Support => CamBam help (General usage) => Topic started by: Doanwannapickle on June 22, 2007, 21:26:59 pm

Title: Speed & Feed Primer ~ Long & Boring & Essential
Post by: Doanwannapickle on June 22, 2007, 21:26:59 pm
How to cut stuff.  If you're of a metric mind, you'll have to do your own conversions.  Here's a web page that will help understand this explanation: (

RPM:  The first and most important parameter you need to keep in mind is RPM.  RPM is arrived at via the formula: RPM = (4 x CS) / Dia. where CS is cutting speed.  Cutting speeds are associated with materials.  Each material has it's own cutting speed for each type of cutter.  There are a number of good charts available that list cutting speeds.  (See above.)
Keep in mind: The formula is a simplification derived from pi.  It's easy to get away with this because the cutting speeds are approximations subject to a number of variables.  The charts and the formula just provide a good starting condition.  However, once you arrive at a good rpm for your particular machine, using your favorite coolant and your typical cutter, it's easy to back figure your actual cutting speed which will then give better results the next time you machine that material.

FEED:  Feed is arrived at via chip load.  Chip load is simply the thickness of the chip.  Chip thickness varies with RPM and feed so if you change your RPM you are changing your chip load unless you also change your feed.  Obviously, the inverse is also true.

VARIABLES:  The big variables are rigidity, coolant and cutting tool.
The more rigid your machine and setup, the faster you can go.  It's as simple as that.  The cutting speed charts and chip load charts are for middle of the road average machines and machining operations.  If your machine and setup is exceptionally rigid, you can adjust everything upward.  If your machine and/or setup is lightweight, adjust downward.
Coolant is a real mixed bag.  Naturally, the best coolants are messy, bad for your health and bad for your machine.  (Must be some corollary to Murphy?s Law)  Coolant should be avoided if possible or at least minimized.  Micro drop application systems work well but are expensive.  Spray mist is affordable but will put a lot of mist into the air that eventually settles on everything.  Use only with coolants made for misters.  No matter how good your ventilation is, you'll be breathing some of it.  Flood coolant is the cheapest and messiest.  Best used on machines built for it.  So, on the one hand, we try to avoid coolant but, on the other, coolant will improve finish and tool life tremendously.  Pick your poison.
Cutting Tools: In general, the softer the material, the sharper your tool needs to be.  CBN inserts for hard turning actually have a bit of negative rake.  Look at a roughing insert for steel and you'll see that the edge has a small radius.  At the other end of the spectrum, plastic needs a very sharp cutter.

DOC:  Depth of Cut.   DOC is almost impossible to define.  DOC is the one parameter that is most affected by the variables.  The only thing that can pinpoint DOC is experience with your machine and your setups.  Use common sense, start conservatively and work your way up.  DOC is also affected by your chosen speed and feed.

Materials:  Material science is essential to machining.  I'm often asked 'how do I machine aluminum (or steel or plastic etc.)'?   This is a bit like asking how fast a car can go.  Which car?  Which engine?  Street or Bonneville Salt Flats?  There are a LOT of different types of steel and aluminum and plastic.  They all have different properties and they all machine different.  It's often cost effective to buy a material that's a bit more expensive just because it will machine so much better.  A lot of forethought to your material will save a lot of work down the way.  Go to a site that sells these materials and they will often list the machining properties, physical properties and the cost.  My personal favorite is McMaster Carr.  Once you have a specific material in mind, it's much easier to address questions.

Tips:  6061 is a good, all around choice for aluminum and is quite affordable.  If you experiment and get the feed and speed just so, it can be machined dry.  The trick is the get the chip to part company with the cutter.  Aluminum likes to stick to the cutter, then comes back around and sticks to the next chip then in an incredibly short period, totally gum up the cut.  If you can get the chip out of there, this won't happen.  If the speed and feed are working together the chip sails right out of there.  In general, when conventional milling you will need a small step-over (~10%) and a high feed rate.  When climb milling back you need a large step-over (~60%) and low feed rate.  To machine dry, you will need to keep the rpm lower to keep from heating things up too much.  If you do need a lubricant, WD40 is excellent.  A very small amount is needed.  I buy it by the gallon.
Steel requires the least amount of explanation.   If your machine is heavy enough to cut it just follow the speed & feed guidelines.  Coolant is recommended.
Polymers.  I already mentioned that plastic wants a keen edge.  Particularly the softer plastics.  What I didn't mention is some polymers can be surprisingly abrasive.  If your cut starts out good then shortly develops a burr, you've lost your edge.  It will look and feel sharp but it's not.  Switch plastics or switch cutters.  Go to carbide.  Keep your rpm low enough not to melt the material.  Coolant can sometimes benefit.

