How would you program milling this bronze part in Fusion 360?

[babiels]

Hi, I'm a CNC machining newbie and would appreciate anyone casting their experienced eyes over this part I'm working on in fusion 360.

I have a 1HP Denford Novamill running on Mach3. Max spindle speed is about 4500 rpm. I have cast some stock in silicon bronze which I am now milling down to the final form using a 10mm 4 flute plain endmill (no tool changes). I've tried milling this part twice and would appreciate some advice before attempt number 3.

First attempt: I went in aggressive using my max spindle speed and FSWizard's recommendation for feeds, however I really have little idea about depth of cut/width of cut nor really how to go about this in Fusion so I opted for 2D contour toolpaths all ramped at 2 degrees and maximum ramp step of 20mm. A first it seemed to be doing great but quickly got hot and owing to smoke, noise and the motor stalling I aborted.

Second attempt: I went down to 1370 rpm @ 254mm/min (43m/min surface speed) and reduced the ramp angle to 1 degree and maximum ramp step of 1.5mm. This kept the heat down for the most part, but made long strings of swarf rather than chips and ended up heating up anyway and by mid way through the program I was spraying WD-40 on the end mill and watching it quickly steam off (see here: https://youtu.be/9Q3zvWefCBA). Additionally I could hear/see the spindle speed diminishing considerably whenever it took anything that looked like a deep cut, and I had to manually increase the spindle speed using the potentiometer on my control unit (so basically managing the speed by ear (I know this is probably awful behaviour but I wanted to get through the program at least once). You can see this in action here: https://youtu.be/j6pDb9zuDF4


Third attempt questions:

• Should I switch to a 10mm carbide endmill? I see that FSWizard advises speeding up the spindle revs and feeds considerably (3500 rpm, 916 mm/min, 109m/min surface speed), which kind of scares me.
• I have watched about a million hours of milling videos on YouTube but still don't know what sort of toolpaths I should be using. Ramping made sense to me because it seems gradual and linear, but should I be using adaptive toolpaths, or something else? This is a Fusion simulation of my toolpaths: https://youtu.be/HJ_Hube_ENo

Thanks a lot!

 

[alphonso]

First, you don't have enough horses.
Second, try using 5mm endmill. Maybe you'll have enough power to run it.
Third, about the worst tool paths I've ever seen.

 

[babiels]

On second look the spindle is actually 1/2 HP.

Here is someone else milling brass with the same mill (Denford Novamill), which looks pretty decent:
Denford Novamill Fun - YouTube

 

[Larry Dickman]

the chips on the floor are worth more than the machine.

 

[Mtndew]

Wow those videos were painful to watch.
You need a smaller cutter because your toy doesn't have any balls at all.
That chatter and vibration is also terrible.

 

[couch]

How close can you get the spindle to the table?

I’d go way smaller on tool diameter and as short as possible stick out. Shorter flutes and deeper in the collet. I’d probably keep tool diameter to .250 max, maybe even .187 max.

You should be able to rough that entire part with a single 3D Adaptive, keep the radial engagement way down, start at 5%. Turn off Cut Both Ways. Can’t tell if it’s on here and cutting or those are just the return moves since the toolpath trail isn’t shown.

 

[dandrummerman21]

You'd also have a better time if you were cutting brass instead of bronze.

 

[implmex]

Ouch, that kinda hurt to watch:
I agree with what everyone has said about the horrible way this is going; you need a radical rethink about how hard you can push this mill.
First, I fully agree about the cutter stickout...that cutter needs to be as close to the front spindle bearing as you can get it.
Second, the cutter is way too big for the horse power that machine has.
Third, the feedrate is way way too aggressive for that little machine...if you mill it with an adaptive toolpath using a 4 mm endmill and a 2% stepover with maybe a 0.05 mm chipload you'll be a bit closer to what that little toy machine can take.
Fourth, silicon bronze is too much for this machine...360 brass would be better unless you really baby it.
Fifth, you could benefit from some kind of coolant...maybe WD40 if it's available where you live.
Sixth, inspect all your cutters and toss all the ones with chipped teeth...even if they were brand new before you started, they will be utterly trashed now.
Seventh, try to find a better toolholding solution than that collet chuck...it sticks out way too far...the closer you can get the tip of the cutter to the front spindle bearing, the better off you will be.
Eighth, buy stub flute endmills instead of standard length ones...you will do better.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

 

[babiels]

Thanks a lot everyone, that's really helpful. I'll try to apply everything you've said to attempt number 3.

