What's new
What's new

Going fast on mild steel tubing

martin_05

Hot Rolled
Joined
Mar 11, 2009
Location
Valencia, CA, USA
I have this project where we would have to make a few hundred parts that look like this:

14-06-2021 09-52-46.jpg

This is mild steel tubing, 2 x 2x 0.120. I also have some parts that are made from 0.060 tubing.

I am very tempted to outsource this to someone with a laser tube cutter. I got a couple of quotes, one is ridiculous and the other can't deliver for many weeks. I won't even mention the folks who, two weeks after submitting an RFQ, can't be bothered to get back to me.

As a side comment, this is a persistent problem with US manufacturing. If I send 50 quotes to companies in China I get quotes back from all 50 of them (and sometimes a few more!) overnight or in a couple of days. In the US you are lucky if people get back to you in a week, if at all. This is truly frustrating.

Anyhow, it looks like we are going to buy the tubes pre-cut to length and just machine them on our VF-2 (8100 RPM spindle).

I am looking for ways to speed-up the cycle time per part.

Our tooling for steel is AlTiN coated, 4 flutes. I don't have a problem buying new cutting tools for this job if they would make a significant difference in cycle time.

The large slots are roughly 1 x 2 inches. All inside corners will be OK if we use a 1/8 in end mill to finish them.

At this point the strategy is to use the largest tool available (I think it is 1/2 in) to open the holes and then switch to 1/8 to finish the corners. It could make sense to go 1/2 -> 1/4 -> 1/8. Not sure yet. I'll be able to run some tests with scrap pieces towards the end of the week.

My thinking is that the opening of the hole goes slower because it is full radial engagement at the full thickness of the part. I am looking at about 3600 RPM and 40 IPM for roughing the initial slot.

I can then switch the same 1/2 endmill to a radial engagement of, say, 0.050 in and speed up to 4000 RPM and 65 IPM cutting speed. I could probably increase that to 0.100 in engagement and run at 50 IPM, this might be faster.

The corners is where I really have to slow down. For the 1/8 endmill I am calling out 8100 RPM (maxed out) and about 8 IPM, if that.

Another part has a 0.140 slot, about one inch long. This will be be slow. Not sure what tricks I can pull on this one other than buying a new cutter that allows me to go faster.

I'd appreciate any feedback (good, bad or ugly) on the above).


Thanks,

-Martin
 

Milland

Diamond
Joined
Jul 6, 2006
Location
Hillsboro, New Hampshire
I'd drill out all the corners with an 1//8" stub drill, then do all the profiling with a 3 or 4 flute 1/4" stub endmill. I wouldn't bother with the 1/2".

What level of burring can you handle? Might want to program in an undercutting burr tool, but small height variations can really play havoc on those.

Richen your coolant a bit. Slippery is good with mild steel.
 

martin_05

Hot Rolled
Joined
Mar 11, 2009
Location
Valencia, CA, USA
Burrs are not a problem at all. This is part of an assembly that will be welded. Any burrs will just melt into the bead.

Drilling the corners is probably the best idea. I don't need to center drill because, again, this is for a weldment and small deviations are not a big deal. A stubby drill should be more than good enough in that sense.

I was thinking of going for the 1/2 to reduce pocketing passes and be able to go faster with a stronger tool. I am also wondering if a 6 flute cutter would make enough of a difference with respect to a 4 flute. The math tells me 51 IPM for 4 flutes and 58 for 6, 63 for 7 and 81 for 9 flutes. At MSC a 1/2 AlTiN end mill with 6 flutes is about $65, 7 is $80 and 9 flutes $120. The way I read it is that $120 buys me 50% greater IPM.

If I go from 0.1 in engagement to 0.025 in I can probably hit 150 IPM.

In terms of MRR, with the same 0.1 in (20%) engagement, 1/2 in cutter:

6 flutes 0.87 (cubic inches per minute)
7 flutes 0.94
9 flutes 1.21


In terms of MRR, with the same 0.05 in (20%) engagement, 1/4 in cutter:

6 flutes 0.37
7 flutes 0.40
9 flutes Not available

For any given number of flutes and the same 20% engagement the 1/2 endmill will remove about 2.3 times more material per minute. I can't get a 9-flute 1/4 in. Comparing the 9 flute 1/2 in to the 7 flute 1/4 in means you remove material 3 times faster.

I am starting to think I might want to consider a larger cutter, maybe 3/4 in?

A 6 flute 3/4 in cutter at 100% engagement can take out about 5.5 cubic inches per minute. That's four times faster than a 9 flute 1/2 in tool. The price at MSC is pretty much the same, about $120 for a AlTiN coated carbide 9 flute 1/2 vs the same specification 3/4 in 6 flute.

This is why I am thinking that going in with the largest possible tool and largest possible number of flutes might be the right formula.

The other thing I am trying to reason through is that, on thin material like this (0.060 to 0.120) more flutes might result in less vibration for any given speed.