Hope this helps,

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: mrbean on June 22, 2007, 22:37:12 pm
That's a good intro into feeds/speeds and should give a good starting point.
I need some tips myself.  I've just been winging it, going with what seems to work and making adjustments from there.

Oh BTW....  I can't stop listening to the "MotorCycle" song.  Groovy man...

Regards MrBean.

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: 10bulls on June 22, 2007, 23:28:46 pm
Yes, thank you Mr Pickles.

That glubbing noise you may have heard was me and MrBean getting out of our depth talking about machining type stuff.  Me?  Hey, I'm more the suck it and see kind of a guy.  But it's wise to know the theory behind it all.

BTW:  Speaking of toxic coolant.  I just had to go fish out my hex keys from the Rocol coolant sump.  I've also been cutting some rather jolly JCB yellow plastic into it.  It's starting to get ugly down there!
Is it me, or do those hex keys appear to be giving the finger?

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: servant74 on November 08, 2008, 01:54:29 am ( has another good speed/feed calculator that includes woods and MDF

It is down from 11/7-11/10/2008 for maintenance.

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: MuellerNick on May 16, 2011, 18:25:00 pm
I know, an old thread.

But I do have to correct it a bit:
You should look at the parameters from a different perspective, so you can make compromises at the right parameters.

But first, it is absolutely right to consult manufacturers' data about their cutters.

The most important factor is chip load. The thickness of each chip. It depends on the material (the harder, the smaller the chip load), the size of the cutter (bigger cutters make bigger chips) and the material (+ geometry) of the cutter. HSS takes less, carbide can take absurd chips. It is important to realize that the effective chipload is what counts. You'll see later what that means.
You can't go much below the recommended chip load, because the cutter will start rubbing and heat up. After some rounds, it will cut and then rub again. The sharper the edge, the smaller the chip load can be. From that rubbing, the edges get dull and the cutter is bent with each rotation. It will break by fatigue, but first it will get dull.
If you increase the chipload, the cutter will break sooner or later by overload.
Small (2 mm) HSS cutters do have a chipload of below 0.01 mm. It is good to use the biggest cutter that does the job.

Cutting speed is a tad less important, but still not to be ignored.
Generally, it is just material (to be cut) dependent. Size doesn't matter. Consult the mfg's data. HSS takes less speed compared to carbide (that often takes something around 5 fold a speed). It might be a bad decission to buy carbides when your spindle doesn't make the necessary rpm.

So, how do you get rpm and feed?
First, calculate rpm from the cutter diameter and the recommended cutting speed. If your spindle doesn't go that fast, either use HSS, a bigger cutter or live with the lower speed. Carbides often gives a less good finish with too low a speed, HSS is much more forgiving with low speed. Too fast is always bad.

From the cutting speed you calculated (and not the one you should have but can't do) and the diameter, you get the rpm :
Cutting speed [Vc] in m/min, diameter [d] in mm
S = Vc * 1000 / (d * 3.14)

From the rpm, the chipload and the number of flutes, you get the feed. But wait!
With a given feedrate, the chipload varies depending on HOW you cut. With a full cut (cutting a slot; half of the circumfence is in contact and cutting) down to the cutter's radius you do have full chipload. If the cut is less (not DOC, but sideways cutting) the effective chipload gets less. With a shallow finishing cut that is just dusting off a tenth of a mm it is just a small fraction compared to a full cut. This means, that you can and have to increase feed to be within the recommended chipload.
Feed F [Vf] is:
feed per tooth (chipload) [ft], number of teeth (flutes; cutting edges) [t] and spindle speed S
F = ft * t * S in mm/min

Depth of cut. It mostly depends on the length of the cut. With a full cut, each edge is cutting for half of the circumfence. When finishing, just a fraction of the circumfence is cutting. Obviously, the more chips you make, the higher the load on the cutter and the hotter it gets. A DOC of 1..2 times the diameter is doable in steel with an HSS and full cut. A safe value is 0.5 times the diameter (10 mm cutter -> 5 mm DOC). When cutting just with the side and a shallow cut, 5 times diameter is no problem.

