What's new
What's new

FSWizard / hsmadvisor speed and feed totally different (and wrong) compared to YG1 recommendation.

poly

Plastic
Joined
Oct 31, 2022
I bought a few YG1 end mills. 1,2 and 3 flute and a 3 flute rougher for cutting aluminum. All 4mm apart from the rougher. I am a little confused that the YG1 recommended cutting conditions for the 1 flute (E5E47 series, 4mm) 15000 rpm, 1800 mm/min feed 190 m/min Vc and 0.120 mm/tooth. If I run these speeds on my machining centre, slotting 1.6mm think aluminium, full depth of cut, it cuts perfectly. The edge quality is great and chips clear well. FSWizard however suggests I run the bit 15000 rpm, 519 mm/min feed 0.034 mm / tooth. This results in the aluminum instantly melting and the end mill having aluminum welded to it pretty enthusiastically.

The interesting thing for me is that the 2 flute 45 helix E5521 4mm has YG1 recommended cutting conditions of 10000 rpm 1100 mm/min feed 0.055 mm / tooth. Slower feed (but also slower RPM) than the 1 flute. The 1 flute doc also says it slots at 1.5D where as the 2 slots at 0.5D.

Is HSMAdvisor / FSWizard wrong for aluminum specific end mills? Am I doing something stupid using it? If I attempt to run any end mills at the numbers it recommends they melt and in my wisdom I didn't look at the YG1 numbers first... so a 3 flute and 2 flute got aluminum welded to them. Is the 1 flute the best way to slot 1.6 mm thick aluminum? I'm cutting parts for bending in my press brake. These YG1 alu powers are basically magic compared to what I've used before. I haven't tried the rougher yet. I'm starting to think it won't be worth tool changing some of areas as the 1 flute is so fast.
 
Hi,

HSMAdvisor and FSWizard calculators assume you are using coolant in aluminum. Also they give results averaged across multiple tool manufacturers.

In your case the manufacturer designed the tool to work best at that specific feed and that's where it should be run at to get good results when running aluminum dry.
 
I bought a few YG1 end mills. 1,2 and 3 flute and a 3 flute rougher for cutting aluminum. All 4mm apart from the rougher. I am a little confused that the YG1 recommended cutting conditions for the 1 flute (E5E47 series, 4mm) 15000 rpm, 1800 mm/min feed 190 m/min Vc and 0.120 mm/tooth. If I run these speeds on my machining centre, slotting 1.6mm think aluminium, full depth of cut, it cuts perfectly. The edge quality is great and chips clear well. FSWizard however suggests I run the bit 15000 rpm, 519 mm/min feed 0.034 mm / tooth. This results in the aluminum instantly melting and the end mill having aluminum welded to it pretty enthusiastically.

The interesting thing for me is that the 2 flute 45 helix E5521 4mm has YG1 recommended cutting conditions of 10000 rpm 1100 mm/min feed 0.055 mm / tooth. Slower feed (but also slower RPM) than the 1 flute. The 1 flute doc also says it slots at 1.5D where as the 2 slots at 0.5D.

Is HSMAdvisor / FSWizard wrong for aluminum specific end mills? Am I doing something stupid using it? If I attempt to run any end mills at the numbers it recommends they melt and in my wisdom I didn't look at the YG1 numbers first... so a 3 flute and 2 flute got aluminum welded to them. Is the 1 flute the best way to slot 1.6 mm thick aluminum? I'm cutting parts for bending in my press brake. These YG1 alu powers are basically magic compared to what I've used before. I haven't tried the rougher yet. I'm starting to think it won't be worth tool changing some of areas as the 1 flute is so fast.
I don't see where you mentioned the parameters from HSMAdvisor. I punched in a 4mm single flute uncoated, cutting 1.6mm deep, and I got a recommendation of 26380 RPM and 1428.15 mm/min, for a .054mm chipload.
 
I use HSM advisor and YG-1 end mills of all sizes. I can push a bit faster than the numbers from HSM advisor, but I also wouldn't think of running alumium without coolant.
 
I don't see where you mentioned the parameters from HSMAdvisor. I punched in a 4mm single flute uncoated, cutting 1.6mm deep, and I got a recommendation of 26380 RPM and 1428.15 mm/min, for a .054mm chipload.

I'm running hangsterfer ozonic 203 coolant MQL. Though coolant and machine shouldn't matter, it's giving me very different numbers than the manufacturer. The manufacturer numbers work fine on my machine.

