Feed and speed starting point ?

Talk about all things CNC
AlainTernet
Posts: 34
Joined: Wed Oct 14, 2015 4:28 am
Location: Québec, Canada
Contact:

Feed and speed starting point ?

Post by AlainTernet » Fri Jan 29, 2016 5:08 am

I started to test my Shapeoko 3 (with DWP611 Dewalt) last week and I have a hard time finding the right feed and speed settings.
I think it is really the hard part, more than I expected...

I checked the wiki material page but it's difficult for the newbie like me to find something corresponding exactly to the endmill I have
or many parameters are mentioned (like feed ranging from 36 to 76 ipm for the same material).
Finally, the few tests I have made are not very satisfying. I know I have to do some tests,
but I would like to begin with some values not too far to avoid wasting too much materials and endmill

One other question: which parameter changes when I decrease the endmill size ? For example, If go from 1/4 to 1/8 endmill,
do I have to cut the feed in half ? (and the other parameters? like speed, plunge, step over, etc). Is there an easy rule of thumb for this ?

So, can you suggest me some starting point for the 3 materials (and endmill) I would like to use:

Hard maple
1/8 endmill -2 flutes - square end (or ball nose end)
1/4 endmill -2 flutes - square end (or ball nose end)

MDF
1/8 endmill -2 flutes - square end (or ball nose end) --- The 2400mm/min (94 IPM?) suggested in the wiki seems really fast ??
1/4 endmill -2 flutes - square end (or ball nose end)

Naturals materials like bone, antler or horn
1/8 endmill -2 flutes - square end (or ball nose end)
1mm endmill -2 flutes - square end

John_TX
Posts: 34
Joined: Tue Dec 01, 2015 5:17 pm

Re: Feed and speed starting point ?

Post by John_TX » Fri Jan 29, 2016 12:11 pm

Thanks for posting this! Sorry I don't have any good numbers to offer up, but I'm in exactly the same boat as you and was thinking about posting the same thing. I started out with what seemed really slow feeds (about 30ipm) and very shallow depth per pass (0.08 to 0.1 inch) on soft wood and MDF. This seemed fine using 1/8 endmill on pine, but job time was very long. I'd like to confidence to either double the speed, or double the depth per pass, but I don't want to risk breaking bits or worse (what is the worst that could happen?)

And when cutting out a profile, I wonder if dust collection is a factor - I was cutting out a piece of MDF using 1/8 endmill, 30ipm, .1" depth per pass, and after two passes the dust collected in the cut looked like it would bog down the bit. I quickly paused the job and vacuumed it out but I wonder what would have happened?

Finally, I would add to your request for information - what router speed settings to use? It seems that burning workpiece (or heat damage to bit?) happens at unduly high speeds, and unduly low speeds would break a bit, miss steps, or pull on the gantry if feed and depth are too high... So many variables!

WillAdams
Posts: 8489
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: Feed and speed starting point ?

Post by WillAdams » Fri Jan 29, 2016 12:13 pm

From Carbide Motion:

Hardwood
- depth per pass: 0.704mm
- step over 1.429mm
- Feedrate: 424.180
- plunge rate: 106.045
- RPM: 6250

MDF
- depth per pass: 0.883mm
- step over 1.429mm
- Feedrate: 586.740
- plunge rate: 146.685
- RPM: 9375

For bone / antler, use the hardwood settings, but a higher RPM? (and impeccable dust collection, and wear a HEPA mask, and clean up w/ a HEPA vacuum)

Always make a test cut: http://www.shapeoko.com/wiki/index.php/ ... FMaterials

I’ve used the technique suggests by the Precise Bits folks to good effect: http://www.precisebits.com/tutorials/ca ... speeds.htm
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)

AlainTernet
Posts: 34
Joined: Wed Oct 14, 2015 4:28 am
Location: Québec, Canada
Contact:

Re: Feed and speed starting point ?

Post by AlainTernet » Fri Jan 29, 2016 7:47 pm

Thanks for your help Will
But I wonder about RPM.

The lower speed of the Dewalt DWP611 seems to be much higher ?
1 = 15820 RPM
2 = 16960 RPM
3 = 18950 RPM
4 = 21280 RPM
5 = 24270 RPM
6 = 27080 RPM

So, if I use the lowest speed (~16 000rpm) do these settings are still good ?

WillAdams
Posts: 8489
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: Feed and speed starting point ?

Post by WillAdams » Fri Jan 29, 2016 8:27 pm

Well, they're a starting point.

Unfortunately, Carbide Create seems to be more oriented towards the Nomad, w/ its real spindle --- those of us w/ routers have to just make do.

You may be able to increase the feed by a similar amount --- or that may result in a broken bit. Try the feed rates as a starting point using the technique I linked to determine an optimal feed rate using a piece of scrap material, then use that (and share it back w/ us).

Alternately, if you're not closed-source averse, just buy G-Wizard --- a single year's subscription will then provide you w/ a perpetual license for a 1HP of G-Wizard Lite which is all one needs when using a router for a spindle.

William
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)

Damin69
Posts: 331
Joined: Fri Oct 31, 2014 3:00 pm
Location: Muscoda, WI

Re: Feed and speed starting point ?

Post by Damin69 » Fri Jan 29, 2016 10:32 pm

Like Will said starting point you will have to do some trial and error to get it all down. You will learn how much and how fast you can push your machine it just takes a lot of practice. I have had my machine for a little over a year and I am still learning. On hard woods on my makita I run my router around 3.5-4 on the dial.
Shapeoko 2 #6971
Upgrades
Makita 0701, Nema23s, ACME Z Axis, Nema 23 Belt drive
Expanded to 1000 x 1800
Electronics upgrade C-10 BOB, SainSmart ST-M5045 drivers, Mach3
Damin69's Build Log

AlainTernet
Posts: 34
Joined: Wed Oct 14, 2015 4:28 am
Location: Québec, Canada
Contact:

Re: Feed and speed starting point ?