Of course, as already said, there are other parameters that will influence speed and feed. But at least, you got a good starting point.

Cut, don't rub!
Look at your chips, they should be nice and and equal. Dust is a bad sign (for metal).
Don't cut too hot. HSS shouldn't make more than yellow chips.
Use flood coolant or mist cooling (with metal).

Hope that helped a bit.


Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: macpod on December 12, 2012, 04:27:44 am
I have found this speeds/feeds calculator to be convenient:

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: Bob La Londe on October 03, 2013, 16:13:10 pm
I have found this speeds/feeds calculator to be convenient:

I have been using FSWIZARD for a while.  I've found in general his cuts work, but you darn well better be doing everything just right.  Also, he assumes a very rigid machine, flood on aluminum, or slotting, etc, without saying so.  On my Hurco I can take some pretty aggressive cuts using his numbers, and its an order of magnitude more rigid than my little machine, but if I push it to the max I can get some "boat steer" plowing of the cutter.  Also, you had better know or measure stickout, helix angle, flute length, etc or his program automatically places ideal flute length and stickout and default helix angle.  Trust me there is a huge difference between ideal stickout and the stickout you have to use a lot of times. 

I'll post a picture later of a piece cut using his numbers without taking everything into account that will make you go hmmmm! 

I think also he has a strong emphasis on high speed machining numbers.  Even when you have the HSM/Chip Thinning selection turned off I feel like the cuts calculated are a little aggressive. 

Title: It was like a train wreck
Post by: Bob La Londe on October 04, 2013, 23:12:18 pm
I watched this cut while it was happening, and it was a like a train wreck.  You want to look away, but you can't. 

Title: Re: It was like a train wreck
Post by: Bubba on October 05, 2013, 01:32:54 am
I watched this cut while it was happening, and it was a like a train wreck.  You want to look away, but you can't. 


Two thinks come to mind seeing this cut. You machined 6061-T3 material? It was a single pass all around? Did you use a downspiral cutter? Soft aluminum will cut like that if there the chipload (depth of cut-feed rate- spindle speed) is not correct. 2024-T3 and 7075-T6 are expected to cut much better, in fact you can hear the chips ringing when they hit the floor.. I never liked to machine the 6061-T3 for reason you described in your post, Had a reasonable result using compressed air directly behind the cutter.

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: Bob La Londe on October 05, 2013, 03:00:02 am
6061-T6.  I have made similar cuts since then using high volume flood coolant and it didn't weld up like that.  my point was that FS wizard is a good speed feed calculator, but you have to be doing everything right.

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: Jeff_Birt on October 05, 2013, 03:25:12 am
my point was that FS wizard is a good speed feed calculator, but you have to be doing everything right.

That is the problem with every feed/speed calculator. Their output is only as good as your input and there is no way possible for them to account for every possible bit geometry, material, machine, GCode type combination. The best you can hope for is an educated guess within the range of materials and bits you normally run on a machine.

I remember going to a SurfCAM training class when they first came out with the 'Velocity' constant tool engagement angle (trachoidal sp?) tool paths. The first demo video they made they maxed out the feed rate on the mill, they could have machined faster if the mill went faster. Point being that your GCode also has a huge impact on your speed/feed rates.

I found this video with a quick search, they are machining 316 stainless: . Here is a neat high speed video showing the chip formation: .

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: pixelmaker on October 05, 2013, 11:57:11 am
Why you don´t use the feed/speed calculator in Cambam?

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: Bob La Londe on October 05, 2013, 23:40:06 pm
There's a feed speed calculator in CamBam? 

I gotta find that. 

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: Bob La Londe on October 06, 2013, 14:53:07 pm
Why you don´t use the feed/speed calculator in Cambam?

