Just found a very good video of testing a table-top gantry router cutting mild steel.

YouTuber named "Breaking Taps" used speeds and feeds generated by HSMAdvisor to get a starting point.

To see where exactly he was in the calculations I decided to reproduce all of cuts in HSMAdvisor.

A couple of assumptions i made:

1. Tool Type: Solid End Mill. It is not recommended to use the HP/Roughing tool type on such light machines, so i assumed this is the tool BT used.
2. Tool Stick-out looked like about 3/4" so I used that number.
3. Material was set to A36 Hot rolled steel.

Test 1) Minute 4:52

Good, slow and very safe starting point.

Test 2) Minute 6:20

Twice as aggressive as before, but we can still push it further.

Test 3) Minute 7:10

Here we can see the lack of machine rigidity starting to show. But at 65% feed rate it is still alive.

Test 4) Minute 8:30

This last test did not go well at all.

The machine has finally hit its limit and the endmill broke at all S&F overrides at about 100%

Was this fault of the software? Not really!

If that were a heavier machine, the last cut would not even be considered that difficult.

Here is a full slotting cut on a Matsuura VMC:

And here is the calculation that was done using HP/Roughing End Mill tool type:

If i were using the "Solid End Mill" tool definition, i would have to dial the feed override to 176% to match the 45ipm feed rate!

So what can users of light machines do in order to not break taps end mills?

First of all make sure the spindle torque curve is built and enabled in your machine profile settings.

The easiest solution is to de-rate the spindle. There is "Warning at" level in machine profile settings. Set that to 50% for starters and it should save you from exceeding the machine's capabilities.

Overall this was a great test of this little machine's capabilities and of the great help that software like HSMAdviasor can lend in discovering them.

Please head over to Breaking Taps YouTube account and subscribe.

HSM with MasterCam Dynamic Milling has long been one of my favorite toolpath strategies when machining hardened and tough to machine steels.

The job at hand was to machine out a 5" disk out of pre-hardened 4340 steel. About 43RC hard.
Due to an island in the middle (leaving only 3/4" room for the tool) I could not use a bigger indexed cutter, so i decided to use the adaptive clearing toolpath.

I started out by calculating Speeds and Feeds with HSMAdvisor and come up with the following starting parameters:

Full depth, at 10% engagement.

Which worked just fine. But the tool was not new and I decided to sacrifice it in the name of science and maxed it up to see how long the tool was going to handle it.

So I adjusted the cutting speed to 170% and feed to 150% (which accounts to heavy roughing):

To be honest I was not sure the tool was going to last very long, but it exceeded all my expectations!
It lasted for about 2 hours and completed the whole run of more than 20 pieces.

I even took a video cutting one of the parts:

Note how there are no sparks coming out. This is because the chip is thick enough to not overheat. This works both ways. Chips stay cool and due to their larger mass carry most of the heat away from the cutting edge.

After the end of the run (and it was not new to begin with) the tool looked like it could do as much!

As unhappy I am to learn that something may be wrong with the software I develop and love, negative feedback is essential in learning whether i am doing everything right.

So a couple of days ago I received an email from a somewhat disappointed user. 

He (lets call him Peter) was complaining that HSMAdvisor calculator gave him "excessively high" speeds and feeds for his 3/4" 4 flute 3.0 LOC  end mill in aluminum.

With the data Peter entered he was getting around 10000 RPM(SFPM 2117) and the feed of 270 inches per minute while usual practice in the shop was side-milling aluminum at that (2.8" axial) depth at only 325 SFM

After double-checking the numbers I replied that in fact his numbers seemed very slow and if for some reason he HAD to run that slow (heck, i machine most steels faster than 325 SFM) due to some conditions, perhaps, he was ought to change the conditions themselves.

This is what I am getting for Peter's end mill setup:

I set the feed override to 50% because it is obvious 0.001" width of cut operation is finishing.
We can see that despite quite long tool projection, deflection in the cut remains below detectable number.
Which means that theoretically he should have been able to run with the speeds and feeds suggested by HSMAdvisor.

In fact it should be able to take a much heavier cut no-problem!

Peter still insisted that my calculations were wrong and that he did not care how fast I ran steels and he wanted the calculator to output the magical low SFM number they were so used to in the shop.

But hey, perhaps my Calculator is wrong and its not possible to spin a 3" long 3/4 dia endmill that fast?

