Should I mess with manufacturer recommended feeds and speeds?

[AmericanMaker]

I have a question about changing manufacturer recommended feeds and speeds (specifically SFM and chip load) to values that I think enable HSM.

I will be machining 1018 (my first time for this material). I have a 1/2 in, 5 flute carbide end mill with TiAlN coating. It is a Haas HSPM2 series end mill.

For that specific end mill and material Haas recommends cutting speeds (pdf link) between 490 and 660 SFM with a chip load of 0.0034, an ADOC of 1.5 x D and an RDOC of 0.5 x D.

Using a feeds and speed calculator, the result is a cutting feed rate of 86 IPM. If I change the RDOC to 0.2 x D at 660 SFM, the RPM is 5,042 with a cutting feed rate of 111 IPM and a chip load of 0.0044. If I change the SFM to 1,000, the RPM goes up to 7,640 with a cutting feed rate of 169 IPM and a chip load of 0.0044.

My Sharp SV-2412SX has a 15 HP 10k RMP spindle with a max cutting feed rate of 394 IPM.

Is it unwise to increase the SFM above manufacturer's recommendation to take advantage of my machines capabilities?

I'm a beginner machinist and have lots to learn. I may be misunderstanding HSM and all the related specs and data. So please correct any misunderstandings I may have.

Thanks!

 

[mhajicek]

Use a feed and speed calculator that accounts for radial and axial engagement and tool length. HSMAdvisor is a good one.

Advanced CNC Speed And Feed Machinist Calculator - HSMAdvisor

HSMAdvisor is an Advanced Speed And Feed Calculator for Professional CNC Programmers and Machinists. It supports hundreds of combinations of cutting materials, tools and coatings!

hsmadvisor.com

 

[Donkey Hotey]

Haas already destroyed a bunch of cutters to compile that chart of data and you're not happy?

Handing you the answer won't teach a thing so lets lead you to the answers:

• Do you have Machinery's Handbook (or another source for this information)?
• What is the recommended SFM for 1018? Not from Haas. What is the industry accepted starting point? Ballpark answer is fine.
• Do you happen to know what it is for aluminum?
• What constitutes high speed machining in your mind?
• What factor causes you to have to slow down a cutter?

 

[AmericanMaker]

mhajicek, thanks I am using FSWizard which is developed by the same guy that created HSMAdvisor. Unfortunately I can't run HSMAdvisor on my MacBook, it's a Windows only app.

But the crux of my above question is this ...

Is it unwise to increase the SFM above manufacturer's recommendation to take advantage of my machines capabilities?

 

[Donkey Hotey]

Is it unwise to increase the SFM above manufacturer's recommendation to take advantage of my machines capabilities?

Yes

 

[AmericanMaker]

Haas already destroyed a bunch of cutters to compile that chart of data and you're not happy?

It's not about me being happy or unhappy. For me it's more about learning if it is wise to push beyond tool mfg recommendations to take advantage of my machine capabilities.

Handing you the answer won't teach a thing so lets lead you to the answers:

I like that! I retain more of what I learn when I have to dig in to find the answers.

* Do you have Machinery's Handbook (or another source for this information)
I don't and I really need to get one. However I do have the Engineers Black book and Morse Cutting Tools Machinist's Practical Guide.

* What is the recommended SFM for 1018? What is the industry accepted starting point?
Ballpark ... I think it's around 400 SFM for 1018.

* Do you happen to know what it is for aluminum?
Ballpark ... I think it's around 800 - 1200 SFM for 6061.

* What constitutes high speed machining in your mind?
- HEM and HFM both provide a means to cut faster than conventional roughing.
- HEM is the opposite of HFM

• Higher ADOC (deeper depth of cut)
• Smaller RDOC (stepovers)
• Faster feed rates
• Solid Carbide End Mills are the tool of choice
• HEM is based on the “RADIAL chip thinning” theory.

- HFM is the opposite of HEM.