I looked and I don't find that.  I feel like a total beginner there.  If CB has an SF calculator built in I sure can't find it. 

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: blowlamp on October 06, 2013, 15:02:40 pm
Why you don´t use the feed/speed calculator in Cambam?

I looked and I don't find that.  I feel like a total beginner there.  If CB has an SF calculator built in I sure can't find it. 

Define a MOP and you'll find the calculator if you right-click on it.


Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: dh42 on October 06, 2013, 15:05:22 pm


Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: Bob La Londe on October 06, 2013, 16:53:53 pm
Ah, I see why not to use it just yet.  Its very simple.  No horsepower or deflection calculated, no material data, no accounting for cut type or cutter type, flute type, materials, coatings etc.  FS wizard is a much more filled out FS tool. 

Now that I have seen it I recall having seen it before. 

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: pstemari on October 06, 2013, 18:40:11 pm
I've been using GWizard from  It's not free, but pretty good at dealing with horsepower constraints, rigidity, and the tradeoff between cut depth, cut width, and feed speed.

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: Bob La Londe on October 06, 2013, 20:31:44 pm
I actually bought G-Wizard, (excuse me a lifetime rental license) but accidentally wound up with the wrong software license.  Instead of trying to help me sort it out Mr Warfield was a total snob about it.  When I accidentally used the phrase "my software" he really seemed to get rude.  I removed "his software" from my computer, and contacted my credit card company.  I was one of his beta testers way back when.  He refunded my money and I will not waste my time again.  Sad, because I felt it was pretty good software. 

I do have a licensed copy of ME Consultant as well as the free version from Micahael Rainey.  ME Consultant is ok.  Even the free version.  Its just very conservative.  (Note:  The free version is no longer available from Michael, but it can be found on some software download sites.)

I will probably buy a copy of HSM Advisor sooner or later.  HSM Advisor and FS Wizard are opposite sides of the same coin.  FSWizard is web based and free to use, and HSM Advisor is standalone PC based but costs.  I have found that FS Wizard is quite good, but very aggressive.  If you put in all the setup data it asks for, use coolant or lubricant  when you should, and have a fairly rigid machine you can make all the cuts it calculates.  Its also got a pretty decent material database built in and calculates for different tools, geometry, coatings, and even machining types like milling, drilling, and turning. 

I've also found zero-divide (the author of FS Wizard and HSM Advisor) is quite easy to work with.  He also has a free and a paid version of FS Wizard for the Android Market.  When I am doing a quick simple job using the Mach 3 Wizards I'll often double check my numbers using the FS Wizard cell ap rather than walk in the office and use the CAD/CAM computer.  I've got 4 FS aps on my cell phone, but FS Wizard is the only one I use anymore. 


What would be cool regardless of the tool is a direct interface from something like HSM Advisor to drop the numbers back into CamBam rather than manually entering them one at a time.  Caluclate a cut using all of your parameters, step over, DOC, stickout, etc, and then click OK to send all of the appropriate numbers to the MOP you are working on. 

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: EddyCurrent on August 18, 2014, 09:53:02 am
New link for whitneytool, they changed it since the OP's link

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: Andrew587 on August 26, 2015, 03:44:52 am
Define a MOP and you'll find the calculator if you right-click on it.
I just learnt something. Thanks.

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: MrJTJinx on October 29, 2017, 19:30:59 pm
Hi everyone,

I'm trying to get my head around feeds and speeds, I have 3 problems.

1, Most the formulas and instruction on the interweb are in american/Imperial measurements.
2, My machine is only capable of 6000 RPM and 500 mm/min feedrate
3, my cutters are not necessarily from reputable suppliers with accurate data tables

On machinist forums you get grief for not knowing where to start and not wanting to start by ramming a tool into stock or even worse the bed at 10k RPM - so we ask

I can use the calculators and can use formulas, what i'm not good at is math and trust in the validity of the answer which may actually be correct even if its scary RPM and feed rates.

