Feed rates... what am I missing?

Talk about all things CNC

Feed rates... what am I missing?

Postby secretspy711 » Tue Jul 08, 2014 10:55 pm

According to this: http://makezine.com/magazine/cnc-routing-basics-toolpaths-and-feeds-n-speeds/

The formula for calculating a basic feed rate is: ChipLoad x CutterDiameter x NumberOfFlutes x SpindleSpeed = FeedRate

So then I go hunting for appropriate chip load numbers. I found that the chip load for Acrylic (for example) is .003"-.005", here:
https://www.vortextool.com/images/chipLoadChart.pdf

So plugging that in, and assuming some other numbers (.125" cutter, single flute, 18krpm) I get:

.003" x .125" x 1 x 18000rpm = 6.75. Note that if you carry the units through, you actually get (in^2/minute).

WHY THEN, does this site recommend 75-100 ipm?!
http://www.engraverssolutions.com/PDFs/tips&tricks-routing_acrylic.pdf

To make matters worse, if we go back to the chip load chart, it gives the feedrate formula as:
FEED = RPM x number of flutes x chip load
notice that cutter diameter is not included this time, so plugging in the same numbers results in 54 inches per minute.

Using the stock altocraft spindle that came with my shapeoko, I've been able to cut most wood comfortably at about 40 ipm, using a DOC of half the cutter diameter (.0625"). If I want to cut at .125" deep then I definitely have to slow down the feed rate to something like 20 ipm.

What am I missing here? Is my spindle simply not powerful enough to get up to these feed-rates without bogging down? I can't possibly cut at 75-100 ipm, at least not at .125" depth with a .125" cutter!
Shapeoko 2 #5510: 1200 x 500 mm, Makita RT0701
secretspy711
 
Posts: 175
Joined: Thu Jun 12, 2014 7:55 pm
Location: Colorado

Re: Feed rates... what am I missing?

Postby WillAdams » Tue Jul 08, 2014 11:32 pm

The ShapeOko is a machine of compromises. Chip load and feed/speed calculators are intended for rigid machines w/ spindles w/ far more torque.

Lacking rigidity and horsepower, one has to work w/ a delicate touch, taking lighter passes.

This is discussed on the Materials page: http://www.shapeoko.com/wiki/index.php/Materials
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)
WillAdams
 
Posts: 8323
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15

Re: Feed rates... what am I missing?

Postby Auarhau » Tue Jul 08, 2014 11:36 pm

Those formula's are for heavy duty industrial size machines. The shapeoko is not rigid or powerful enough to use those numbers. Reference the wiki for feeds and speeds for various materials, and make your own adjustments according to your machine,endmill and material. It requires some trail and error, and experience. The best procedure for figuring the optimal settings, is in my opinion, the precise bit zigzag test posted by will some time ago.
ShapeOko 2. Nema 17 74 oz·in. GAUPS shield on Arduino Uno. DRV8825 Drivers x4 . Kress 1050 FME-1. Z Acme Screw. Threaded inserts table.
Auarhau
 
Posts: 243
Joined: Tue Feb 25, 2014 8:46 pm

Re: Feed rates... what am I missing?

Postby WillAdams » Tue Jul 08, 2014 11:48 pm

I'm given to understand that the CNC Cookbook folks have a feed/speed calculator which is configurable for horsepower and adjustable for how fast one wants to cut (and by extension, how rigid one's machine is).

The tool which I'd really like to see is a full physics simulator which would take all aspects of a machine into account and calculate optimal feed rates for each path of a given G-code file.
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)
WillAdams
 
Posts: 8323
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15

Re: Feed rates... what am I missing?

Postby UlteriorMotors » Wed Jul 09, 2014 4:12 pm

Here's the thing about chip loads. Yes, most (if not all) resources online are targeted towards large, stiff machines. However, that's not to say they can't be applied to smaller, inflexible machines like the Shapeoko. You just have to approach them slightly differently. I tend to disagree with most of the cutting recommendations that I see on CNC routing pages, and derive my own feeds and speeds from what I've learned in running large machining centers.

Chip load is a physical thing. It's the thickness of the thickest part of the chip that the cutter generates. If your cutting feeds are set up right (i.e. actually generating chips), you should be able to straighten out a chip (carefully! they can be sharp) and measure the thickness. That would be your chip load. I like to keep chip load constant, since the thickness of the chip has a huge amount to do with where heat goes, where cutting forces go, and ultimately the cleanliness of your cut and the life of the tool. I'll always start with the chip load to get a feed rate. Here's how that works:
Feed = [chip load]*[#of flutes]*[RPM]
You'll notice that cutter diameter doesn't come into play there. If you add it to your formula, you're going to come out with really weird numbers. Basically, I say I want each tooth of my cutter to take off a certain amount of material, say 0.004". Now let's say my cutter has two flutes, so every time it rotates I have two chips being removed. In order to remove 0.004" per flute, I have to move the cutter by 0.004*2, or 0.008" per revolution. Now I can multiply that out by my spindle RPM (12000, because why not) to get 0.008*12000 or 96 inches/min. You'll notice units cancel out to a sane unit of IPM for feed. "But Jeremy," you say, "If I'm trying to run my poor little 1/16 cutter through acrylic at 96 IPM it won't last two seconds! That's just too fast!" Well, I hear you. The thing is, it's not too fast. It's actually the appropriate speed to get a good cut. (I'm not vouching for 0.004" necessarily being an appropriate chip load for acrylic. I'd actually suggest something more along the lines of 0.002" to 0.003", but that's a discussion for another time.) The thing at this point in time that will break your cutter is excessive cutting forces, which come from the last variable in our cutting equation: depth of cut.

