What's new
What's new

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

memphisjed

Stainless
Joined
Jan 21, 2019
Location
Memphis
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.

:D

Brass is just yuck. Banks and casinos are its native habitat. Bronze is a real metal.
 

babiels

Plastic
Joined
Apr 29, 2018
Ok, so I cast some new stock and switched my endmill for a 6mm HSS two flute cutter that sticks out 20mm. Slowed down speed to 2500 rpm (48m/min) and feeds accordingly with 0.05mm feed per tooth and 5% stepover. I changed my toolpaths to 3D Adaptive and followed up with 2D contours without a ramp. Program time jumped from 30 mins to 3.5 hours but I'm all for it if it gives me a good looking part.

I'm happy with the chips I'm getting and the surface finish is much better than before (thanks). Much less chatter too. However I'm still seeing the cutter get hot enough to steam/smoke up the WD40 immediately when I spray it on during the bigger cuts. I'm seeing a little smoke on those cuts even before I spray too. Video is below. Is this kind of temperature normal for milling brass/bronze or am I killing this cutter too? I've read quite a few articles saying that I should be milling completely dry, but presumably without the WD40 the endmill would get smoking hot and go blunt?

https://youtu.be/I-_P4qw3HXs

Also @Evenglischatiest - I am going to give your advice a go too, once I receive my new short gauge collet chuck I've ordered.

Thanks
 

mhajicek

Titanium
Joined
May 11, 2017
Location
Minneapolis, MN, USA
You can hear that spindle bogging down to about half RPM in every pass. As a guess, if it were me stuck with that machine, I'd try a 3mm 3 flute carbide endmill with non-ferrous geometry, and crank up the RPM. Or maybe a small highfeed cutter; those tolerate lack of rigidity well.

You're really handicapped by that machine. It's like fighting with one hand tied behind your back, a huge weight tied to the other, and your feet shackled. That thing is low end for a hobby grade machine.

Hmm; thinking on that, maybe you should replace the spindle. You can get a decent 18K RPM trim router for not very much, and just bolt it on. Dewalt makes a decent one.
 

neilho

Titanium
Joined
Mar 23, 2006
Location
Vershire, Vermont
Slower everything (like half) and clear the chips somehow. There's a lot of chip recutting going on. Compressed air blast is my favorite, even if you have to stand over it. Cools the cutter, too.

Best to start slow and work up than the other way. Less chance of damage.
 

implmex

Titanium
Joined
Jun 23, 2002
Location
Vancouver BC Canada
Hi again babiels:
Did you know that the machinability rating of silicon bronze is around 60% of 1212 (the steel against which other alloys are compared in standard machinability ratings).

You can see how your machine is struggling to cut this fairly tough alloy.
I recommend you try a bit of 6061 aluminum first; it's much easier to cut.
The toughness of bronze makes it hard to force a cutter into it so when your machine is not very rigid, the cutter will deflect rather than penetrating into the material properly.

Get your feet wet, learn how to cut aluminum, and then step up to bronze.

Cheers

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

plastikdreams

Diamond
Joined
May 31, 2011
Location
upstate nj
Hi again babiels:
Did you know that the machinability rating of silicon bronze is around 60% of 1212 (the steel against which other alloys are compared in standard machinability ratings).

You can see how your machine is struggling to cut this fairly tough alloy.
I recommend you try a bit of 6061 aluminum first; it's much easier to cut.
The toughness of bronze makes it hard to force a cutter into it so when your machine is not very rigid, the cutter will deflect rather than penetrating into the material properly.

Get your feet wet, learn how to cut aluminum, and then step up to bronze.

Cheers

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

Ehhh...probably better off starting with tooling board.
 

vmipacman

Cast Iron
Joined
Nov 21, 2014
Location
Virginia, USA
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 :)

Zamak3 is a low melting temp alloy (900~ deg). Strong and machines really nice. Ticks the reusablility box.
 

memphisjed

Stainless
Joined
Jan 21, 2019
Location
Memphis
I think it is in the free fusion, change your no engagement speed to a high value. It is in the last tab (linking)on your 3d adaptive settings.
 

implmex

Titanium
Joined
Jun 23, 2002
Location
Vancouver BC Canada
Hi memphisjed:
I don't think his machine can do much over the feedrate you see in the video.
I don't know but I suspect it's an open loop stepper driven machine.

Other videos exist on Youtube showing it in "action"
Kinda like a tortoise...I recall particularly a tool change video.
"Stately" is a kind way to describe it.

This machine is never going to be a rocketship, but if the OP learns how to squeeze maximum advantage out of it, it can still be a great hobby machine; and if he's having fun and learning cool new things, it's as good as it needs to be.