Marcus and Couch - sorry to be dense but you mention radial engagement, stepover and chipload on that adaptive toolpath. Fusion refers to these differently so I want to check:


Radial Engagement = Minimum Cutting Radius?
Stepover = Optimal Load?
Feed per tooth = chipload?

The fusion settings screen has these fields:


Also you say 2% stepover and 5% radial engagement; is that percentage of the cutter radius? I.e. 2% stepover would be 0.12mm and 5% radial engagement would be .3mm?

Thanks again!

 

[couch]

Thanks a lot everyone, that's really helpful. I'll try to apply everything you've said to attempt number 3.

Marcus and Couch - sorry to be dense but you mention radial engagement, stepover and chipload on that adaptive toolpath. Fusion refers to these differently so I want to check:


Radial Engagement = Minimum Cutting Radius?
Stepover = Optimal Load?
Feed per tooth = chipload?

The fusion settings screen has these fields:
View attachment 341087

Also you say 2% stepover and 5% radial engagement; is that percentage of the cutter radius? I.e. 2% stepover would be 0.12mm and 5% radial engagement would be .3mm?

Thanks again!

Radial Engagement will be your “Optimal Load” in Fusion, same as step over (vs step down / axial engagement). Always forget they labeled it that, even though I use it every day. If you hover over the fields you’ll see a description, usually with some images, explaining each field.

 

[implmex]

Hi again babiels:
Sadly I can't read the screenshot you took...it's too small for my old eyes.
But I'll try to give you something useful anyway.

Radial engagement and stepover mean the same thing...they are the amount the cutter takes sideways with each pass, and they're commonly expressed as a percentage of the cutter diameter.

High speed machining (HSM) toolpaths (which is the strategy we are encouraging you to adopt) are different from traditional milling in that you try to go very deep with your cuts to engage the entire length of the flutes, but you whisker only a small amount off sideways with each pass...commonly less than 5% of the cutter diameter so you nibble out your part with gazillions of tiny whiskering cuts but using the whole length of the endmill flutes whenever possible.

The benefit is that you distribute the wear over the entire cutter flute length so it lasts longer, you load the machine far less and far more evenly, and it is an efficient way to remove material so it's often very fast and doesn't introduce a lot of heat or stress into the part, so it warps less when you unclamp it.

Also, because so little of the side of the cutter is engaged per cut, you can run the hell out of it, and so long as the control is good enough to start and stop the toolpath where it intends, all goes very smoothly.
When you look at Youtube videos of guys whistling along at hundreds of inches per minute, that's how they're doing it without blowing things up.

Flimsy, low horsepower machines benefit from a strategy like this because they never see much load...one of the features of HSM toolpaths is that they slide the cutter into each cut with a nice entry radius and without an abrupt wallop, so the cutter doesn't see shock loads and the sideways radial engagement never goes above the value that you set.
That is kind to the cutter, to the workpiece, and to the machine.

Sadly for your machine, you will not have the ability to crank up either the spindle speed or the "No Load" feedrate...the rate at which the cutter repositions itself for the next cutting pass, and those two things make the process go much faster as you can imagine.

But you have to dance with the girl you got, and the benefits of HSM toolpaths on otherwise inadequate machines is still very worthwhile to capture, so I encourage you to learn how to program them in Fusion 360 and use them often.

Your programs will be HUGE but if your computer can handle them and drip feed them to the control, you need not care.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

 

[apoet]

Radial Engagement = Minimum Cutting Radius?

Minimum cutting radius defines how sharp an internal radius the cutter will take at a corner. Larger minimum radius will be easier on your tools and machine but will leave stock to clean up with follow up operations.

 

[plastikdreams]

Douse it in gasoline and light a match...for real life

Edit: I mean petrol

 

[implmex]

Hi plastikdreams:
Am I guessing correctly, that you are unimpressed with the videos?

Yeah, the machine leaves a lot to be desired, and I certainly couldn't find a use for something like that in my own shop. but it's all he has.
So if he can get it to work even a little better than what's happening now, he can happily noodle on his projects and have some fun.
I don't think he's going to run away with your customer base or mine anytime soon, so I'm not too worried about fending off competition.