Post by AlainTernet » Mon Feb 01, 2016 4:53 am

WillAdams wrote:Well, they're a starting point.
Unfortunately, Carbide Create seems to be more oriented towards the Nomad, w/ its real spindle --- those of us w/ routers have to just make do.
Ok, this is starting point for Nomade. Too bad they do not take into account the Shapeoko 3 with Dewalt router.

There he has some Shapeoko 3 users willing to share its wood cutting settings with us ?
WillAdams wrote: You may be able to increase the feed by a similar amount --- or that may result in a broken bit. Try the feed rates as a starting point using the technique I linked to determine an optimal feed rate using a piece of scrap material, then use that (and share it back w/ us).
Ok, the feed you suggest for hardwood (424mm/m -17ipm) can be considered as a slow feed speed for hard wood ?
How far I can go up on a Shapeoko (to cut wood). Is 50ipm or 100ipm is conceivable?
(these numbers are very abstract for a beginner).

Another question: Is it better to make fewer passes (but more heavy) or make more passes (but lighter) ?
WillAdams wrote: Alternately, if you're not closed-source averse, just buy G-Wizard --- a single year's subscription will then provide you w/ a perpetual license for a 1HP of G-Wizard Lite which is all one needs when using a router for a spindle.
Since I plan to work only with some materials and the same bits, I wonder if paying for G-Wizard is a good investment.
(and my planned materials are certainly not in the software)

WillAdams
Posts: 8489
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: Feed and speed starting point ?

Post by WillAdams » Mon Feb 01, 2016 11:55 am

I think the under-lying concept behind G-Wizard is brilliant --- I wish it was programmed in something other than Adobe Air.

What I would really like to see is that sort of algorithm built into a CAM tool and used dynamically as paths are computed — I believe the more sophisticated HSM/trochoidal CAM systems do that sort of physics-based calculation.

This is a hobbyist kit, which started as an opensource project — what’s on the wiki is what’s available until Edward releases his book, Carbide3D releases more information, or someone tries some material and shares that information.

Yes, please start w/ those numbers and use the testing methodology suggested — it would be great if you’d then share your experience so that it can be added to the wiki. Eventually it will be cleaned up so that it reflects the greater family of machines, and tightening up the longer pages such as the feeds and speeds page will be a part of that. If you want an account to pitch in, let us know.
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)

edwan
Posts: 19
Joined: Wed Nov 11, 2015 5:04 am
Location: Schaumburg, IL

Re: Feed and speed starting point ?

Post by edwan » Mon Feb 01, 2016 4:03 pm

I cut a lot of .25" -.75" oak, cherry, maple, and poplar. I use .250 2 flute bits flat and ball nose, and .125 ball nose. Insert V bits from Amana (Toolstoday) and a precisebits collets and nuts. I use mostly upcut, though downcut is nice on some woods to minimize fuzzies. I use Vectric software.
I use a 1" insert surfacing bit to keep my spoilboards flat. All my wood is screwed (through pilot holes in the workpiece) to the spoilboard.

I ran a lot of jobs at 20 ipm when I started, though as I got more experienced I use 30-50 ipm without any issues depending on the woods, depth of cut etc.. I keep the plunge down to 10 ipm to minimize spindle deflection (and possibly loosing steps), though I did noticed some in birch (wood, not plywood)with a 10 ipm plunge and 40 ipm feed (dense stuff). I realize these speeds are slow, but I will continue to raise them as my skill level and confidence level increase. Right now they are adequate for the work I am doing.

I use the Dewalt router at 1-3 speed. Pay attention to chips on the hardwoods. If you are making sawdust the speed is to low. You want to see discernible chips, even if they are small.

Thats it for me. My SO3 has done a good job so far. The Z is a weak point, but by keeping my speeds/feeds down it has rarely been a problem. I see there are some nice threads going on improving the Z and I am following them with closely.
S3 #1105

sgth0mas
Posts: 101
Joined: Sat Dec 12, 2015 5:57 pm

Re: Feed and speed starting point ?

Post by sgth0mas » Mon Feb 01, 2016 6:53 pm

CAM systems come preloaded with some tools, but the feed rate, Depth of cut (DOC), and rpms depend on so many other variables that its best left to the user to do the proper work up front to optimize the set up.

The parameters that may change your feed, DOC and rpms include but are not limited to:

Machine:
-rigidity
-coolant system
-max rpm
-max feed rate
-spindle power

Cutter:
- diameter
-number of flutes
-geometry
-coating

Material and finish requiremets.

The proper way to approach a baseline starting point for feed rate is to use the cutter manufacturers published data for a particular bit. Onsrud and Amana both publish data for each of their bits. The data will typically be presented as chipload, and feed rate is calculated based on the following formula:

Feedrate = chip load*rpm*number of flutes

So if i a 1/8 diameter 2 flute end mill has a chip load of .002" IN MDF, the feed rate in inches per minute at 20,000 rpm is:

Feed rate= .002*20,000*2 = 80 IPM.

This is typically for 1xDiameter of the cutter. With small desktop machines, its good to limit the depth of cut based on your machines capabilities. I start with 1/2 to 1/3xD

Feed rate will be given in a range as well such as .002 to .004.

Also, taking several light passes will dull the tip of the cutter since its doing all the work. You target the speed based on the calculation above, then vary the DOC based on machine limits.

Post Reply