Is there an Html Link (or freeware of somesort) that can allow you to input your differant conditions (Cutter #Flutes, Cutter material, stock material, side milling plunging, drilling or whatever)
and output a rpm and feed rate?
If not is there recommended software that specializes in this. I use Pro Manufacture.
I've obtained a Machinist Handbood (that is almost as thick as it is wide) but I don't have the patience for it. Maybe there is another text that is a bit more specialized in what I want.
Thanks
Tony

You might try getting hold of a Speeds and feed slide rule calculator. Iscar makes one that is really nice. All you need to know is your SFM, cutter dia, #flutes and all the calculating is done.

I started using a Shareware progam in 1995 that was written by Micheal Rainey called ME HELPER. Ironically 7 years I bumped into Michael on-line in a few of tthese forums. He has posted his updated version of the program at www. cnc masters unleashed.com for free downloading (leave out the spaces in the url). Just do a search for it there.

Xeno:
There is a program called Machinist's Toolbox that has speed/feed calculations for many situations programmed in. They have a free Lite version. See it at:
http://www.ptcam.com/toolbox.html

robotic regards,

Tom

There is a really nice program out there alled "Machinist's Tool Box" written by Tim Markowsky. It has a library of materials that allows you to add or remove materials as needed. Tons of other features. I know people that have been using it for years and swear by it. You can contact me if interested and I can give you all details and prices.
Regards,
Sorin

you can go to www.shopfloorautomations.com they offer the full blown "Machinist's Tool Box"you will also be able to see some of the features and screen shots of whats offerd..

If you want it I will see about getting a discount for being a CNCzone member.

Sorry about my miss posting folks I have restated the post to be proper for this board.:)

I have already talked to Tim and I can offer the discounted prices if interested. I wouldn't publish them here since this is not a place for soliciting busines....
Regards,
Sorin

Onecnc XP series software has exactly what you want. You do have to fill in the tool and materials chart one time, or I should say, edit it to suit your preference/experience. :)

Originally posted by HuFlungDung
Onecnc XP series software has exactly what you want. . :)

LOL LOL... HU This reminds me of the I love Lucy episode: "The answer to all your problems is in this little bottle- vitamina vegiman". Oh vell, we know what was in that bottle (or better yet, I KNOW who sels it.........) and I for one wouldn't buy it from him..
Best regards,
Sorin

I had made a few suggestions how this can be done in this post:

http://cnczone.com/showthread.php?
s=&threadid=203#post739

I have used the Machinery Handbook 19th edition for many years. But I keep most of my calculations as simple as I can get away with. And to make it even simpler I had written for myself BASIC programs to do these calculations.

The 25th and 26th editions have information on also how to estimate feeds and speeds for tool life. Which I have found of interest. But have not at this time worked out a simpler way to do those calculations. So I haven't yet bothered.

Basicly the SFPM dictates tool life for the most part. As a rule of thumb so to speak, I suppose the 80% rule double the tool life.

Currently most feed and speed programs that I have seen ingnore tool length. My personal programs do not. Shorter tools can run faster than longer tools. And CAM package calcuations also ingnore changes in width and depth of cut in the calculations as well as horse power needed at the spindle for a given RPM.

So I am not real fond of the ISO9000 CAM requirements. Fortunately for me I am not under such restrictions when it comes to estmating feeds and speeds.

Hey Mortek,

I second Xeno's suggestion, but add that if you can't find an Iscar sliderule, Kennametal has one as well. The Kennametal version also calculates horsepower, force etc.

I created a spreadsheet in Excel using the basics from the sliderule, and inputting variables that are dictated by the job or machine, ie; material, tool, rpm's etc. I have been thinking of refining it to include force and horsepower to maximize the metal removal rate of my programs instead of just "that looks right".

Adam

Hey,

Once of the first things I did when I started G code programming was sit down and write a tight little speed and feed calculator. One thing I did was make it so it stays on top of all the windows so you don't have to go looking for it everytime you want to use it.

