or register to reply here.

Similar threads

OK_Bill
Compound/Crossfeed nuts - Material Choice: Bronze v Brass
Replies
15
Views
10K
Zahnrad Kopf
Zahnrad Kopf








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top