Nope

Back in the days when i was machining aluminum all day long i did use similar numbers but never got to record a video.
Luckily there is YouTube for that.
Check out this guy running his  SGS S-CARB 3/4" DIA X 3 1/2 LOC  end mill cutting QC-10 aluminum at 12000 RPM 360 inches per minute

Clearly 10000 RPM and 270 IPM does not seem that radical compared to that!
In fact HSMAdvisor is suggesting numbers very close to the ones posted in the video.

So what was the reason Peter is using such conservative cutting speed (he never mentioned the kind of feed rate he was going at) ?

Perhaps he was getting chatter and/or was afraid of snapping his cutter?

One thing stands out to me from this story is Peter mentioned he is using a 4 flute endmill. Knowing that usually Aluminum-specific cutters come with 3 flutes, I immediately thought that he perhaps is using a wrong tool for the job. Incorrect tool will cause al kinds of problems like chatter, bad surface finish and such.

Unfortunately Peter never told me what were the reasons for using the current low cutting numbers. Only that my calculator's numbers were wrong for his application.

If I were Peter I would call the SGS guys and ask them to set up a test with their tool. With the $250 cutter on their tab he will not be as afraid to snap it:)

Start low and slowly creep up the overrides (and confidence) until the spindle' load meter pegs out at 80%-90%

Try HSMAdvisor Speed and Feed Calculator too. Aside from suggesting cutting Speeds, Feeds, Depth of Cut it will aslo tell you about the Tool Deflection, Spindle Load and tons of other useful information that will help you stay safe while being productive.

In this particular case Peter could easily increase his productivity tenfold versus the old numbers. I hope this makes him reconsider his current approach.

Nobody has to machine aluminum at 325 SFM these days!

Have you ever wondered how much tool life can deteriorate when using coolant with High-Speed Machining (HSM)?
Or maybe you never really saw the boost in tool life when using HSM techniques because you had to use coolant?

Well, here is a test result I just got from running the same tool at the same Speed and Feed with and without coolant.

A short preamble: 
I had to machine a 1080 steel component where chip clearance was an issue. Without programmable airblast and due to an unattended run of the machine I  decided to try and see how long the tool is going to last with the coolant turned on.

I calculated cutting parameters using HSMAdvisor Speed and Feed Calculator and came up with the following data:

Because I had hundreds of parts to machine, I could get good sample data.

So I ran each tool for as long as I was comfortable with the noise level.

The results of the test surprised me quite a bit.
Yes, I knew tool life with coolant would be less than without, but I did not expect such a dramatic difference:

	Through Spindle Coolant. Perfect chip removal.	Dry. No Airblast - some chips re-cutting in the pocket
Number of Parts	45 pcs	400 pcs !! Could do another 400 easily.
Tool after the run		(Picture for demonstration only. The original file was lost.)
Comments	The run stopped when the tool was making a lot of noise and pushing too much burr up the wall. Coating stripped from cutting edges. Lots of plastic deformation.	Tool survived barely touched! Finished the rest of the batch with the same cutter and could run the same amount easily. No considerable wear on cutting edges and no built-up edge.

We got at least a 10-fold improvement in cutter life just by turning off the coolant.

Counter-intuitive, but that is High-Speed Machining for you. It does not have to make sense!

We know that the bad tool life is caused by the thermal shock of the tool coating and the carbide itself at high temperatures that are produced by high cutting speeds.
You can read more on the theory behind HSM in this article->How to: High-Speed Machining (HSM), CNC Milling
Here is a small excerpt from it:

How about that gummy stainless?

I know what you are going to say: "Let's see you try no coolant with some 304 Stainless Steel"
And I agree with you. Sometimes when we are getting a lot of built-up edge on gummy tough materials we just have to use coolant. And that will negatively impact your tool life!

There are, however a few tips on dry HSM-machining gummy stainless:

• Use less radial engagement (about 5%).
• Use heavy feed.
• As a result of the above, you can use a higher cutting speed

What this less radial engagement does, is it allows you to surpass the "no man's land" between 300 and 900 SFM where built-up edge forms on the cutting edge.
In addition to Chip Thinning our HSMAdvisor accounts for the SFM boost, you can get in that case. Just turn on the "HSM" checkbox! 

If you tried everything and you are still getting chip weld, you might have no other option than to turn on your coolant and suck up the bad tool life.

Some materials are just crap to machine and that's the end of it.

Happy Millin'!

Look for the HSM machining of the round central pocket in the beginning.
Here we have a 12mm 6 flute Coated hi-performance endmill, cutting 1" deep at 0.047" (10%) rWOC.
at 10000 RPM and 300 ipm feedrate. the chipload works out to be 0.005". Material is 4140 pre-hardened steel.

