Thanks - another vote for 0.001 inch starting chip-load and other getting starting recommendations that actually make sense! Great free downloadable workbook calculator too (no “high level math”, “artificial intelligence”, or obfuscation/magic used.) K factors (1/unit power) are also provided for lots of materials. I’ve been looking for that for a long time.
2 Likes
Yup, the 0.001" min chipload for aluminium with a 1/4" tool seems to be agreed by so many different sources that I made it the cornerstone of the chipload table (somewhere near the middle of this thread), and basically derived all other values from that.
I’ll check out the spreadsheet tonight and what he has to say about unit power. The catch though may be that these is all excellent guidance…for a Tormach, and that some dialing down needs to be applied for a Shapeoko (e.g. the “DOC up to 200% of endmill diameter”, well I would not try that on my machine)
3 Likes
@Julien
Their unit power (1 / K factor) seems higher than most, but even using that value you should be able to achieve 1/4" DOC with your Makita router (at 30,000 RPM) if your X axis V-wheels can handle 5.66 lbf endmill force without too much deflection (can they?). You might be pushing the Makita at 1/2" DOC, but your new 2.2 kW spindle should easily handle that. That would double the endmill force though, so?NYCCNC Speeds and Feeds Modified.zip (130.3 KB)
1 Like
Yes I agree, in terms of required power & force on the cutter, I should be able to cut at 1 diameter depth indeed. This is the trauma from my first cuts talking, when I would blindly follow some advice out there to cut at 1D or even 2D depth, and did not understand the feeds and speeds thing well enough at the time, and to make things worse I was mainly doing profile cuts (slotting) in e.g. oak, resulting in scary sounding cuts.
And it’s also because I am too comfortable living in the “10.000 o 15.000 RPM” zone to go and explore what I could pull off by using the higher end of the RPM range. This is the main reason why I went for the spindle upgrade: I just cannot bear the sound of the Makita at 30.000RPM, despite the enclosure.
Anyway, last night I re-read one of your earlier post in this thread:
and found it quite interesting, I’m getting more interested in the MRR and unit power considerations now, even though I have no need to optimize cutting times or push the machine to its power limits. I have a few questions if you don’t mind:
-
how did you establish that the actual router power limit was likely in the 400-500W range, versus the theoretical 932W (1.25HP). I get that there is a power efficiency factor, I saw elsewhere that it is in the “0.75 to 0.9” range for spindles, is it really that bad for routers (~0.5?) or do I miss another factor of efficiency loss ? EDIT: just saw in that Kress spindle user manual you mentioned in some other thread, that indeed there is a x2 difference between input power and output power. Wow.
-
where does the “20 lbf limit for the Shapeoko X-axis” come from ? (stepper motor max torque before they skip steps and/or some experimental limit before belts slip ?)
-
short of using G-wizard, is there a simple rule determine cutter torque ? (from which you then derive cutter force, and compare it to the Shapeoko’s limit).
EDIT: sorry, it’s actually mentioned in the excel sheet from NYCCNC : Cutter Torque = Cutter Power * 63024 / RPM. I really hate magic numbers though, I’ll do some more googling to find the full story.
EDIT2: got it, 63024 is how we get from value in ldb-in (for torque) and HP (for power) to metric units of N.m and Watts
I wish I did not have to manipulate both metric and imperial to sort this out…
So finally, over here in the old world, Cutter power in Watts = 2pi radians * (RPM/60) turns per second * cutting torque in N.m, which is what I learned in school many years ago.
1 Like
Lemme ask a question that’s been on my mind.
At what point is a cut “bad”? On super low power machines like the Nomad and Bantam you will simply stall and shut the machine down but with shapeoko power it’s quite easy to machine through the chatter.
Now we know that any chatter is bad for cutter life and surface finish. Maybe we should all come up with a way to standardize a limit.
After all, how can you know how far to go if you don’t know how far it too far? Just thinking out loud here.
2 Likes
Well when the workpiece lifts off the table and launches, that is typically a pretty bad sign.
My desired finish depends on the project, and the materials.
