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.
@gmack:
Well, seeing is believing, I have to admit you opened my eyes.
First test: 1/4" 2 flute endmill; pocketing in HDPE, 25.000RPM, 100ipm, DOC 0.1"
(excuse the lousy video quality, I captured this through the acrylic front window of my enclosure)
And…I confirm that there is no way I can bear the sound 25.000 RPM for a long time, nor can my neighbors at 10pm.
So, it looks to me like there will be two conclusions:
if you can/are willing to max out RPM first, this is the best way (given the optimization of cutting forces) and you can use low chiploads
if you can’t or won’t, then you should increase the chipload (and accept higher cutting forces) as an alternative way to keep things cool. Call it the hobbyist/amateur way, it still works
Now I can’t wait to receive my water-cooled spindle, to further venture in high RPM territory.
@Julien
" So, it looks to me like there will be two conclusions:
if you can/are willing to max out RPM first, this is the best way (given the optimization of cutting forces) and you can use low chiploads" Also minimizes heat generation and buildup
“if you can’t or won’t, then you should increase the chipload (and accept higher cutting forces) as an alternative way to keep things cool.” Generates more heat and heat buildup on the workpiece due to thicker chips and slower feeds rates which prolong any rubbing
I follow @Vince.Fab threads religiously, so there is no question that pushing the RPM & feeds can result in spectacular results. Also, I have been sold for a while on the possibility to use large DOCs…if using adaptive clearing (my test at 200% diameter DOC in aluminium is here).
In what other situation/toolpath would you use the 300% DOC limit you recommend ?
Using anything above 50% while slotting in e.g. oak sounds scary to me (from past tests), but then again I was probably using wrong RPMs at the time, so I definitely want to give it another go at higher RPMs now
What is still beyond me is,
if this is such a clear-cut case of higher RPM is better as long as you keep the chipload above a minimal (0.001") value, why does EVERY feeds & speeds guideline out there (Carbide3D’s table, Winston’s videos, wiki…) recommend RPMs in the lower 10k-18k range, and with chiploads that more or less match what I have in my table ?
why does using higher chiploads at lower speeds also seems to work to keep the cutter cool ? I (like many others) have had nice cuts in plastics going at min RPM, low flute count, and feeding fast (i.e. using high chiploads). And successfully cut hard woods at “high” chiploads with no noticeable heating of the cutter. I don’t deny this might not be the right way, but why does it work, if it’s supposed to generate heat and heat buildup on the work piece?
why would it be a such a widespread recommendation to keep cuts relatively shallow on hobby CNC machines it is wasn’t right ?
p.s. : I am not trying to argue forever, this thread is long enough as it is, but now that we are debating this (and that I’m learning so much in the process!) we might as well get to the bottom of things, and I hope to end up with a conclusion that my fellow Shapeoko freshmen can apply in day to day casual/hobbyist use.
You have summarized my thoughts also. I’m happy to see that you were able to get good results in plastics with this method, I noticed that you hid behind your enclosure during the experiment.
If some of the values are good only for adaptive clearing, it should probably be in a different entry in your table since it is not available in most CAD programs we use.
When you say the chipload has to be kept above a minimal (0.001"), that leaves room for interpretation, IMO it should be in a range.
As I said previously, these values need to be validated with experimentation and I commend you for taking the first step.
This new paradigm certainly could could change how we use the Shapeoko.
To be fair, I almost always close the front door of my enclosure anyway during cuts, for noise but definitely also for safety, I value my eyes way too much to take any risk. I actually also try to have my goggles on at all times whenever I’m in the garage. Honestly, the high RPM and feedrate is not scarier/more dangerous than lower RPM & feedrates.
My comment about adaptive is for DOC only (adaptive => lower radial cutter engagement => higher DOC is possible for a given total cutting force budget), while the table is about chiploads, which are applicable regardless of the type of toolpath
This was discussed earlier in this thread, and the conclusion was that while it should be possible to determine a generic value for minimal chipload, the maximal chipload depends on the rigidity/mods of every machine so it is difficult to provide a relevant value. The latest discussion above also tends to indicate that maximising the chipload may not be desirable anyway. Still, a “sweet spot” chipload range would be good to capture indeed.
It is definitely my intention to have actually tested every single guideline/value myself, to give all of this a little bit of credibility.
wood and plastic have a wider range that will ‘cut’, so that doesn’t surprise me.
high chiploads work in these material, rubbing from too high rpm and slow feed will bring the heat.
shallow and low chiploads is a tendency for hobby because they can stall out, skip steps, deflect, etc. not to say they’re the best, but that they will generally just work. i feel the recommendations air on the conservative side for the novice or the machine that is in need of some lovin’/adjusting.
