CamBam

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:
http://www.whitney-tool.com/html/calculatorSpeedFeed.html (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



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...

Cheers.
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
http://www.onsrud.com (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.


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

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


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:
http://zero-divide.net/index.php?page=fswizard



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:
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. 


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. 

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.


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
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 .


Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: pixelmaker on October 05, 2013, 11:57:11 am
Why you donīt 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 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. 


Title: Re: Speed & Feed Primer ~ Long & Boring & Essential
Post by: blowlamp 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.


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

http://www.cambam.info/doc/dw/0.9.8/cam/SpeedsFeeds.htm

++
David


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 cnccookbook.com.  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. 

ALL OF THAT ASIDE:

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

https://www.whitneytool.com/SpeedAndFeedCalculator.aspx


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.