• Smaller ADOC (shallow depth of cut)
• Larger RDOC (stepovers)
• High feed rates.
• Indexable Cutters are the tool of choice.
• HFM is based on “AXIAL chip thinning”

* What factor causes you to have to slow down a cutter?
- The first thought that comes to mind is heat reduction. However it's also my understanding that solid carbide TiAlN coated cutters work best in a high heat range with air blast to clear chips and no coolant to prevent thermal shock.
- I think the harder the material is, the slower the cutter speed, but there's probably ways around that too.
- Another thought that comes to mind is for a finish pass. I think HEM is primary focused on roughing.

Thanks for the great questions @Donkey Hotey!

 

[Donkey Hotey]

Slow golf clap. Bravo. Good answers.

I'm using Machiner's Handbook 27 so my answers may be a little old. 1018 with uncoated carbide lists optimal at 735 SFM and coated as high as 1050. Problem with that is it's under optimal conditions and we don't always have that. By comparison, HSS is all the way down at 110 SFM on the same material and cutting conditions.

What Haas did was break and wear out a bunch of cutters to find the optimal conditions for that particular cutter. As you noted, heat is your enemy. As heat goes up, so does the wear and damage to the carbide. Don't forget the impact the cutting edge makes every time it climbs into the cut.

What you'll likely find is that targeting the middle of their range will give you the longest tool life. Going for the higher end might shorten cycle time but, cutter life will go down. So too will the ability to not be damaged in less than optimal cutting engagements or places where it's shadowed from the air blast. Then again, Haas might be recommending coolant with those numbers so I'd personally do whatever they say works.

If those feeds and speeds aren't enough and you still want to go faster, the answer may be in cerammic cutters:

 

[AmericanMaker]

@Donkey Hotey that was very helpful, thank you!

I will take that advice and target the middle of their range. I definitely want to take advantage of the longer tool life for now. At some point, as a learning exercise, I will mess around with speeds and feeds to see how much I can push the machine and the cutters. But for now I have tons to learn, so I'll kick that can way down the road.

Thanks again!

 

[mhajicek]

Is it unwise to increase the SFM above manufacturer's recommendation to take advantage of my machines capabilities?

No, absolutely not. If you stick to those numbers you're wasting time. Most cuts will not be at exactly the depth and step listed; if it's shallower or narrower, you can go faster. That's why you NEED to use a calculator program like HSMAdvisor, or the Helical Machining Advisor, etc. Shallower cuts can take a heavier chipload, and narrower cuts can take both a heavier chipload and a higher surface footage.

And I hate to be this guy, but if you bought a MAC for CADCAM, you made a bad mistake.

 

[MaxPrairie]

Please post video of 0.5xD at 86 ipm. 10% radial is my go to in steel. 20% in aluminum, 8% in stainless. SFM sounds good though.

 

[Freedommachine]

What an unusually pleasant exchange of information this has been so far.

@Donkey Hotey the SFM numbers from the Machinery's Handbook, are those for TiAln coated carbide or uncoated? It makes a substantial difference.

When it comes to exceeding recommended SFM, I believe that one of the most important factors becomes tool rigidity and run-out. A solid holder with a Weldon flat retaining screw probably isn't a good idea. Having a good chip evacuation and a smooth tool path with consistent chip load is also important.

 

[eaglemike]

I too had good luck with HSM Advisor. I did find that I was able to make things work better after a bit by changing parameters. Often they have not run exactly the same job you are running with the same machine.
Good luck!!

 

[AmericanMaker]

Please post video of 0.5xD at 86 ipm. 10% radial is my go to in steel. 20% in aluminum, 8% in stainless. SFM sounds good though.

Will do. I'm first making the part in plastic to prove out my design. I'll follow that up with the 1018 which I will record. It should be fun to either watch it succeed or watch the end mill explode.

 

[Donkey Hotey]

What an unusually pleasant exchange of information this has been so far.

@Donkey Hotey the SFM numbers from the Machinery's Handbook, are those for TiAln coated carbide or uncoated? It makes a substantial difference.

I quoted both with and without coating. Of course you guys are all correct in what you're sharing. I was trying to give him enough to get started and learn the nuances later.