Impressive isn't it?
Those results have been achieved with uber-expensive BlueSwarf tap-test technology.

This is one video that caught the eye of one of my HSMAdvisor trial users:

Being a geek and wanting to help the user make the right decision I immediately punched the numbers into my HSMAdvisor app.

Here is what I've got:

Not too bad huh? My Speed and Feed calc suggests almost the same chip-load.
But because it is caring about your tool life, HSMAdvisor suggests slower cutting speed. 4464 RPM versus BlueSwarf's 10000 RPM

Now, if we wanted 15 minutes of tool life (what the tool on the video is probably going to have)
We could have entered 10000 RPM and voila!

We are getting almost the same feedrate at the expense of tool life.

86% of Tool Life versus 18% - You decide which is better. HSMAdvisor gives you that ability.

You can also decide whether super-expensive technology like BS is really worth the hype and the money spent.

But we are not over yet.

Let us try another calculator. The HSMAdvisor's direct competitor.
Introducing the G-Man(real name hidden).

This series of screenshots was sent to me by a user of that software, who showed me the okuma video to try and make sense of his results.

He entered the same tool numbers with the same material to see what the Goliath of the S&F business suggests:

All the tool data is absolutely the same.

We can see that G-Man really cares about his customer's tool life because his RPM is really low.
However his Feedrate seems kind of HIGH....

How high - I do no know. What's the Chipload? 0.003" or 0.005".....hmm OK.....

Then the user set RPM to 10000 like in the Okuma Video at the top of the article:

HOLY FLYING CUPCAKES!

10000 RPM and 650 IPM !

Why is the Feedrate so high?
Isn't there something in the calculator that should prevent the machinist from leaving the Endmill inside the pocket once the E-Stop is pressed and Z-Axis is retracted?

Yes, everything is set to "Rigid" and "Rough" but you would not normally expect such mild words to cause much trouble, would you?

I am starting to realize that something is very very wrong here.

In the last screenshot his Chipload(IPT) shows 0.0108". Please note in the previous screenshot he has 0.003".....

How does a mere fact of changing the RPM change the Chipload so much?

I am going to the previous screenshot and start doing some math. Something that G-Man should have done for him:
185.9ipm / 6 flutes/ 2640 RPM = 0.0117" Chipload.

Where does 0.0117 show on that screen? Nowhere!

Whelp. Perhaps before "...considering over 60 variables..." G-Man should get his basic math in order?
Or a program workflow. I don't know - I am not an accredited IT engineer to advise on that.

Also note that aside from the Deflection nothing shows us how hard we are really pushing the Endmill.

What if I told you that the endmill in question WILL NOT survive 0.004" deflection at all?

How does my HSMAdvisor know it? Math. Not even some hard-core science. Just a high-school level.

Does G-Man know it?

Dohis customers it?

HSMAdvisor users learned to trust the Limits I have put in place to protect their tools.
If it says "Can't do it" there is a really high chance that you really should not!

What do other people who run HSM machining toolpaths for a living say?

Here I assembled the cuts posted for 4140 PH or similar steel with a similar tool diameter on Rizzo's Dynamic Database :

Chipload:	0.007"	0.0068"	0.007"

At the bottom of each column I calculated the actual chipload the comparable tools were making.

These results by real people are in fact more in line with HSMAdvisor's default suggestion than with the Okuma Video.

And shure as hell none of them goes any close to 0.011" per tooth in such situation.

It is not my job to point to my competitors mistakes (though he probably should thank me for finding them).
But it is a word of caution for those who use Speed And Feed Calculators, that do not consider the endmill's strength and do not show you how hard you are pushing your tools and machines.

A user who does not see what he is doing is bound to break something.

So the big question everyone is having: Is G-Man plain wrong?

I seriously, do not know. His calculations seem just too wonky to be even sure this is the intended result.
Here is what I have when I try to simulate G-Man's results:

It is possible! With Torque Limit almost at its maximum (190% is no joke)

For a minute or two! Then you will likely hear an unmistakeable sound of the endmill snapping.

Only a mad man would run his tools like that. I mean who has the time and the money to replace his tools like that?
Unfortunately for his customers G-Man does not tell them that kind of information.

What did I advise the customer? I sent him a link to this article, so he can decide.

Regards.

Sometimes I get asked whether hsmadvisor CNC Machinist Calculator is reliable enough out of the box.

I and many others test it at work every day. This 2"x1.5"x1.25" 4140 PH piece was programmed on masterscam with hsmadvisor speeds and feeds with all overrides set to default.

Worked out fast and awesome. As usual!