Many places will have fundamental rules of thumb for how deep you should cut with your CNC router. They'll say "cut at 1/2 your cutter diameter," or something along those lines. Ignore that for these models. I don't trust something that simple, as its bound to be overlooking something. In this case, proper chip and cutter loading. There are a lot of ways to use a lot of math to calculate how deep you should cut, but at the end of the day you're still using a shapeoko machine, which is quite flexible. What I'm saying is, every machine will be different and hard to predict. Start shallow (won't hurt anything) and work down deeper and deeper until it sounds like your cutter is really loading down, then back off a shade and remember that value. I usually suggest starting with 0.012" depth per pass for harder plastics (acrylics) and 0.024" for woods. Those will be very light cuts, and you can play with increasing them more and more until you're happy with how the cut goes.

TL;DR
Cut fast and shallow, and play with things until you're happy with how it works out. Yesterday I was using an embiggened shapeoko to rip through plywood an 130 IPM, just with shallow cuts. I got a clean cut that didn't take much longer than a slow, deep cut and I was able to talk with the person standing next to me while cutting without raising my voice. Try it sometime, I think you'll like it.
--
Jeremy Bloyd-Peshkin

http://ulterior-motors.com
UlteriorMotors
 
Posts: 10
Joined: Wed Jul 09, 2014 3:29 pm
Location: Nomad

Re: Feed rates... what am I missing?

Postby WillAdams » Wed Jul 09, 2014 4:35 pm

Thanks! That's very interesting. Do you mind if we copy the whole thing into the wiki?

I think that w/ that, and the precisebits zig-zag test, we can get a straight-forward technique for working up optimal feed-speed rates.
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)
WillAdams
 
Posts: 8323
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15

Re: Feed rates... what am I missing?

Postby UlteriorMotors » Wed Jul 09, 2014 4:43 pm

Yeah, sure. Happy to help.

One thing to understand is that depth (axial depth, along the cutter) vs width (radial width, or stepover) is very different in traditional machining as opposed to cnc routing. In traditional machining, you tend to start out with a block of material slightly oversize of the actual part. You then whittle it away to reveal the part hidden inside, which usually involves very deep axial cuts with a very shallow radial cut. This is the opposite of routing, in which we're cutting parts out of sheets, so most of the time we have no choice but to have 100% radial engagement (full width of the cutter is cutting). This is less than optimal, and means that we have to cut shallower to compensate. Most "rules of thumb" for cut depth don't quite grasp the fact that you are more or less locked in to 100% width of cut. You can't choose an optimal depth and adjust the width to compensate as normal. You can implement various strategies to do that when cutting parts out of a sheet or panel, but it really doesn't make any sense in that context because it's much less efficient from a cycle time perspective. I'm working on a simplified version of a speeds and feeds calculator that's optimized for shapeoko right now, and when it's done I'll be sure to post the spreadsheet on the forum.

Thanks!
--
Jeremy Bloyd-Peshkin

http://ulterior-motors.com
UlteriorMotors
 
Posts: 10
Joined: Wed Jul 09, 2014 3:29 pm
Location: Nomad

Re: Feed rates... what am I missing?

Postby WillAdams » Wed Jul 09, 2014 5:22 pm

Great!

I copied things in, and edited things a bit. We'll let it sit there and percolate and see what happens in the way of editing and touching-up and improvement.

One thought on the Materials page --- it's getting kind of long and unwieldy and rather wall-of-text-like.

How do people feel about the table up at the top? Would it be okay to re-format the current bulleted-list format used for the bulk of the feeds-speeds into similar tables? (We'd keep the overview table --- does anyone think anything should be added to it? I'd like it filled w/ an assortment of stuff suitable for novices to cut w/ a stock SO2).

Another thing I've been thinking about is posting one or more image per major material type showing a detail from a project made of that material from the project galleries --- seem reasonable?
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)
WillAdams
 
Posts: 8323
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15

Re: Feed rates... what am I missing?

Postby UlteriorMotors » Wed Jul 09, 2014 5:58 pm

Here's a quick clip of running the "fast & shallow" strategy on plywood. 1/16" bit, 12kRPM.
The large sheet was getting sucked up into the cutter because of insufficient clamping and so the cut quality was sub-optimal and the tabs were as good as not there. But otherwise the cuts were fantastic and the bits near the clamps were clean clean clean.

--
Jeremy Bloyd-Peshkin

http://ulterior-motors.com
UlteriorMotors
 
Posts: 10
Joined: Wed Jul 09, 2014 3:29 pm
Location: Nomad

Re: Feed rates... what am I missing?

Postby Woodworker » Wed Jul 09, 2014 7:21 pm

I like the table format. I am more likely to find what I am looking for and it is easier to compare
BRuce - SO2 #4798 - IC's Z axis upgrade, customized Z rail and Z motor mount, spindle Dewalt 611
Woodworker
 
Posts: 639
Joined: Tue Mar 11, 2014 1:37 am
Location: 5 miles north of Benson, NC

Next

Return to Discussion

Who is online

Users browsing this forum: No registered users and 1 guest