If he had a contract to reduce cycle times on 10,000 parts, playing with all the numbers and pushing to the limits is advisable. From his post history, he's just getting started. Simply ramming the cutter through the part at much higher speeds is obviously not possible.

He's also chosen a 5-flute end mill. While shallow engagement will be okay, side cutting forces on the cutter and work holding will go up rapidly as more and more flutes get introduced to the material (radial step-over). Blowing up a $50 end mill and/or having a part violently yanked out of the vise is probably not something he wants while he's feeling his way through this.

 

[AmericanMaker]

And I hate to be this guy, but if you bought a MAC for CADCAM, you made a bad mistake.

Nope, I already own several Macs.

I'm a full-time software engineer and I do all my coding on Macs.

I was a part-time touring musician for 10 years and Macs are the go to computer for running music software for live shows.

Also I love working in Fusion 360 which works great on Macs too.

Maybe one day I'll become a Solidworks or Mastercam guy, but I'm not dropping that kind of coinage now.

 

[Freedommachine]

I quoted both with and without coating. Of course you guys are all correct in what you're sharing. I was trying to give him enough to get started and learn the nuances later.

If he had a contract to reduce cycle times on 10,000 parts, playing with all the numbers and pushing to the limits is advisable. From his post history, he's just getting started. Simply ramming the cutter through the part at much higher speeds is obviously not possible.

He's also chosen a 5-flute end mill. While shallow engagement will be okay, side cutting forces on the cutter and work holding will go up rapidly as more and more flutes get introduced to the material (radial step-over). Blowing up a $50 end mill and/or having a part violently yanked out of the vise is probably not something he wants while he's feeling his way through this.

I'm pick'n up what yer puttin down. "Probably best not to" is likely good advise for a new guy playing with house money.

Will do. I'm first making the part in plastic to prove out my design. I'll follow that up with the 1018 which I will record. It should be fun to either watch it succeed or watch the end mill explode.

1018 is the most common, generic cold rolled steel you will come across, it shouldn't give you any trouble. I don't think you mentioned the axial doc but here is what FS Wizard recommends for a tool with 1.75" LOC:

 

[Mtndew]

Is it unwise to increase the SFM above manufacturer's recommendation to take advantage of my machines capabilities?

For drilling and turning, yes.
For end mills not at all because the stepover and depth of cut can be a thousand different combinations. It's all about chip thinning to get the max out of your tool and machine.

 

[gregormarwick]

Using a mac is not an obstacle to running windows software. Buy HSMAdvisor and run it in a VM. It's worth it.

Don't buy a copy of Machinery's Handbook - every single piece of information in that brick of paper is a 100 fucking years old and I don't know why people keep recommending it.

 

[nn21]

Using a mac is not an obstacle to running windows software. Buy HSMAdvisor and run it in a VM. It's worth it.

I'll second this. I do all of my solidworks, solidcam, and hsmadvisor work through parallels. Works just as stable as pretty much any windows computer I've ever used. hsmadvisor is such a valuable asset that the <$100/yr price of parallels (I'm sure there are cheaper alternatives) is an easy decision. It will basically pay for itself when hsmadvisor saves you from blowing up one endmill.

 

[zero_divide]

mhajicek, thanks I am using FSWizard which is developed by the same guy that created HSMAdvisor. Unfortunately I can't run HSMAdvisor on my MacBook, it's a Windows only app.

But the crux of my above question is this ...

Is it unwise to increase the SFM above manufacturer's recommendation to take advantage of my machines capabilities?

It is actually recommended to adjust both the SFM and the chip load when machining at low radial engagement.
You will get a better tool life and increased productivity.
It is often also beneficial to use air blast to clear the chips and no coolant because it causes thermal cracking and cutting-edge deterioration.
In this case, I was running HSM tool paths at 1300 SFM and 0.010" ipt for days with the same tool:

Best High Speed Machining is Dry Machining | HSM Machining

Resources and Software For High-Performance CNC Machinists

zero-divide.net