Over the last few years I've imporved it and added tapping feed rate calcs, and drill point length calcs. Lately, I've been tweaking it up in order to market it for ultra low cost - anyone interested in beta testing?

I'm willing to help you test it and offer some feedback as needed. Good Feed/Speed calculation is essential to making good parts effieciently.

Originally posted by chleborad
...Lately, I've been tweaking it up in order to market it for ultra low cost - anyone interested in beta testing?

I'll run it thru the wringer for you also.

'Rekd teh entomology

Originally posted by Rekd
I'll run it thru the wringer for you also.

'Rekd teh entomology

Talk about team players:p
PEACE:D

I would not be adverse to beta testing.

I have written three different feed and speed calculators. The current ones (two) I use on a TI-86 calculator. And are for end milling.

I also have written some for tapping for calculated pull out. Those will run in Qbasic.

Also wrote for drilling, reaming, core drilling and spade drilling. But only the drill, reaming and core drilling have been transated to the TI-86.

A triangle solver that can be used to solve any triangle. That one can be downloaded from ticalc.org (http://www.ticalc.org) That is the TI-85 version. But will load and run on a TI-86.

My rough milling program askes for the following:

First you slect whether you will be making a linear cut, ID cut or OD cut.
(If ID or OD asks radius.)
Next asks for the material SFPM (Surface Feet Per Minute.)
Then it asks for a material cubic inch per horse power rating.
Then,
Side depth of cut.
Z axial depth of cut.

End mill diameter.
Lenght of flutes.

HSS or carbide.
Number of flutes.

Maxium spindle RPM.
Maxium feed rate.

Program gives calculated RPM.
Asks what the available horsepower at the spindle at that RPM.

The program then gives as output:
RPM
IPM
IPT

O.K....

I have a release package ready to go. People who are interested should send and email to:

CNC@Chleborads.com and I will reply with a link to the download location.

Thanks

Speed/feed calculators, bwhahahaha.

I just make it up as I go along :D

Originally posted by M@T
Speed/feed calculators, bwhahahaha.

I just make it up as I go along :D

+1

If it's screamin', crank it up. If it breaks, back 'er off. :cool:

'Rekd teh Destroyer

LoL, keep the chip thickness less than the cutter radius and you'll be okay, Matt :D

Originally posted by HuFlungDung
LoL, keep the chip thickness less than the cutter radius and you'll be okay, Matt :D

LoL, that's what the sales rep keeps saying. I just shrug and walk away.

'Rekd teh If it gets hot enough, shouldn't it just melt it's way thru...? :eek:

Originally posted by M@T
Speed/feed calculators, bwhahahaha.

I just make it up as I go along

Thats what you call years of experience:p :p

PEACE:D

Hey Xeno,

Why don't you consult the manufacturers recommendations for the inserts/cutters that you are using. In my experience, there is no single speed and feed for any given situation anymore. Different geometries, coatings, substrates, workholding......Too many variables.

My advice is to choose the cutter based on the forces that the setup and machine can withstand. In other words, if you are cutting 316SS for example, and your depth is 1/2", you are using a 1" two flute indexable, but you don't have much to hold on to, then you might choose a slower tougher grade (like Iscar 328), and run with coolant. If you have a good hold, then something like Sandvik has a cutter that is much faster and you can run it dry.

My point being that the speeds and feeds data that you get from Machinery's Handbook and the like are outdated (including the 25th edition). If you don't get enough chip, it will cost you in inserts and time.

Again, just my two cents worth.

Fish

When I was an apprentice AHC (Automatic Hardinge Chucker) operator, and setup trainee. The machinist that was showing me the setups, told me he was taught, turn it up till it catches fire, then back it off.

The old timer general machinists, scoffed, that I would even calculate my feeds and speeds. Or that I would even use the
Machinery Handbook. Saying that it is for engineers, and that
engineers don't make good machinists.

