CAMheads CNC Router Forum By: CAMaster CNC

Go Back   CAMheads CNC Router Forum By: CAMaster CNC > New CNC Setup. > materials and bits, collets, etc.

Reply
 
Thread Tools Display Modes
  #11  
Old 06-05-2015, 11:38 AM
Gary Campbell's Avatar
Gary Campbell Gary Campbell is online now
CNC Tech & Trainer
 
Join Date: Dec 2012
Location: Marquette, MI USA
Posts: 2,741
Default

Javier...
Its nice to put this "stuff" out to someone that understands. While you are at it, don't fall into the "I just throw 1000 inches per minute as a feedrate and let the controller take over" trap.

We all know a bicycle is slower than a corvette.
But what if they race in a gymnasium?
What if they must stay on the "line"

All the speed and acceleration of the Corvette will be useless when accuracy is required. Same goes for CNC machines, in many cases they will cut at lower quality when accelerating.

You will seldom get quality cuts when you exceed 1 inch per second (60 ipm) for each inch of geometry size. This will also be reduced by number and distance between nodes in the geometry. This means you may be able to pocket a postage stamp size geometry at 60 ipm, but you cannot expect to vcarve similar sized graphics at that speed.
__________________
Gary Campbell
CNC Technology and Training
The Ultimate Woodworking Machine
GCnC411@gmail.com
https://www.youtube.com/user/Islaww1/videos

"There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"
Reply With Quote
  #12  
Old 06-05-2015, 07:01 PM
CosmosK CosmosK is offline
CAMaster Owner
 
Join Date: Jul 2014
Location: Fort Worth
Posts: 799
Default

Quote:
Originally Posted by Javierunzueta View Post
In your (all forum members) experiences ...
I'll chime in now that you've opened it up to non-gurus :)

I had a good amount of machine shop experience before getting a Stinger. I never took the time to learn how to calculate speeds and feeds. Everything I knew was from asking people and observing. However, I took it upon myself to get educated on the subject when I bought a machine because the stakes are higher. I don't want to trash the machine, and I've seen enough trashed machines from people using them incorrectly.

RPM and feedrate combine for chipload. There are calculators out there, but I'd advise to find the equations and understand how they work and make your own calculator. For me, there are too many factors to take into account for me to try to learn by testing each combination. I need a starting point, and I don't want to overload the machine, so that's why I do the calculations. Might be overkill (for machining softer materials), but it's how I prefer to learn.

In general, why would you go faster? Time and money. In production, you want to make "in spec" parts as fast as you can.

I've had good luck doing details in hard maple with:
1/8" 2 flute: 6000rpm, 60ipm
1/16" 2 flute: 12000rpm, 30ipm
__________________
2014 Stinger II (SR-44)
1.7 kW Spindle w/ speed control, Performance kit, VCarve Pro
www.cosmos-industrial.com
>Pen Marking Tools
Reply With Quote
  #13  
Old 06-07-2015, 12:07 AM
Javierunzueta Javierunzueta is offline
CAM aster Owner
 
Join Date: Feb 2015
Location: Miami
Posts: 45
Default Taking it slow... Way too slow.

Well, I ran a few tests (See attached pics.)

Unfortunately, it showed somewhat inconclusive results. There was little (if any) difference between 20 IPM and 400 IPM in the grand scheme of things (Other than moderate debris size.) The 10 IPM produced fine dust and SLIGHTLY better quality, but not enough to matter.

I tried my " Diameter (MLCS) " Shank Spiral Downcut Endmill as well as my " diameter " Shank 60 Degree V-bit (MLCS) thus far.

I ran, as you can see, a series of fluted paths from 10 to 400 ips on some " cypress pieces at 12K and 16K RPM.

I must state, the 16K (albeit annoyingly noisier) produced an ever so slightly better cut overall so I'm probably keeping my speed there for most future work. Most cuts were crisp and quite similar with the only TRUE factor being the wood grain itself.

For sanding-free no-tearout smooth finish cut, the 16K at a staggeringly slow 10 IPS produced the cleanest look.

No burn marks anywhere at any speed/feed tested.

The Downcut spiral EM surprised me at it sliced through " of all three materials at 400 IPM without a hint of slowing down. I love this machine.

