Time study to 3D surface a part

[vmipacman]

For those who have real world experience with 3D contouring...
I was asked to estimate machine time for a plate with kinda a rolling hill surface. The plate in question is 18" x 30" x 5" tall max and 2.5" tall at the min. So picture a rect plate with the center pulled up and the slide sloping off. The part approximates a small section of the exterior curve of a large pressure vessel (done shaped). Just that surface. Just picture a piece of paper flat on your desk and push the ends together slightly. No other features, small areas or gotchas.

The plate is 304 SS.
The material needing to be removed is approx 500in^3.
The surface should be "good" but not polished necessarily.
The mill is pretty stout, CAT50. Lots of torque but rpm limited to about 4K.
I used HSMWorks to do some quick tool path calcs.

For roughing I came up with a pretty conservative estimate of 6.5 hrs using a 3" APKT facemill. With a high feed 4" insert cutter, computer says I could do it in less than half that time! Roughing to .02" of the surface.

For finishing I used a 1-5/8 insert ball mill. Taking .03" steppover passes at ~30 ipm. That gives a finishing time of 9-10 hrs. And in my (limited) experience that will yield a pretty smooth finish, maybe with some scuffing at the ball mill center. With a few hrs of handwork you could really finish it out nice.

I estimated that in 20 something machine hrs you could have it done, plus a few hrs for some easy hand work (if needed).

I heard another shop that does foundry patterns pretty regularly estimated literally 100's of hrs of machine time!? They have newer equipment, higher rpm's and feedrates.

What am I missing in my approach?? I'm sure i am under estimating some, but I either don't understand the 3d strategies at all or the other shop is over complicating.

 

[Bobw]

What am I missing in my approach??

Could be a 1000 things. They see something that you don't.. This customer is a pain in the
ass so they are getting quoted the "You're a f'n PIA up-charge".

Maybe they aren't as good at what they do as you think they are. Maybe they are and they
know it, and charge accordingly.

Millions of reasons that prices can fluctuate all over the map.

 

[mmurray70]

This customer is a pain in the
ass so they are getting quoted the "You're a f'n PIA up-charge".

Any customer bringing a block of stainless that big needing that much material removed, and a 3d surface would certainly get a pain in the ass charge at my shop.

If your planning on hogging that out with APKT inserts, 6.5 hrs could be closer to time spent on changing inserts...

 

[sirAIG]

Size of material vs risk of problems, warping, scrap, and time. For how many parts?

Maybe that's why the other guys are so expensive [emoji51]

Sent from my SM-G955U using Tapatalk

 

[Rstewart]

Your finishing pass with that inserted BN at the limited RPM you have will be the struggle. You'll most likely go through lots of inserts on roughing and finishing. Add at least 50% more than what you think.
Hope it's not shit 304...

 

[garyhlucas]

Tilt it. Don’t cut with the center of a ball mill at zero fpm. Better finish, faster cutting.

 

[Milland]

Tilt it. Don’t cut with the center of a ball mill at zero fpm. Better finish, faster cutting.

If it's a dome-like shape, tilting won't help - some sections will still be close to planer with X-Y, unless you get pretty steep, and that brings its own headaches.

Rather than an insert BEM, I'd use a bull-nose cutter, either inserted or large diameter solid, with a big corner radius. The second is what I did when I was making a roughly similar size/type of part (a radar dish analogue), although it was Al rather than stainless. I used a 1" x .190R carbide tool with eight flutes, worked a treat as our Brit friends might say.

 

[Mike1974]

I can't say I've tried to picture your net part shape... but Dapra ball end mill cutters (inserted) used to be the bees knees for us in tool steels. Run wide open for roughing, 250 ipm, most rpm you have.... solid carbide for finishing, likely need 2 or 3 if you need a good finish...

 

[Hardplates]

I'm sure someone will disagree but I wouldn't use APKT style inserts for anything other than torturing someone. It's been years since I played with them but I could never get good life out of them.

IMO high feed cutters are where its at when it comes to working with steel, stainless and exotics. By design the insert is really durable and the small stepdown makes for very small cusps from roughing 3d work. With my work this usually allows me to skip semi finishing and go straight from roughing with a high feed mill to finishing with a ball or bull.

 

[Evenglischatiest]

I second the feed milling. If for some reason you're stuck with APKT inserts, use the biggest radius/champer you can find.

I heard another shop that does foundry patterns pretty regularly estimated literally 100's of hrs of machine time!? They have newer equipment, higher rpm's and feedrates.