My uncertainty could easily be answered if some kind individual would kindly explain how to convert unrealistic feeds and speeds into something my machine can handle, OR help me understand how to transpose the formulas so that i can calculate an appropriate feedrate at lower speeds.  I'm sure its impossible as old milling machines and CNCs from the 1960's didn't run much faster than 7000 RPM, unfortunately all the new tooling in catalogues is running at 10K + speeds.
SFM's and m/min for materials seem to differ between different sources which also does not help when using the feed and speed calculators, the properties of materials do not change much from their ANSI/BS standard so why so many different examples.
I'm in the process of learning yet another engineering discipline, be it teaching myself.  The colleges around where i live barely offer engineering courses let alone adult learning night classes - Remember there is a huge skills shortage, so we will fill the gap with ?, that's right nothing.
My machine is an old Elliot 181 Milling machine which i have lovingly converted to a CNC Its not completely calibrated but within 0.1 mm and runs like a dream, i'm trying to mill a 12 mm deep 6001 aluminium block (75 m/min) my spindle is set for 6100 RPM (ok its 900 short of max, scary first job and all that) I have a 2 flute 3mm HSS end mill and wish to cut 3 mm deep slots to make a vacuum chuck. I have a tool catalogue just to get a ballpark figure for a HSS 2 flute 3mm end mill which gives me an ideal setting of 11000 RPM ,250 mm/min feed, 105 m/min Surface speed for Alu, and 0.011 chip load.  This is very informative and the Cambam calculator is pretty damn close.
here is the problem i mentioned earlier how to manipulate feed and speed to account for machines max RPM.
I would be milling like a realun if my machine did 11k RPM. I have not even got started on WOC and DOC yet, no bloody idea how to calculate these babies.  £60 for FSWizard or more for CNC cookbook  is way out of most's budgets.  Considering this is taught to those young enough and fortunate enough to have covered it at college, why is there naff all educational material available available even on google.  I'm going to get Alexa just so i can get into philosophical debates with it.  Like i said help would most definitely be appreciated even if its too late to stop me going mad.

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: lloydsp on October 29, 2017, 19:40:08 pm
We're lucky that feed rates and RPMs are linear in relationship.  If (say) your calculations call for 10KRPM at 1M/minute, at 5KRPM, the appropriate feed rate would be (approximately) 0.5M/minute.

I, personally, cut 'slow'.  I use coolant, and typically get cleaner cuts with fewer cutter breakages if I "just take it slow".  So I use feed rates usually quite a bit below what the tables will call-out.  I will also use smaller depth increments than the tables call for.  But I get good results, with less worries than at the optimum table rates.

They are, after all, 'optimum rates for productivity', not so much 'comfortable' rates.


Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: MrJTJinx on October 29, 2017, 20:42:33 pm
Hi LLoyd,
Thanks for your reply.
I had read of this method being adopted by someone on the model machinist forum, having you confirm the same calculation gives me some confidence to just go for it. 
Its interesting that you didn't mention any magic math or formula to manipulate RPMs and feeds, this also gives me  the impression it was not a stupid question.  I will be impressed if someone points to a definitive formula (in Metric).
I did try a cut at 5500 Rpm and 200 mm/min 0.7mm DOC 3mm WOC which should have been 50% of optimum,  I heard a wonderful ping sound.  To be fair the stick out was huge, the cutter i tried had a 20mm stick out, the 45 degree rake on the tool before disaster said it all.  I reduced the feed to 68mm/min, for the life of me i cant even remember how i got to that figure but it worker really well if not good enough for industrial standard.
all went well until my GRBL controller froze, i sent a +Z move to extract from the work and ended up drilling down into the bed through the work. Bummer.  The Invert axis setting in my config got overwritten ? obviously still some EMI gremlins in my system.

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: Garyhlucas on October 29, 2017, 22:26:57 pm
A couple of things. If you aren’t breaking cutters you haven’t passed the optimum feed rate! This might sound a little crazy but the faster you feed without breaking a tool the longer the tool lasts, sometimes a LOT longer. Each time the cutting edge enters the material it wears a little. Faster feed means less entry into the material.

I once took over a job in the middle. The previous operator had worn out 4 cutters already and the job was going really slow in cold rolled steel. I quickly broke 3, the 4th finished the job in half the time! That saved way more than the cost of some 1/4” end mills.