14497779489640.jpg

A couple of days ago I helped a gentleman by answering a few questions about using HSMAdvisor Speed and Feed Calculator to machine a 310 Stainless Steel piece using HSM techniques.

Today he created a post on PracticalMachinist forums walking us through his experience.
And he even took a video of the part being cut!

Endorsements like this is the best thing any software developer can hope for.

I always welcome any feedback regarding my software and never mind helping anyone, whether he is a novice, experienced machinist, my customer or not.

Thank you Sebastien, good luck to you!

Here is a video of a 3 flute Hi-performance endmill slotting aluminum 0.75" deep per pass.

Well, not entirely slottimg, more like pocketing, but the very first move is a full width slot.

Stepover is 0.4"

First i calculated the cut on HSMAdvisor.

Used 6061 aluminum as material and HP endmill at a tool type.

Tool torque and deflection limits were both set at 100% and performance slider was at maximum.

This is what it came up with:

S9127 RPM 125 IPM.

Full slot, 0.75" deep.

45 in^3/min mrr.

Looking at how easy it went i think i should allow for more load in my calculator.

If you have not yet tried HSMAdvisor, make sure you do.

You will be amazed at how much productivity you have been missing out on.

Sevaral weeks ago i saw a post on CNCZone.

A HSMadvisor user Peter Neil used it to calculate cutting conditions for cutting a block of pre-hardened stainless steel.
His machine was Tormach.

Here is an exact copy-paste from that forum post:
_____________________________________________________________________________________

Did a test cut on the Tormach today using feeds & speeds from the latest version of the excellent HSM advisor.
To make it interesting, I did the cut using some 1.2085 pre-hard Stainless Steel as I have plenty of stock of it and have a job in mind for this, and wanted to see how it cut on the Tormach.
The material is like a stainless P20, at 16% Chrome/1% Nickel & 0.5% Sulphur (which makes it slightly free-er machining) and is hardened to around 33-35 Rockwell C, so I used the HSM advisor guidelines for machining P20 rather than Stainless. Cutter was a 10mm 4-flute Carbide TiAlN coated EM.

So...... ticking the HSM/Chip thinning option I got a speed of 5120 and feed of 2214mm/minute( 87 IPM). I used a DOC of 10mm and WOC of 0.5mm/0.020" - and turned off the flood cooling to machine it completely dry. The finish pass on the 1st level was 15mm DOC and 0.5mm WOC and slightly lower speeds/feeds.

Loaded up a 40mm x 63mm block , pressed the start button, and it went from this....





...to this!

Very impressed. Total cut time around 12 minutes. The spindle load meter went into the Yellow zone on some of the 10MM DOC corners, but for the rest it was firmly in the green. And when it was finished I could easily hold both the part and the cutter, which were both 'warm' rather than 'hot'. Lots of lovely golden coloured thin chips though.
Could do with an air blast to clear the chips when cutting the pockets as the finish suffered slightly because of this, but will sort that out, and had a slight programming anomaly which produced a weird cut on the very top surface.

But overall I'm quite pleased with that. I wish I had a video camera so I could show it in action.

________________________________________________________________
Thank you Peter,

The complete forum thread is located here

Sometimes people ask me: "I tried your calculator, and i liked it, but it seems to me a little too aggressive...do you actually do any testing?"

Well, to those I say that not only i do testing, but i run production jobs 100% calculated with my own HSMAdvisor.

Many machinists say that nothing beats an experienced operator holding his hand on feed hold button and playing with speed and feed override trying to find the "sweet spot" where cutting speed and feed rate are maximized and chatter is eliminated or reduced.

And it is correct, but not any machinist is experienced or actually knows what he is doing.
Many machinists also finish their apprenticeship program and never learn a single thing about new tooling types and materials since. They bag years of experience, but their knowledge is stuck on a level it was when they first got their license.

Also not a single person can possibly know cutting conditions for hundreds of materials and remember all of the jobs he had ever ran.

This is where tool database comes in.

Not only can you save tools to cut down and in many cases eliminate entering parameters for every calculation.
But you can (and should) save cutting data for each particular case.

A single tool entry can contain an unlimited number of cuts attached to it, so machinist never has to remember everything.

Here is a i made video of slotting D2 with variable helix hi-performace endmill.

Material: D-2 Tool Steel 200-250 HB
Tool: 0.500in 4FL Carbide TiAlN coated Solid HP End Mill
Speed: 360.0 SFM/ 2751.6 RPM
Feed: 0.0023 ipt/ 0.0094 ipr/ 25.76 ipm

Engagement:  DOC=0.330 in   WOC=0.500 in