I just tried the online version of FSWizard in case it was some weird bug that was phone specific. You can try the numbers as well, I'm using 6061 in the example because it's in the free version, though I was using 5000 before because I have the paid version. I'm cutting 5005 H34 specifically.

I put in the solid end mill, carbide, 4mm tip, 1 flute, 25mm stick out 0 corner radius, 15mm flute length, 30 deg helix angle 90 lead angle (not sure where to find that in the data sheet...) 4 mm shank diameter. Engagement 1.6 mm, slotting (100% width of cut) chip thinning and HSM turned off. Max RPM set to 15000 to give me a comparable result to the YG1 numbers.

Result from the calculator is attached. 0.013 mm/tooth feed 195 mm/min, totally wrong. Am I doing something wrong?
 

Attachments

  • fswizard.png
    fswizard.png
    56.3 KB · Views: 6
I just tried the online version of FSWizard in case it was some weird bug that was phone specific.
...
Result from the calculator is attached. 0.013 mm/tooth feed 195 mm/min, totally wrong. Am I doing something wrong?
I think I figured out our miscommunication. FSWizard and HSMAdvisor are two completely different products, made by different companies. You complained about both, but you're only using the first. I only use the second:
 
I think I figured out our miscommunication. FSWizard and HSMAdvisor are two completely different products, made by different companies. You complained about both, but you're only using the first. I only use the second:

They are both on that website and have the same contact, so I assumed HSMAdvisor was just the desktop version and they were the same company. I can get a trial of the HSMAdvisor to check.
 
They are both on that website and have the same contact, so I assumed HSMAdvisor was just the desktop version and they were the same company. I can get a trial of the HSMAdvisor to check.
Okay, I stand corrected. It seems FSWizard is the mobile version, which probably runs different code.
 
I put in the solid end mill, carbide, 4mm tip, 1 flute, 25mm stick out 0 corner radius, 15mm flute length, 30 deg helix angle 90 lead angle (not sure where to find that in the data sheet...) 4 mm shank diameter. Engagement 1.6 mm, slotting (100% width of cut) chip thinning and HSM turned off. Max RPM set to 15000 to give me a comparable result to the YG1 numbers.

Result from the calculator is attached. 0.013 mm/tooth feed 195 mm/min, totally wrong. Am I doing something wrong?
Same inputs in the desktop version of HSMAdvisor, full width slotting:
5000 series Al: 259.81mm/min, 0.01732mm chipload
6061 T6 Al: 240.06mm/min, 0.01600mm chipload

These numbers will be for a general purpose cutter with good flood coolant or TSC. It's probably calculating chipload similar to that for a two flute, and cutting it about in half for your single flute. Single flute cutters aren't used in metals very often so there isn't a lot of data on it; I expect the cutter you're using is a relatively recent development.
 
yeah, so I'm happy the YG1 numbers are right because they mean my parts cut a lot faster, but 1800 mm/min feed 190 m/min Vc and 0.120 mm/tooth. is pretty different to 0.016 mm / tooth... maybe the YG1 are just very strange cutters or the calculator really doesn't cope with single flute end mills. Datron has a bunch of high speed single flutes as well but i'm not sure how much they want to cut per tooth. Either way I learned an important lesson, look at the datesheet and don't trust the calculator too much if the numbers are very different.
 
Last edited:
yeah, so I'm happy the YG1 numbers are right because they mean my parts cut a lot faster, but 1800 mm/min feed 190 m/min Vc and 0.120 mm/tooth. is pretty different to 0.016 mm / tooth... maybe the YG1 are just very strange cutters or the calculator really doesn't cope with single flute end mills. Datron has a bunch of high speed single flutes as well but i'm not sure how much they want to cut per tooth. Either way I learned an important lesson, look at the datesheet and don't trust the calculator too much if the numbers are very different.
Hi,
Just like I said in my very first reply. The difference in numbers (between the manufacturer-suggested and the calculator) is due to parametric nature of the software that relies on average between many manufacturers. It will work in most cases but will fail with tools designed for a specific application. For example I am having very hard time trying to work out parameters for router bits. Same thing happened here with the single flute end mill.
 
Hi,
Just like I said in my very first reply. The difference in numbers (between the manufacturer-suggested and the calculator) is due to parametric nature of the software that relies on average between many manufacturers. It will work in most cases but will fail with tools designed for a specific application. For example I am having very hard time trying to work out parameters for router bits. Same thing happened here with the single flute end mill.

That makes sense, the calculator gives basically identical numbers to the manufacturers recommendations for the 3 flute YG1 alu powers, the 1 flute alu powers are just very strange. They seem to be excellent end mills if you want to slot fast.
 








 
Back
Top