The V-bit faired just as nicely. What was absolutely fascinating was when my V-Bit, at the 60 IPM mark, started creating thin slices of wood peel (not unlike a smaller scaled version of my surface planer). I was a bit surprised because all the cuts I made were ACROSS THE GRAIN on purpose to gauge the tear-out. Quite an eye-opener for me.

All in all, the only discernible difference in quality (other than a slightly nicer cut at the turtle's pace) was from the actual wood itself.

I'll make more chips tomorrow. Good night all.
__________________
Javier Unzueta
Stinger 1, FTC, 2.25 PC, Touch Top, Vcarve Pro, PhotoVCarve, WinCNC
Miami, FL.

"I'm a firm believer in learning from my mistakes and failures, but I prefer to learn from others'!"
Reply With Quote
  #14  
Old 06-07-2015, 10:09 AM
Terry Williams Terry Williams is offline
Cobra Owner
 
Join Date: Mar 2012
Location: Naples, FL
Posts: 197
Default

Here is a resource for some very handy links:

http://www.precisebits.com/library.htm

I spent many hours late at night googling various topics like wood hardness, Speeds & Feeds and virtually anything that had to do with CNC routing. This list is now the first place I go when I have a question.

The process for determining correct speed and feed in the following link works:

http://www.precisebits.com/tutorials...s_n_speeds.htm

If you are producing a part that you will make many copies of, this effort will be repaid many times over, but for a one-off, the payback isn't obvious, since you do have to invest some time and effort in the process.
__________________
Terry Williams
Cobra 510 with Recoil
Reply With Quote
  #15  
Old 06-07-2015, 11:05 AM
rcrawford rcrawford is offline
Cobra Owner
 
Join Date: Dec 2011
Location: Alberta
Posts: 2,194
Default

You will get much better results by carefully choosing the woods you cut! Maple, cherry, and walnut seem to give me the best results.

The next factor is the bit. If I want a better cut, I often choose a larger diameter cutting tool. For the best edge finish, I use a 3 flute 1/2" low helix downcut. 14000rpm and adjust the feed speed to get the best finish.

Cutting 'conventional' vs 'climb' will also affect the cut quality. Usually conventional will give the best cut, but will also give the most tear-out. When the finished edge is important, I will often offset .01 and cut climb in a couple passes, then go back with no offset and cut conventional in a single pass. This gives a very clean edge (again, depending on the grain).

Cut quality is often higher when you increase the rpm and slow the feed speeds, but if you take it too far you will burn the wood. Cherry and purple heart are the worst for this, and its common on the corners where the feed slows down.
__________________
Russell Crawford
Cobra 408 ATC with recoil
Alberta, Canada
www.cherryleaf-rustle.com
Reply With Quote
  #16  
Old 06-07-2015, 12:27 PM
Javierunzueta Javierunzueta is offline
CAM aster Owner
 
Join Date: Feb 2015
Location: Miami
Posts: 45
Default Thanks...

Terry,

Thanks for the links. There was quite a good bit of information on it. Coincidentally, I was looking for a source for micro-bits for my stinger so this site was perfect.


Russell,

I've also had the same results with conventional vs climb cuts. I've been using that technique (offset climb and final conventional cut) recently and am thankful for the confirmation. I'm most definitely adding a 3 flute " low phlox dc to my arsenal. Thanks again for the advice.
__________________
Javier Unzueta
Stinger 1, FTC, 2.25 PC, Touch Top, Vcarve Pro, PhotoVCarve, WinCNC
Miami, FL.

"I'm a firm believer in learning from my mistakes and failures, but I prefer to learn from others'!"
Reply With Quote
  #17  
Old 06-07-2015, 12:33 PM
james mcgrew's Avatar
james mcgrew james mcgrew is offline
Administrator, (MOD, KOTR)
 
Join Date: Sep 2008
Location: ridgeway sc
Posts: 6,758
Default Moved to tech thread

Moved to a more technical thread subject
__________________
James McGrew
CAMaster ATC 508
The principle of Measure twice cut once has not been replaced by a CNC

www.mcgrewwoodwork.com

https://www.facebook.com/pg/Mcgrew-W...=page_internal

Camera 1 ATC Closeup !
https://video.nest.com/live/esNTrZ
Reply With Quote
Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump


All times are GMT -4. The time now is 04:26 PM.


Powered by vBulletin® Version 3.8.4
Copyright ©2000 - 2018, Jelsoft Enterprises Ltd.