I started my shop with a little manual mill that was not much better than that one is...of course I got rid of it again pretty quickly as soon as I could spring for something better.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

 

[plastikdreams]

Hi plastikdreams:
Am I guessing correctly, that you are unimpressed with the videos?

Yeah, the machine leaves a lot to be desired, and I certainly couldn't find a use for something like that in my own shop. but it's all he has.
So if he can get it to work even a little better than what's happening now, he can happily noodle on his projects and have some fun.
I don't think he's going to run away with your customer base or mine anytime soon, so I'm not too worried about fending off competition.

I started my shop with a little manual mill that was not much better than that one is...of course I got rid of it again pretty quickly as soon as I could spring for something better.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

What up Marcus! Heh they leave something to be desired. But at least it's not a mini mill.

Trial and error...usually more error lol

 

[Evenglischatiest]

In the longer of your two cutting videos, you were doing okay until the 16 second mark. That's when you stopped ramping, and pushed straight into the corner. You suddenly went from a light ramp, to the heaviest possible cut you can take at that depth. You dove in to the corner, cutting with the entire width of the tool. That's called full slotting, and it's what the adaptive toolpaths were created to avoid. The horsepower requirement instantly went up by several hundred percent, which is why you had to manually adjust the spindle speed. Your machine didn't have enough torque to maintain 1370 rpm at that point. That potentiometer reduces torque almost linearly with rpm. Since horsepower is torque x rpm, You have roughly 1/4 of your max hp at 2250 rpm. That's why turning it up helped. But by that point, the endmill was already destroyed. When you get a steel endmill that hot, it gets soft, and dulls instantly. There really isn't any fix, except a new endmill.

The toolpath suggestions listed above are correct, but they may be more advanced than you're ready for at the moment. Assuming your goal for today is just to get the part done, I'd go with a very different strategy. Reduce the bearing to part distance as much as possible, as mentioned above. Replace the steel endmill with the same thing in carbide, and run exactly the same program as your second try. But increase the rpm to about 2500, and cut all your feed rates by 70%. Alternate between oiling it, and blowing the chips off. The tool should stay wet at all times, surrounded by as few chips as possible.

This isn't how any of us on here would make that part in our own shops. But we have far superior machines, and years of experience. Considering what you have to work with, I think you're doing pretty good so far. Your program, exactly as it is, would work fine in aluminum. Silicon bronze is just a tougher material. Regardless if how you do it, lighter cuts are the answer. Slowing down the feed rate will take a lot longer, but it gets you there with the least amount of work.

 

[mhajicek]

HSMAdvisor will tell you the theoretical horsepower requirements for a cut:

Advanced CNC Speed And Feed Machinist Calculator - HSMAdvisor

 

[babiels]

Wow thank you so much everyone for taking the time to help me - I really appreciate it!

Just to say that the choice of silicon bronze is because I can cast it easily and avoid buying brass billet which is so expensive - especially for a beginner. And any mistakes can be melted back down. Potentially there is another alloy out there that ticks both boxes better, or I should just melt free machining brass, but that’s a topic for another day.

Again, thank you

 

[memphisjed]

smaller end mill like everyone said. Slow the speed way down. Go to hss ranges of speed (80 fpm) even with carbide and si-bronze is silk on the mill. Depending on how small your end mill is you might need to reduce flute count, without air or constant coolant you will get gummed up flutes.

Cutting Speeds - LittleMachineShop.com

 

[neilho]

Wow thank you so much everyone for taking the time to help me - I really appreciate it!

Just to say that the choice of silicon bronze is because I can cast it easily and avoid buying brass billet which is so expensive - especially for a beginner. And any mistakes can be melted back down. Potentially there is another alloy out there that ticks both boxes better, or I should just melt free machining brass, but that’s a topic for another day.

A topic for another day....

Silicon bronze is a good choice for remelting, prob the best. Melting brass involves clouds of zinc, which would have to be replaced when remelting. BTDT, yuk.

Folks here at PM would generally just buy a chunk of brass and have at it. When in pro mode, time is what we have to sell and we try to maximize our margins. Different scene in your case.

When chatter happens or smoke starts rising on a one-off, slowing speeds and feeds improves HSS end mill life considerably.

Shortening the cutter "stick out" is huge for reducing chatter. Stiffness is a geometric function, not linear, so as has been said before, reducing the cutter end to spindle bearing distance, in combination with slowing rpm and feeds will eliminate chatter.

Hang in there, ignore the arsonists