BTW, it's about 170 kilos total weight and the spindle taper is ISO 30.
He has 1/2 horsepower at the spindle.
It has ballscrews and what looks like dovetails.
The literature describes it as a "training mill".

Cheers

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

memphisjed

Stainless
Joined
Jan 21, 2019
Location
Memphis
I get the mill is small Marcus. Just passing on the untrained machinist tips I have found so far.
My mill is dove tail and steppers... anyone with class enough to go to bronze instead of ‘shiney wood’ or brass (devils metal) is already way ahead of most in my book. Op finish on second videos looks better than Titans already. The milling machine might be small but it is not too ragged.

Wd 40 is expensive, simple green makes a decent coolant/tap fluid that is less dollars and lung cells. Be sure to wd your table after playing or rust can happen. Air blast is annoying to listen to but will do more to improve finish and tool life than squirt bottle. Hss mills cost more than carbide in many cases, provide a better finish than carbide in bronze. Bronze is a old soul metal and likes old school tooling. Radius end mill is better than square.
 

implmex

Titanium
Joined
Jun 23, 2002
Location
Vancouver BC Canada
Hi memphisjed:
You wrote:
"I get the mill is small Marcus."
I'm not running the Denford mill down, I'm describing its limitations so they can be worked around...a process that's necessary even with a half million dollar Hermle if you want to get the best out of it that it's capable of.

These little hobby mills need much closer attention to the basics than a bigger more rigid machine does, but too many beginners get all of their cues from watching guys with solid industrial iron ripping through material with ease on YouTube, and think THEIR toy should be able to do it too.

As you probably well know by now, it doesn't work that way, but a NOOB has no experience based points of reference from which to decide what to do...he's a NOOB after all.

So I try to evaluate what I see in front of me and make constructive and helpful comments, not to slag the toy simply because it's not that half million dollar toy.

YouTube is a real mixed blessing in this domain...I see lots of really bad practice and lots of pontificating by obvious "Know Nothing Egos", and the unlucky who are trying to learn this stuff but get caught in the web as their sole instructor, see bad or inappropriate practices and try to imitate with poor or dangerous outcomes as a result.

It's the modern reality...those who are motivated eventually learn what they can get away with and learn what is "YouTube Bullshit" and what's worth adopting.

In any event, if the OP learns the limitations of his machine, there's no reason he can't learn to do impressive work with it.

Cheers

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

plastikdreams

Diamond
Joined
May 31, 2011
Location
upstate nj
Rewatching the videos, you can see how much the spindle slows and recovers. I really think a ramped tool path would be best. On mastercam I can change between angle and depth as my input. If I were you I'd program maybe a .02 depth per pass on the ramp if you can.

But man does that thing shimmy and shake.
 

babiels

Plastic
Joined
Apr 29, 2018
It’s taken me a little while to get here, but finally applied some of the advice you shared. I changed to a shorter Chuck, and made a DIY fogbuster, changed to adaptive toolpaths with 5% stepover at 2000 rpm. Reduced cutter size to 6mm two flute (painfully slow), then upped it to 8mm three flute but had my best results here with 8mm four flute. I’m sure I’m still making a ton of mistakes that will explain my tools getting dulled quickly, but overheating is not so obvious a problem now. Need to find some of those short endmills. I have a high pitch noise intermittently on the adaptive toolpaths, and I think my contours toolpaths are still aggressive, but I’ll figure those out next. Thanks again guys for your help!

The video:
https://youtu.be/0OLqDkQOHI4
 

implmex

Titanium
Joined
Jun 23, 2002
Location
Vancouver BC Canada
Hi babiels:
OK, that looks and sounds a whole lot less scary, so I think you're getting much closer to the realistic performance envelope of your mill.

You can start to jack up either the stepover or the feedrate until it gets wobbly looking, and then you will know how hard you can push in this material.
Back off a bit from there and you will be in your sweet spot.

With respect to why your cutters are still getting dull too quickly for your taste. there are a number of potential causes:
1) If you sand cast the blank, there will be sand in the casting and it will beat the shit out of your cutters.
2) When you recut the chips it will have a similar effect.
3) If the mill is still deflecting rather than forcing the cutting edges of the cutter to bite in and shear a chip, the cutter will start rubbing.
A rubbing cutter will hurt you in two ways:
a) The cutting edges are loaded in shear instead of compression, so the carbide cutting edges begin to crumble.
b) The rubbing can work harden certain materials to the point you can't force a cutting edge into them without a huge amount of force...I don't know if silicon bronze is one of those, but I would not be surprised.

But what I see in your latest video is so much better than what I saw in your first video, that I'm greatly encouraged.

Cheers

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








 
Top