@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!
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 ?
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)?
@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”
Well, while working on improving the spreadsheet I got carried away and butchered it to the point where it does not look like the original one anymore (though all formulas are still there, it’s all mostly cosmetic)
While writing instructions, I started shuffling parts around, to the point where I rearranged everything vertically in “my” logical ordering from top to bottom, and instructions ended up being redundant so I removed them. I also gave up on the idea of making a separate tab for metric, which sounded like maintenance would be a nightmare when anything changed in the imperial version. So I settled for just displaying the metric conversions of all values for now, which suits my need at least. In its current form the spreadsheet goes hand in hand with the summarized “generic process” I have written down in the e-book draft currently:
@gmack: thank you for the pointers on optimizing cutting force. I need to digest that, and then write it down in my own words
@WillAdams: Jupyter looks nice, and it probably an excellent solution to make it web-friendly once this topic will have matured enough, but for now nothing beats an Excel spreadsheet to support discussion on the process itself.
@luc.onthego: once the dust settles this is probably a good way forward, but for now I’m being selfish and will stick to the local excel file while the discussion progresses, because now that I want to include a version of the calculator in the e-book, I need it to be 100% self-sufficient / independant from any external link. It’s hard enough as it is to release a first version while keeping my motivation above the breaking point
Sorry for the lengthy post, I’m looking forward to receiving comments and additional bits of wisdom from @gmack and others
Thanks- I just finished adding some features and worksheets for additional measured K factors and their calculation to the 2019-07-05 version. I’ll look at yours later or tomorrow. 2019-07-07 NYCCNC Speeds and Feeds.zip (139.0 KB)
@Julien
" look-up the desired minimum chipload for this material+endmill combination:
see guideline table" TBD?
" choose a radial depth of cut / stepover:
35% to 50% stepover for roughing using a regular toolpath
10% to 35% stepover for roughing using an adaptive clearing toolpath
5% to 10% stepover for a finishing toolpath" Need 100% for initial (slot) cut too?
" if stepover is less than 50%, adjust target chipload for chip thinning Calculator does that
" select target RPM
somewhat arbitrarily within your router RPM range: NO!
slower is quieter (and better for plastics) Quieter depends on spindle - Faster works for plastics too
higher is better to reduce cutting forces" You’ll have to show me that faster isn’t always better - at least with “soft” materials even plastics!
" determine depth of cut:
5% to 10% of the diameter of the endmill for metals e.g. Nope
10% to 50% of the diameter of the endmill for softer materials Nope!
" if possible, check deflection to make sure there is no risk to break the tool" See latest workbook
Thank you for the brutally honest feedback, that’s what I’m after. I will not fool anyone into thinking that I know what I am doing, but I may get things correct enough to be useful for a beginner, or even just for me.
guideline table: I am referring to the baseline chipload values mentioned much earlier in this thread, and that currently looks like this:
Soft plastics
Hard plastics
Soft wood / MDF
Hard wood
Aluminium
Hard plastics+100%
softwood + 20%
hardwood + 100%
baseline + 100%
baseline
1/16"
0.0025"/ 0.06mm
0.0012"/ 0.03mm
0.001"/ 0.025mm
0.0005"/ 0.0125mm
0.00025"/ 0.0063mm
half of 1/8" values
1/8"
0.005"/ 0.12mm
0.0024"/ 0.06mm
0.002"/ 0.05mm
0.001"/ 0.025mm
0.0005"/ 0.0127mm
half of 1/4" values
1/4"
0.01"/ 0.254mm
0.0048"/ 0.12 mm
0.004" ,/ 0.1mm
0.002"/ 0.05mm
0.001"/ 0.0254mm
baseline
I know you will not agree and prefer to have it all at “0.001” and a sharp cutter" and then optimize other parameters, this is the interesting discussion we are having right now. But after reviewing tens of recommanded/tested settings on the forum/wiki, and testing a good share of those myself, this is the closest approximation I could come up with, and it’s working fine for me. If I’m using 0.001" chipload in plastics for example, I’ll be melting the stuff, or I am missing something in the recipe.
stepover: true, the “100% for slotting” was implied since there is nothing to choose then, I’ll include it.
chip thinning: indeed the calculator does it, this is just the description of the process/steps (which concludes a chapter going over the details of the parameters and formulas).