BTW, it is always best and recommended, that when automatic feeds are used, they should be calculated.

Often when doing some cuts for tooling, I'll only calculate the RPM, but hand crank the feed, just like on a manual mill.

Proper chip formation, should be curled like a 6. A heaver feed will give a chip like a C.

On the Automatic equipment, I would measure the thickness of the deformed chip and adjust the feed accordingly.

Typically I find my calculated feeds are faster and much better than the guess and by gosh feeds and speeds by other operators and want to be programmers.

Often, more recently, I have had operators complain, that the feeds are too fast. And have some in, time past, not only reduce the roughing feeds (which some times is needed.) But needlessly reduce the finish feeds too.

A number of years ago, when I programmed Bridgeport Series II mills. The RPMs were to be set by the operator. One newer operator thought he would be smart and NOT use the RPM that was noted in the program. That tool turned cherry red. He didn't do that again. LOL

For a really nice, free program to make machining calculations, see my post in "Product Announcements" (ME Consultant 2.0).

I've also got a TI 86. Would your program work in my calculator too?!:D

Xeno,

Check this out, hope it helps a bit:

http://www.hougen.com/tech_tips/speeds/speed.html

Try out this one. It free-ware.

http://www.cimco-software.com/index-main.html

There are so many variables to this formula that your most reliable tool will be your personal experience. I believe that the best and least expensive way to gain a working knowledge of speeds and feeds is to understand tooling material types vs workpiece material types and how they translate into surface feet per minute (SFM) and chip load per tooth (CL) if that makes sense. My personal preferences are for instance:

Mild Steel:
Drill-(Dia-3/16-1in)
HSS Spot Drill: 90 SFM/.003 CL
HSS: 55 SFM/.0015-.004 CL
Cobalt: 90 SFM/.002-.005 CL
Solid Carbide: 240 SFM/.0025-.006 CL
Insert Carbide: 300 SFM/.0025-.007 CL

End Mill-(Dia:3/16-1in)
HSS: 90 SFM/.0005-.004 CL
Cobalt: 150 SFM/.0007-.005 CL
Solid Carbide: 220-280 SFM/.001-.006 CL
Insert Carbide: 300-400 SFM/NA-.007 CL

You want to reduce surface footage when working with harder/tougher workpiece material but dont monkey with the chipload too much. Too little chipload is just as bad for the tool as too much. You need to look at the chips you are producing too. Generally speaking, if they are ragged and dark blue or at all black then you most likely have too much RPM vs feed. If chips are clear or natural looking (like the metal you are machining) then you could do with more feed. Normally, a brownish or gold-colored chip is ideal. This usually means that most of the heat generated during the cutting process is being carried away by the chips. Exactly what you want for long tool tool life. Some tool materials that is. HSS would do better machining at a natural chip color state while a coated carbide almost demands to be pushed to achieve optimum cutting conditions.
Then there are some harder and more exotic metals in which chips will appear irradescent when cutting conditions are right. Variables are truly endless. Workpiece rigidity, tool length, depth of cut, radial cut, bla...bla...bla...
I'm tired and my grandma is invading my privacy so I gess its time to go. I hope I helped more than I confused, and I know my surface footage is conservative but thats just my style.
Good luck

I forgot to mention to get one of those machining calculators (slide rule) and learn how to use it. Tool salesman hand them out by the pile. It also helps you commit variables to memory better than a computer program that does it all for you.

Wow, what a source of info on here!!!

I was just looking for some info too!.

Im not an experienced CNC programmer, I was an apprentice on manual machines and now Im an office dweller needing to program!.

All I was looking for was a simpler rule of thumb like:

Mild Steel, general 6 tipped cutter roughing cycle + ??rpm & ??feedrate, ?? cutdepth.
As above, 25mm ballnose, ??rpm, ??feedrate.

you know, a kind of basic, everyday range you cant go wrong with!!! lol. No cut per flutes or whatever! lol, just 'common sense' values!! hahahah. nah, Im not that bad, but there is conflicts of 'its too fast it ruining tips and shaking the whole machine' and "its not cutting enough you will '****' the tips up!"