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: dh42 on October 29, 2017, 22:27:03 pm

Math are not complicated.

RPM = 318 * Surface speed(m/min) / Tool Diam(mm)

so for a SS = 60m/min (steel 35CD4 - carbide tool) and a tool = 12mm

318*60/12 = 1590 RPM

The feed rate F (mm/min)

F(mm/min) = Fz(mm)*Z*RPM

Z = number of flute of the tool
Fz = tooth load in mm
RPM the calculated RPM above, or if the spindle can't reach the calculated speed, use the max speed usable.

ex: tool Ø 5, 2 flutes, alu machining: SS = 150 m/min, Fz = 0.04mm

RPM = 318*150/5 = 9540 RPM ... too much for your spindle.

we take 6000 as RPM to calculate F

F = 0.04*2*6000 = 480 mm/min

Except for micro tools, don't use a Fz value < 0.01mm

I've an excel sheet that do calculation in both direction (Surface speed or RPM maxi and Fz or F maxi) but it's written in French, but if you want to try it I can help you to translate it in English and explain how use it, and you can modify it as you want for your own use.

Black cells are those where you can enter data for calculation.

The sheet is unlocked so you can change any cells you want ; if you lock it, only black cells can by changed (so formula are protected)

First enter tool diameter (Ø Outil), Vc (surface speed) Z and Fz ; you get the result in the cells below for RPM and F

if the calculated RPM is to high for your spindle, enter an RPM value in the Rotation cell at the right side, and click on the SET button at it's left side, a new Vc is calculated and copied in place of the Vc you have entered and the other value are calculated again.

You can do the same with F (Avance) if the value is too high after the new RPM as been calculated, this time, it's the Fz that is calculated.

Depending of the machining, Surface Speed and Fz can be altered, so:

Fz decrease when the tool is long compared to is Ø

Fz and surface speed decrease when WOC increase

Fz decrease when DOC increase, but SS do not change

Those last alterations are not (yet) taken in account in my excel sheet.


Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: MrJTJinx on October 31, 2017, 18:23:16 pm
Thanks David,
I have downloaded your excell calculator and dusted of my secondary school french Tricolour book.
I'm trying it out as we speak
many thanks Jason

Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: MrJTJinx on April 11, 2019, 22:17:43 pm
For novices and newbies

We buy cheap cutters from Ebay and other unknown sources.  Hell even my local steel stockist and tooling supplier does not provide any information with the cutters.

We are terrified to run the tool in a machine at 6000 Rpm its seriously damaging to our health or at least could be.   The grumpy old grandfathers love to preach about feeds and speeds and leave us all bewildered by the vagueness of such a variable subject matter.

Most of us can tell the difference between High speed steel (HSS) Cobolt, carbide, tin coated etc
but finding out what the feed per tooth (fz) or Rpm for a cutter with no data is like the proverbial watering your snake into the wind.

There is a simple solution which really will help new starters.  If you have an 3/8 (9mm) 3 fluted Endmill cutter with no information and you have a fair idea its high speed steel, take a look at any tool suppliers catalogue  for HSS tools   and look up your 3 flute 9mm cutter.  There will be a tool table with different sized tools listed and generally some indication as to the materials the tool is suited for.  Looking at the table you will find information like Slotting or Profiling profiles, material & SFM (removal rate), feed, speed and chipload.  Is this not all the information you ever wanted to know and asked on numerous forums.  The Cambam Feed and speed calculator is fine, bit of a bug bear of mine is that you cant look at the calculator until you have created a mop.  If you cant verify the values you see from the calculator its hard to trust yourself, the manufacturers tool data is worth its weight in gold.

say you have a tool which is higher spec, perhaps coated or solid carbide, guess what they will cut better than HSS so the basic settings will still work fine you will simply not be using the cutter to its full potential - means it will probably last even longer.

You are now a rocket scientist.
And will not kill yourself

There is still a lot to be said for destroying tools, many machine shops will be using one if not more tools per job, they will be maxed out and on occasion will self destruct.  Pushing hard is not a sin, if you get everything right you will see a steady stream of chips flying off the tool like the spray from a water cannon.  Now that's making chips.

Use guards and eye protection and stop worrying about a piddly $5 end mill