What am I missing in my approach?? I'm sure i am under estimating some, but I either don't understand the 3d strategies at all or the other shop is over complicating.

Have you seen the actual drawings they're quoting? Depending on material, geometry, and tolerances, surfacing can EASILY go in to the hundreds of hours. You may be looking at a much simpler part than what they normally do.

Or, that other shop might just not be very fast. Just because they do it every day, doesn't necessarily mean they're any good at it. It's shocking how much inefficiency you can find in some shops.

 

[vmipacman]

Thanks for all the suggestions. All well taken. I only did a quick look to give them a rough idea of machine hrs. They just wanted to know if it was a 10k or 100k feature. If it materializes, tilting will be an option as is high feed, as is more flutes for finishing.
I had just used the APKT tool so I just plugged in the numbers I had used, knowing a high feed cutter would put it to shame and better suited. Same with the insert ball vs 6flute ball.
I was even worried I was overestimating too much on my budgetary machine times. Only to find others ballparked 10x the hrs I told them. That’s why I was baffled.
So let’s just say roughing out 500in^3 stainless, just spindle time with the tool of your choice. How fast could you do it on a normal day without redlining your machines?

 

[ChipSplitter]

So let’s just say roughing out 500in^3 stainless, just spindle time with the tool of your choice. How fast could you do it on a normal day without redlining your machines?

Assuming 304 SS, you should be able to get about 0.70 in.[SUP]3 [/SUP]/ min. / hp with indexable tools. Solid carbide will be a bit better.

You have a 50 taper with, let's say 30 hp continuous (real horsepower, not Haaspower). At 90% spindle load, it should take about 20-30 minutes.

Of course that's all relative to hp/torque curve, tool diameter, insert geometry, and moon phase.......

 

[Rick Finsta]

With my favorite SECO 2" inserted face mill I'd rough at around 14 cubic inches a minute really givin'er, which is the most my CAT40 30hp machine can actually do at stainless SFM at that diameter. I would likely cut that in half to save inserts. I can only get about 5CIM with my 1" high feed for reference. Semi finish with a SECO/Niagara solid carbide high feed and then finish with a 3 flute ball. Both solid carbide tools I'd use 1/2" so if I run through a few it is not too expensive.

So figure a few hours for programming, setup, and roughing, another few hours for semi-finishing, and then around 6-7 hours to finish with a 0.005" stepover which would give a really nice surface finish. I would likely go to around 0.007-0.008" to cut the time down so I could finish the whole thing in a 12 hour day. $180 in inserts, and maybe $250-300 in solid carbide on tooling?

I'd be at around $1350-1500 if I was hungry for work, or $1850-2000 if I really didn't have a day to do it. I'll work a Sunday for $500.

 

[vmipacman]

With my favorite SECO 2" inserted face mill I'd rough at around 14 cubic inches a minute really givin'er, which is the most my CAT40 30hp machine can actually do at stainless SFM at that diameter. I would likely cut that in half to save inserts. I can only get about 5CIM with my 1" high feed for reference. Semi finish with a SECO/Niagara solid carbide high feed and then finish with a 3 flute ball. Both solid carbide tools I'd use 1/2" so if I run through a few it is not too expensive.

So figure a few hours for programming, setup, and roughing, another few hours for semi-finishing, and then around 6-7 hours to finish with a 0.005" stepover which would give a really nice surface finish. I would likely go to around 0.007-0.008" to cut the time down so I could finish the whole thing in a 12 hour day. $180 in inserts, and maybe $250-300 in solid carbide on tooling?

I'd be at around $1350-1500 if I was hungry for work, or $1850-2000 if I really didn't have a day to do it. I'll work a Sunday for $500.

Thank you for the great info and experience. This is much closer to my reasoning. Sounds like about 14-hrs campared to my conservative 20, as opposed to the couple hundred that others locally had suggested. This makes me feel much more confident that i wasn't completely out to lunch.

 

[Hardplates]

Don't forget about programing time. Depending on what the desired end result is, its not as simple as just letting the software surface the entire part. This is especially true of SS and exotics where the finishing tool has little tolerance for plunging and center cutting. This often requires sectioning off surfaces and using a host of different tool paths for different areas.

Another point I didn't see brought up is just how fast can you finish surface while holding tolerance and acceptable surface finish? Being a CAT50 4000RPM machine I'm going to guess you can't finish very fast. I wouldn't be shocked if you end up down in the single digit feed rates.

You may want to play around on a piece of scrap to get a better feel for 3D work.