Well, thanks for the info so far, Ill have to try and figure it all out.


Cheers :)

Sirius.

Sirius,

It's not common sense until you've practised using the formulas for a while. If you apprenticed already, you should be halfway there :)

Yeah, Ill have to get my maths cap on!!!!:eek: :D

When I was apprentice, I used to look and listen and tweak till i was producing a good finish on the old manual machines.......it was oh so simple then! lol. Now, with a new 'machining centre' and being located off the shopfloor, the values can be hard to imagine in 'reality'. I should have payed more attention to what the readouts were giving me at the time!!.....but saying that, you could only take cut depths of about .75 of a millimeter on those old things whereas you can cream off 8mm per cut on this baby!! lol.

Im going to save the page on a floppy and take it into work. The chips usually coming off the machine are deep blue (due to feedrates recommended off the CNC operator)....I always thought it was going too fast, becuase tips wouldnt last, so at least if I start to get a balance back and the recommended swarf colour, I'll be laughing! :)

Thanks,

Sirius.

Unless you are machining with coolant, the chips are normally a deep blue color when machining steel. So I am afraid that is not too useful of an indicator any more.

One thing to watch for with carbide is sparking at the tool tip: if it sparks once in a while, you are going too fast. This would apply to machining dry, though.

Resist the temptation to overspeed and underfeed, which is a common fault of newbies. Some guys will run the snot out of the spindle and barely be moving. Tool life really amounts to so and so many chips, and if you use up that number on whispy little chips, you are not going to get much done before its time to change the insert.

Well, Ive yet to download some of the software mentioned earlier, but I had a look in the back of the Tooling Catalogs today armed with a calculator and a rusty remeberence of algebra........Jeezuz its compliacted!!!!!!.

What is the difference between surface speed and feedrate? They are given different 'labels' in both catalogs I looked in.

Why does the catalog give me the average chip thickness (ie .12mm) and why on earth would I need to know this? - it just falls in the scrap tray.

For example I tried to calculate a 20mm x r3.5 tip "Hognose" cutter for ToolSteel (BD2). The catalog reckoned a cut depth of 2mm (but the machine can only handle 1.25mm cuts) and an 8mm stepover. After gyrating through the mathematical hoops, I got a "Surface Speed" of approx 150 Meters per Minute.

Now, in the catalogue it says ( i think) to find the RPM.... Times the Surface speed x 1000, divide that by 3.142 x Dia of cutter.......which gave a RPM of about 2830!!! At which one guy said the tool would just disintegrate inbetween laughing, lol.

I worked out a feedrate per tooth which came at something like 0.51mm/minuite........how does this help me? I need a overall feedrate.

The job is a block of Toolsteel, roughing cycle with the above cutter on an old 'retrofit' style CNC that can usually only handle 1.25 cuts with that cutter without vibrating the head!!! lol.

There seems to be too much information required in the formula's than I know what to do with!! I just wanna know how fast I can go with tipped cutters on ToolSteel with 1.5mm cuts and what rpm that would be! hahah.

We have two old CNC's and a new 'Machining Centre' thats more robust, So I need to suss out what to do with each machine.

Im going to have look at the programs mentioned, but I think the ones I tried last time are only for endmills/slotdrills and I dont think this helps me with using the tipped tools, or working out for tipped ballnose or face mills.


Cheerio

Sirius.

Grasshopper ;) :D

Surface speed = velocity of the largest cutting circumference of your milling cutter. This is a factor of the type of tool, whether it be high speed steel, plain carbide, coated carbides of various types.

Feed rate in terms of chip thickness is the most basic fact about the tool's capabilities, while assuming that you are already running it at the correct velocity (surface speed).

Take the rpm of the cutter * number of teeth * chip thickness = feedrate in inches or mm per minute.