The formula, then, looks something like this:

- Drill out inside corners with 1/8 in stubby drill bit
- Take out as much material as possible with a 3/4 endmill with 6 or more flutes
- Come in with a 1/4 in end mill to clean-up the little bits that will be left around the inner corners (where the 3/4 can't reach)

I am using CAMworks, which doesn't have any kind of adaptive/high speed machining capabilities (unless you are willing to give them your left eyeball every year in license and maintenance fees). So if I am going to get clever it will have to be with some equally clever programming. That, or use this an an excuse to migrate CAM to HSMWorks and be done with CAMworks for good.
 

hahn_rossman

Plastic
Joined
Jan 27, 2010
Location
Seattle
You should price out rotary plasma cutting. Lincoln electric and others sell relatively cheap machines that could process this way faster than machining them. That's a lot of chattering/vibrating tubing cutting to do on a VMC.
Hahn Rossman
 

AARONT

Stainless
Joined
Feb 19, 2013
Location
Madison, WI
Check with any of the major metal suppliers near you. They should be able to laser cut that for you. You won't be able to run as fast as you want on that tube without a bunch of chatter and blowing out end mills.

If you insist on doing them in house, I would profile it out with a 1/4"EM and let the slug just drop, then clean up with an 1/8"EM.
 

spaeth

Hot Rolled
Joined
Jan 28, 2008
Location
emporium pa
Martin,
Anybody nearby with a big ugly punch press or iron worker?
Pretty simple punch and die would punch one notch per stroke and they make a lotta strokes per minute. No clamping no coolant and no broken end mills. My 2 cents.
spaeth
 

martin_05

Hot Rolled
Joined
Mar 11, 2009
Location
Valencia, CA, USA
You should price out rotary plasma cutting. Lincoln electric and others sell relatively cheap machines that could process this way faster than machining them. That's a lot of chattering/vibrating tubing cutting to do on a VMC.
Hahn Rossman

Yeah, I cut a few pieces today. The machine was singing. I played with RPMs to try to mitigate but there really doesn't seem to be a simple formula to make this happen without lots of chatter/vibration.

I have no experience with CNC plasma cutting. I did some looking around and learned of guys mounting an extension arm out the front/side of their VMC to plasma-cut outside the machine. Sounds wicked enough that I could see myself trying that one day (not for this).

What kind of tolerances can a real CNC plasma cutter hold? +/- 0.010" is probably fine for this job, maybe more.
 

martin_05

Hot Rolled
Joined
Mar 11, 2009
Location
Valencia, CA, USA
Check with any of the major metal suppliers near you.

I did. The quote I got was insanely high. Maybe they are trying to amortize their laser tube cutter quickly...or, perhaps, they charge a lot just to avoid being in competition with raw metal customers.

If you insist on doing them in house, I would profile it out with a 1/4"EM and let the slug just drop, then clean up with an 1/8"EM.

Yup, was thinking about that as well. It might have to take the form of holding the slug with small tabs in order to avoid damaging tools as the slug fails to drop in a "civilized" fashion. It might just beat removing material you don't need to remove.
 

martin_05

Hot Rolled
Joined
Mar 11, 2009
Location
Valencia, CA, USA
Martin,
Anybody nearby with a big ugly punch press or iron worker?
Pretty simple punch and die would punch one notch per stroke and they make a lotta strokes per minute. No clamping no coolant and no broken end mills. My 2 cents.
spaeth

How would a punch press support the bottom of the cut in a pipe? We do a bunch of sheet metal work. Our vendor has CNC punch presses, but I think it will only handle flat stock. The negative side of the die has to be on the bottom of the sheet.
 

cyanidekid

Titanium
Joined
Jun 4, 2016
Location
Brooklyn NYC
Yeah, I cut a few pieces today. The machine was singing. I played with RPMs to try to mitigate but there really doesn't seem to be a simple formula to make this happen without lots of chatter/vibration.

I have no experience with CNC plasma cutting. I did some looking around and learned of guys mounting an extension arm out the front/side of their VMC to plasma-cut outside the machine. Sounds wicked enough that I could see myself trying that one day (not for this).

What kind of tolerances can a real CNC plasma cutter hold? +/- 0.010" is probably fine for this job, maybe more.

yup, LOL! I was going to post that you could forget about all your MRR calculations because this is tube...

a decent hi-def plasma can get you well within that tolerance (generally), but I think a fiber laser will make a much cleaner cut particularly at sharp outside corners and projections.

anyone really serious about throughput and cost per hour will be running a fiber laser for tube work, but with the high capital cost up front they will probably not want to bother with a few hundred parts. I'd keep looking for a shop that doesn't mind doing those quantities though, and if you go in understanding that you are a PIA job for them that is hardly worth it that MAY help. good luck! :)
 

spaeth

Hot Rolled
Joined
Jan 28, 2008
Location
emporium pa
Martin, I would think the the die or bottom would be under the top side of your square tube. So you would slide the part onto the die plate to a stop, punch it slide it off then rotate for the next notch, maybe all eight notches in a minute or so. 1/8" thick by 1/2" x 1" shouldn't need much more than 10 ton press or small ironworker. There may be standard ironworker tooling for that notch.
spaeth
 