 

[vmipacman]

Don't forget about programing time. Depending on what the desired end result is, its not as simple as just letting the software surface the entire part. This is especially true of SS and exotics where the finishing tool has little tolerance for plunging and center cutting. This often requires sectioning off surfaces and using a host of different tool paths for different areas.

Another point I didn't see brought up is just how fast can you finish surface while holding tolerance and acceptable surface finish? Being a CAT50 4000RPM machine I'm going to guess you can't finish very fast. I wouldn't be shocked if you end up down in the single digit feed rates.

You may want to play around on a piece of scrap to get a better feel for 3D work.

Well yes and no. My question was about machine time only, and really more looking for others experiences with large (but simple) 3d surfacing. and the tolerances were covered as just being representative of a curved surface in the field. I feel comfortable with my swag. I will run a small test part for approval if it goes forward, and Id expect to use a large enough ball with as many flutes as I can find so the rpm isn't as big a limiting factor.
Thanks All

 

[Joe Miranda]

For those who have real world experience with 3D contouring...
I was asked to estimate machine time for a plate with kinda a rolling hill surface. The plate in question is 18" x 30" x 5" tall max and 2.5" tall at the min. So picture a rect plate with the center pulled up and the slide sloping off. The part approximates a small section of the exterior curve of a large pressure vessel (done shaped). Just that surface. Just picture a piece of paper flat on your desk and push the ends together slightly. No other features, small areas or gotchas.

The plate is 304 SS.
The material needing to be removed is approx 500in^3.
The surface should be "good" but not polished necessarily.
The mill is pretty stout, CAT50. Lots of torque but rpm limited to about 4K.
I used HSMWorks to do some quick tool path calcs.

For roughing I came up with a pretty conservative estimate of 6.5 hrs using a 3" APKT facemill. With a high feed 4" insert cutter, computer says I could do it in less than half that time! Roughing to .02" of the surface.

For finishing I used a 1-5/8 insert ball mill. Taking .03" steppover passes at ~30 ipm. That gives a finishing time of 9-10 hrs. And in my (limited) experience that will yield a pretty smooth finish, maybe with some scuffing at the ball mill center. With a few hrs of handwork you could really finish it out nice.

I estimated that in 20 something machine hrs you could have it done, plus a few hrs for some easy hand work (if needed).

I heard another shop that does foundry patterns pretty regularly estimated literally 100's of hrs of machine time!? They have newer equipment, higher rpm's and feedrates.

What am I missing in my approach?? I'm sure i am under estimating some, but I either don't understand the 3d strategies at all or the other shop is over complicating.

We do a lot of 3D work. If you are only doing one side of a plate, and the other side is flat, that is a pretty straightforward task and I think you're in the ballpark at 20hrs (my guesstimate would be closer to 25).

As far as a foundry quoting 100's of hours, not sure what they are seeing that you are not. You're sure the other side is flat and not contoured? If it is contoured as well, and features have to be held relative to each other from top and bottom, that will complicate things exponentially and can easily lead to 100's of hours.

We are in the middle of some complex 3D work that is two setups and requires about 80 hours of machining time per piece. We are starting with a block of ductile iron that weighs 120lbs and end up with a part that weighs 20. And ductile is pretty stable compared to SS. Be careful about warping. Make sure you take that into your consideration.

 

[Hardplates]

I was referring more to how quickly you can dump code on the machine before it gets jerky and or just won't move at the commanded feed rate. Doesn't matter if you program 100 IPM if the machine can only go through the code at 8 IPM. You can see where the projected cut time would be off by an more than an order of magnitude from the actual time.

You don't mention the machine, control and if it has any look ahead. Yes the spindle RPM can be displaced by using a larger cutter but that does nothing for the control itself and speed.

Just trying to help you with any unforeseen issues as I gather from your post you haven't done much 3D work. That is almost exclusively all I do and I'm able to do it on some pretty old machines.

 

[vmipacman]

I was referring more to how quickly you can dump code on the machine before it gets jerky and or just won't move at the commanded feed rate. Doesn't matter if you program 100 IPM if the machine can only go through the code at 8 IPM. You can see where the projected cut time would be off by an more than an order of magnitude from the actual time.

You don't mention the machine, control and if it has any look ahead. Yes the spindle RPM can be displaced by using a larger cutter but that does nothing for the control itself and speed.

Just trying to help you with any unforeseen issues as I gather from your post you haven't done much 3D work. That is almost exclusively all I do and I'm able to do it on some pretty old machines.

Yes thanks. Yeah I’m aware of control limitations and processing speed but with this spindle rpm is really my limiting factor. At least in this instance.