CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
December 11, 2017, 11:15:15 am


Login with username, password and session length


Pages: 1 [2]
  Print  
Author Topic: Speed & Feed Primer ~ Long & Boring & Essential  (Read 31953 times)
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 4783



View Profile WWW
« Reply #15 on: October 06, 2013, 15:05:22 pm »

Hello,

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

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

Posts: 3023


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #16 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. 
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
pstemari
Storm Trooper
***
Offline Offline

Posts: 133


View Profile
« Reply #17 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.
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3023


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #18 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. 
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
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 3253



View Profile
« Reply #19 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
Logged
Andrew587
Droid
**
Offline Offline

Posts: 73


View Profile
« Reply #20 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.
Logged
MrJTJinx
CNC Ewok
*
Offline Offline

Posts: 20


View Profile
« Reply #21 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.
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7209



View Profile
« Reply #22 on: October 29, 2017, 19:40:08 pm »

Jinx,
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.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
MrJTJinx
CNC Ewok
*
Offline Offline

Posts: 20


View Profile
« Reply #23 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.
Logged
Garyhlucas
CNC Jedi
*****
Offline Offline

Posts: 1027


View Profile
« Reply #24 on: October 29, 2017, 22:26:57 pm »

A couple of things. If you arenít breaking cutters you havenít 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 1/4Ē end mills.
Logged

Gary H. Lucas

Have you read my blog?
 http://a-little-business.blogspot.com/
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 4783



View Profile WWW
« Reply #25 on: October 29, 2017, 22:27:03 pm »

Hello

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 ō 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 (ō 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 ō

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.

++
David

* Calc_Vcoupe2.02.zip (14.58 KB - downloaded 18 times.)
« Last Edit: October 29, 2017, 22:41:14 pm by dh42 » Logged
MrJTJinx
CNC Ewok
*
Offline Offline

Posts: 20


View Profile
« Reply #26 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
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 0.126 seconds with 19 queries.

Copyright © 2008 HexRay Ltd. | Sitemap