RPM:
the “quieter” part is aimed at the 90% (?) of Shapeoko users that use a trim router. 30.000RPM is not an option for some of us (it’s beyond the WAF for me, for example)
could you post your feeds and speeds for cutting plastics at high RPM ? Even with an O-flute, I’ll max out the feedrate very quickly if I use anything but the lower part of the RPM range.
I am not saying that faster is not always better from a theoretical standpoint, the cutting forces formulas speak for themselves. BUT, for some of us other factors come in the picture, e.g. tolerance to router noise. At least people should have a choice in the compromise they prefer to make?
depth of cut: please explain why those values are incorrect (for regular slotting/pocketing). They result from observation and averaging of tens of recommandations out there (I must have watched every Winston video two times by now, the @cgallery process that I think makes a lot of sense is to take recommended F&S values and halve the DOC for the Shapeoko, etc…). Of course, for adaptive the picture is very different, and I happily use several hundred % of the tool diameter. I mentioned that, but not in this summary, is that maybe what you refer to ?
deflection : yes, the worksheet does that now as well as the force and power stats, I like that a lot and still have to include that part in the text indeed.
Re: RPM I agree with Julien, faster may be better but for the majority other considerations especially noise but also safety and I understand that brushes, especially on Dewalt appear to wear out more quickly at high speed. People have also reported that the high speed can cause the plastic to melt maybe it is a question of finding the right F&S but so far experience appear to show that faster does not work properly.
Hardness table, I see all the woods being rated as 1 and a K factor of 10. Based on this, if I cut soft or hardwoods, I should use the same F&S settings? From my experience, it seems wrong but maybe I do not completely understand your worksheet.
I see two sections that may be contradictory first:
I suspect that if you’re melting plastic/aluminum and/or burning wood, your federate is too low, not your chipload. I plugged the measurement conditions and values from line 10 of the “K Factor Measurements” spreadsheet into the Acrylic at 9k and 25k RPM.zip (139.2 KB) workbook to demonstrate the differences at high and low speed. I had to double the chipload to 0.002 IPT to compensate for the higher federate of the measurement. I also had to adjust the SFM value option to provide the 9000 RPM speed to enable a side by side comparison of the predicted performance at the two speeds. Note that the feed rate is 25/9 = 2.77 times higher at 25,000 RPM than at 9,000 RPM for the same 0.002 IPT.
I’ve quite successfully cut a lot of plastic (mostly acrylic) with this 80 tooth sawblade at 3540 RPM on my table saw. 60 IPM / 3540 RPM / 80 Teeth/Revolution = 0.0002 IPT chipload.
I have never milled plastic so far, did not burn wood either but the idea of doubling+ speed and doubling SFM while cutting a piece of maple scares me for some reason. The plastic issue was reported by others who were trying different F&S and found that the lower RPM gave better results. I’m not disputing the theoretical, I want someone braver to try it and report.
I was referencing the CNC. Yes many times I have used manual or table mount routers and yes I did burn wood/router bits and yes I operated at higher speed on a table router but I was controlling the work piece by hand and could easily pull it out if I sensed any issue (chatter, sound, vibration, etc). I also encountered times when the router went sideways and ruined my piece. Controlling speed by hand is not an exact science, I usually go by sound. In the CNC, it will continue on its merry way even if the gantry comes off or the bit wants to dig to the bottom of the earth or workpiece start flying until I can press pause/stop. I know others feel the same; doubting Thomas maybe but I still have all my fingers and eyes and I would like to see some experimentation on the Shapeoko before I rely blindly on the theoretical calculations and a recommendation to max out the RPM in most situation. The lower RPM still can lead to good results even if it may not completely optimizing the potential of the CNC.
Like many here I’m a hobbyist and if it takes me an extra 1/2 hour and feel safer and not have a splitting headache from the increased sound so be it.
Unless I missed something, this example demonstrates that 25k/100ipm is better than 9k/36ipm from a power perspective (only?), but the question remains whether this 0.002" chipload would allow to cut plastics without melting at 25k/100ipm. I’m game for putting that to the test tonight, in HDPE or Acrylic.
@Julien
25,000 RPM consumes 2.77 times as much power and delivers 2.77 times as much MRR and is in contact with the workpiece 1/2.77 as long, so is probably 2.77 times less likely to melt it.