Nagol

Aluminum
Joined
May 21, 2020
I would recommend a Gorilla Mill brand Knuckle Dragger in 3/8" to do most of your roughing. The variable geometry of the flutes and chip breaking shape should eliminate most or all chatter. From there I would go to a 3mm or 1/8" Yeti from them. These also have variable flute design but no chip breaker. Recommended feed and speed on these for mild steel is 800 SFM and .008 on the 3/8" tool and about .002 for the 1/8". I would probably start with a Yeti for both though. They tend to not chatter in thin stuff pretty well. They last a long time at these speeds. I would expect 50 complete parts per tool at least from what you've shown here. 3/8" tool runs about $40 and the 1/8" is about $20.
 

Garwood

Diamond
Joined
Oct 10, 2009
Location
Oregon
I did a bunch of 2x2x.120 tubes on a VMC because they were part of a precision table and the weld shop wanted all weld prep and fits perfect.

I did not have any small inside radius to deal with and after playing around some I threw an old cobalt corncob in and it chewed threw that tube WAY faster than I could reliably run it with carbide. The edges looked pretty good, had to play with size a bit to hit my numbers with a rougher, but it worked great.

That said, that part is an obvious punch job. 20 ton OBI will dominate that part. EDM shop could cut the tool hard and you could be running that in a day. I would guess a minute per part if you're cutting one slot per hit.
 

martin_05

Hot Rolled
Joined
Mar 11, 2009
Location
Valencia, CA, USA
I would recommend a Gorilla Mill brand Knuckle Dragger in 3/8" to do most of your roughing. The variable geometry of the flutes and chip breaking shape should eliminate most or all chatter. From there I would go to a 3mm or 1/8" Yeti from them. These also have variable flute design but no chip breaker. Recommended feed and speed on these for mild steel is 800 SFM and .008 on the 3/8" tool and about .002 for the 1/8". I would probably start with a Yeti for both though. They tend to not chatter in thin stuff pretty well. They last a long time at these speeds. I would expect 50 complete parts per tool at least from what you've shown here. 3/8" tool runs about $40 and the 1/8" is about $20.


Interesting. I didn't think of variable geometry tooling. I'll look into it. At those prices getting 50 parts per tool would be just fine in my book.

Thanks.
 

martin_05

Hot Rolled
Joined
Mar 11, 2009
Location
Valencia, CA, USA
I did a bunch of 2x2x.120 tubes on a VMC because they were part of a precision table and the weld shop wanted all weld prep and fits perfect.

I did not have any small inside radius to deal with and after playing around some I threw an old cobalt corncob in and it chewed threw that tube WAY faster than I could reliably run it with carbide. The edges looked pretty good, had to play with size a bit to hit my numbers with a rougher, but it worked great.

That said, that part is an obvious punch job. 20 ton OBI will dominate that part. EDM shop could cut the tool hard and you could be running that in a day. I would guess a minute per part if you're cutting one slot per hit.

I'll look into this. I need to make a few parts for prototyping, followed by a mid-quantity run and then a large quantity. I can't go for custom tooling until our client commits to the larger project, otherwise the punch would be, as you said, the obvious path.

I am still hoping I can convince one of the laser guys that this job is worth their while.

Frankly, I know I can get these parts made in China and brought in and still hit my numbers. It's just that this makes me sick to my stomach. Just not interested.
 

Garwood

Diamond
Joined
Oct 10, 2009
Location
Oregon
Do you have a big, slow spindle brickshithouse VMC back in the corner maybe?

Build an expanding hard mandrel mounted to a beefy 4th for the tube to slip over. Probably want an outboard support to one-op these. Mill all the slots with a 1/2" corncob. Change tools to a big square punch in a toolholder or just mount the punch to the headstock behind the spindle so a different Y position uses that tool (no toolchange). Now knock the corners out with the punch in the VMC. Make sure the slugs are cleared out.
 

Vancbiker

Diamond
Joined
Jan 5, 2014
Location
Vancouver, WA. USA
Place I retired from cut parts like that on a regular flatbed laser. Cut a simple bend tab fixture on the table. Bend up the tabs and screw on some spring pushers. 10 or so parts at a load. Cut one side on all of them then machine stop and rotate the parts. Cut the next face. Repeat until 4 faces cut. There was some dross blown to the opposite side inner wall. When that was an issue the operator would just spray the inside of the tube with welders anti-spatter compound.
 

DJ2

Aluminum
Joined
Feb 12, 2007
Location
Ontario, Canada
A Mennonite fabricator with an ironworker in rural Ontario would make that up in an afternoon. Look for a guy that does automotive shipping racks.
 








 
Top