4 Likes
“Yup, the 0.001” min chipload for aluminium with a 1/4" tool seems to be agreed by so many different sources that I made it the cornerstone of the chipload table (somewhere near the middle of this thread), and basically derived all other values from that." Just because larger diameter cutters may support higher chiploads, does that mean they require them? Isn’t minimum acceptable (and desirable) chipload more determined by how sharp the cutter is? The workbook uses chipload as the primary driver and I’m starting to think that makes a lot of sense.
“EDIT: just saw in that Kress spindle user manual you mentioned in some other thread, that indeed there is a x2 difference between input power and output power. Wow.” That’s why the attached latest version of the workbook bases router power output on input power and efficiency rather than advertised power.
" EDIT2: got it, 63024 is how we get from value in ldb-in (for torque) and HP (for power) to metric units of N.m and Watts 
I wish I did not have to manipulate both metric and imperial to sort this out…" Yup the “Imperial System” is a real PITA - I’m glad I was an E.E.! The workbook has all the formulas and isn’t protected, so you/someone might want to make a copy of the worksheet(s) (in the same workbook?) and convert them to metric if you think it’s worth the effort. Let me know if you find any errors or have any questions. I’ll probably continue to refine it though.
“where does the “20 lbf limit for the Shapeoko X-axis” come from ?” That’s my understanding of where the stepper motor starts to slip - its easy enough to measure. But it seems more likely that cutter deflection caused by torque on the Z and or X axis V-Wheels would limit useable force to less than that. That’s easy to measure too.
2019-07-05 NYCCNC Speeds and Feeds.zip (130.5 KB)
3 Likes
I like your modified version of the spreadsheet a lot. So much so that I’m thinking it would be great to improve it collectively here on the forum to make it (even more) user friendly, and then include it in that Shapeoko (free) e-book side project of mine. What do you think ?
We would obviously leave the NYCCNC/SaundersMachineWorks logos in there, as well as credit you and whoever else contributes. Sure there are several nice online calculators, but I’m often frustrated by the “black box/black magic” side of it.
Anyway, what I would volunteer to do is:
- make a metric version of this as you mentioned
- highlight user inputs and protect computed outputs (I actually liked this detail of the original version better : bright yellow for inputs)
- make a small user guide/process for how to fill this (it’s easy enough, but I remember when this all looked like a very daunting foreign language to me).
- make it useful for other materials than metal. The spreadsheet is currently very metal-oriented (no wonder given its origin), and all K-factors of anything non-metal is set to “10.00”…
EDIT: oh, and I’m with 100% you on the “everything starts from the chipload” approach. This was the very root of this thread, I did not understand inconsistencies in chipload values from various F&S recommanded settings, and did not understand either where to find a proper chipload value to plug in G-wizard, that takes care of everything else. For metal the answer might well be “don’t think twice and just use 0.001” always", for other materials a guidance is useful, and it still feels very logical to me that the chipload recommandation would scale with endmill diameter. Indeed, that’s assuming we are using a sharp cutter in all cases.
3 Likes
Really? I’m surprised that there would not be a difference say between aluminum and steel or titanium. I wonder if @Vince.Fab and @RichCournoyer who have a lot of experience milling metal on the Shapeoko agree with this.
Yeah, scratch out metal and replace with aluminium, I have never cut steel or titanium so I have no idea what a good chipload is for those materials, and from what I remember reading @Vince.Fab posts, what matters more for titanium is being in the (narrow) optimal range of SFM.
2 Likes
Cut 304L stainless steel yesterday with the Nomad.
Online minimums read 0.0001 but I was able to cut very well between 0.0007-0.0011 actual maximal chipload. Ended with adaptive with 0.125 4 flute, 10krpm, 325 sfm, semi dry, 0.025 axial doc, 0.015 radial doc.
Ready to try some Inconel or Monel to test chipload minimum theory. Its interesting how the optimum axial/radial ratios change for different materials.
1 Like
@Julien
“improve it collectively here on the forum to make it (even more) user friendly, and then include it in that Shapeoko (free) e-book side project of mine. What do you think ?” Great idea IMO
“We would obviously leave the NYCCNC/SaundersMachineWorks logos in there” Yup - we should share our version too. If they’re willing we could even collaborate with them.
“Sure there are several nice online calculators, but I’m often frustrated by the “black box/black magic” side of it.” Me too - like the “high level math and artificial intelligence”?
