CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
December 11, 2017, 11:13:39 am


Login with username, password and session length


Pages: [1] 2
  Print  
Author Topic: Speed & Feed Primer ~ Long & Boring & Essential  (Read 31948 times)
Doanwannapickle
Storm Trooper
***
Offline Offline

Posts: 100


View Profile
« 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:
http://www.whitney-tool.com/html/calculatorSpeedFeed.html

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,
Walt

Logged
mrbean
Administrator
Storm Trooper
*****
Offline Offline

Posts: 213


Web Jedi


View Profile WWW
« Reply #1 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...

Cheers.
Regards MrBean.

Logged
10bulls
Administrator
CNC Jedi
*****
Offline Offline

Posts: 2041


Coding Jedi


View Profile WWW
« Reply #2 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?


* the-finger-of-doom.jpg (255.22 KB, 1024x763 - viewed 939 times.)
Logged
servant74
CNC Ewok
*
Offline Offline

Posts: 32



View Profile
« Reply #3 on: November 08, 2008, 01:54:29 am »

http://www.onsrud.com has another good speed/feed calculator that includes woods and MDF

It is down from 11/7-11/10/2008 for maintenance.
Logged
MuellerNick
CNC Ewok
*
Offline Offline

Posts: 25


View Profile
« Reply #4 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

DOC:
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.

Nick
Logged
macpod
CNC Ewok
*
Offline Offline

Posts: 12


View Profile
« Reply #5 on: December 12, 2012, 04:27:44 am »

I have found this speeds/feeds calculator to be convenient:
http://zero-divide.net/index.php?page=fswizard

Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3023


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #6 on: October 03, 2013, 16:13:10 pm »

I have found this speeds/feeds calculator to be convenient:
http://zero-divide.net/index.php?page=fswizard

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. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3023


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #7 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. 



* HSM Cut.jpg (125.61 KB, 735x1306 - viewed 638 times.)
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Bubba
CNC Jedi
*****
Offline Offline

Posts: 2277



View Profile
« Reply #8 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. 

Bob,

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.
Logged

My 2Ē
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3023


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #9 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.
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Jeff_Birt
CNC Jedi
*****
Offline Offline

Posts: 821


View Profile
« Reply #10 on: October 05, 2013, 03:25:12 am »

Quote
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: http://cam.cad2design.com/camworks/demos/82158/SURFCAM+Velocity+Metal+Cutting+Video+Stainless+316 . Here is a neat high speed video showing the chip formation: http://cam.cad2design.com/surfcam/demos/82153/SURFCAM+Velocity+high+speed+metal+cutting+video .
Logged
pixelmaker
CNC Jedi
*****
Offline Offline

Posts: 1576


View Profile WWW
« Reply #11 on: October 05, 2013, 11:57:11 am »

Why you donīt use the feed/speed calculator in Cambam?
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3023


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #12 on: October 05, 2013, 23:40:06 pm »

There's a feed speed calculator in CamBam? 

I gotta find that. 

Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3023


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #13 on: October 06, 2013, 14:53:07 pm »

Why you donīt 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. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
blowlamp
CNC Jedi
*****
Offline Offline

Posts: 1183


View Profile
« Reply #14 on: October 06, 2013, 15:02:40 pm »

Why you donīt 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.



Martin.
Logged
Pages: [1] 2
  Print  
 
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.19 | SMF © 2013, Simple Machines

Valid XHTML 1.0! Valid CSS! Dilber MC Theme by HarzeM
Page created in 0.153 seconds with 19 queries.

Copyright ÂĐ 2008 HexRay Ltd. | Sitemap