“highlight user inputs and protect computed outputs (I actually liked this detail of the original version better : bright yellow for inputs)” I tried to use Excel’s “Cell Styles” formatting for that.
“make a small user guide/process for how to fill this (it’s easy enough, but I remember when this all looked like a very daunting foreign language to me)” Me too - that’s what’s nice about the NYCCNC video. It does a really good job of explaining things.
“make it useful for other materials than metal. The spreadsheet is currently very metal-oriented (no wonder given its origin), and all K-factors of anything non-metal is set to “10.00”…” I’ll add my estimates of some woods when I get the chance. That’s something else that others could contribute, if they’re willing.
“For metal the answer might well be “don’t think twice and just use 0.001” always”, for other materials a guidance is useful, and it still feels very logical to me that the chipload recommandation would scale with endmill diameter. Indeed, that’s assuming we are using a sharp cutter in all cases." Higher chiploads require more power and force, lower chiploads require sharper endmills and lower runout!
2 Likes
Cool, I’ll get to work then (on the metric version + my take on instructions/steps/subtitles on how to fill this).
The nice thing is that target chipload will be a primary user input in any case, so anyone can use the reference values they like best, and we can continue to agree to disagree on what those values are
*Higher chiploads require more power and force, lower chiploads require sharper endmills and lower runout!
=> yes, but our tools are not always as sharp and our runout as low as we would like, so there must be a middle ground ? What would you recommend as guidelines for the values of target chipload ? As far as I can tell, all the calculators/manufacturer datasheets out there have a different chipload target depending on material and endmill diameter. Do I understand correctly that what you are saying is actually, max out your RPMs before you try to max out your chipload ?
2 Likes
How about you guys convert this to javascript and make sure the formatting works for smaller devices (phones)?
2 Likes
I’m not proficient in Js but if anybody is, that could be nice indeed
1 Like
Options for minimizing force (Shapeoko’s and likely many other CNC router’s Achilles-heels):
- Maximize spindle speed - minimizes torque/force for a given power/MRR.
- Maximize cutter diameter - less force for given MRR.
- Minimize chip-load to acceptable value (0.001 " is reportedly good for metals, so it seems like it might be a good starting point for softer materials too - regardless of cutter diameter). Feed rates can always be increased/decreased to increase/decrease chip-loads as required if possible. Carbide Motion allows that to be done while milling (+/- 100%).
- Decrease depth of cut (DOC) - most endmill manufacturers’ speeds and feeds guidance recommends using the endmill diameter for DOC when slotting (DOC=WOC) and DOC 2-3 times the endmill diameter for smaller WOCs. Using more of the cutting surfaces likely increases endmill life by more evenly distributing the cutting and heating.
- Decrease WOC - seems viable too.
I don’t know anything about modern software beyond how to use some of it a little. Would it be possible to develop a user friendly GUI wrapped around (or replacing) the Excel spreadsheet for PC use too (without obfuscating how it works)?
I was hoping Jupyter Notebook could be used for this sort of thing:
and was working through that at:
which at least resulted in the nice interactive Tableau version:
https://public.tableau.com/profile/willadams#!/vizhome/Carbide3DCNCFeedsandSpeeds/Sheet1?publish=yes
Perhaps we should just make a version of that which has only the selection options:
- chipload
- feed
- speed
- endmill diameter
- number of flutes
1 Like
@WillAdams
"Perhaps we should just make a version of that which has only the selection options:
- chipload
- feed
- speed
- endmill diameter
- number of flutes"
IMO the primary value of effective speeds and feeds calculators is that they enable users to evaluate the likely impact of varying any/all of the milling parameters, not just a subset.
Just an idea while I’m looking at this, how about putting the material table with F&S on Google Spreadsheet and build in a basic calculator for the Shapeoko/Nomad based on this. A few of the gurus here would have all access to update and modify while the plebes would have access to use it. The idea of using Google is that we would have one version although someone could copy it but since there is still a lot of discussion about the right values, any change would be available to everyone.
@luc.onthego
IMO we should make sure that we and NYCCNC are both happy with it before we discuss/consider “putting the material table with F&S on Google Spreadsheet”