As shown below that likely required less than 1.7 lbf of cutting force and 40 Watts of cutting power and resulted in a MRR of 0.18 cu-in/minute. (That’s less than 1/10th the feed force and power capabilities of stock Shapeokos.)
Since apparently no speed ratings are provided for the Carbide 3D endmills, they probably shouldn’t be used at 60,000 RPM (or even above Winston’s 18,000 RPM maximums?) So these endmills were used for those calculations instead.
Interesting that Winston’s reply to one of the comments on the “Speeds and Feeds for Wood on the Shapeoko” video supports my assertion that, at least with wood, “make dust not chips”.
" Winston Moy 2 months ago Chipload isn’t really a big deal, so I wouldn’t worry too much about it. The reason it matters in other materials is heat. And here if you rub more than cut, you’ll just see a little burnishing/blackening of the cut edges. That you can recover from because wood is forgiving, in aluminum you’d break a tool. If it works, just go with it. Woodworkers have been pushing router bits through wood by hand for decades, and i guarantee you they haven’t measured their feedrates!"
Cubes, you know, cubic inches per minute. Also I used a lakeshorecarbide 0.125 that is rated to 2000sfm. As far as the carbide 3d single flutes, they aren’t perfectly balanced and I didn’t like running them much past 26,000.
I dont understand you you wouldn’t want to consider chipload on every cut. Do it at least for the tool life.
Thanks!,
The 5.5 lbf predicted cutting force would cause about 0.025" of machine deflection (measured at the tip of the endmill) each time an endmill flute entered the workpiece in our stock Shapeoko. It would be interesting to see if that is workable. Note that the 654 SFM (200 m/m) Vince used slightly exceeded the manufacturer’s recommended 550 SFM and was well below the “HSM” cutting speed threshold.
I was trying to define a length of a ramp, not the type which is another good question. I think the ramp should be proportional to the size of the endmill diameter. A little guidance could be good since we recommend ramping.
Well at least on paper. While I don’t know much of either endmill, when choosing an endmill, the durability, the price and quality of the cut should also be factored-in. Maybe @Vince.Fab has tried both and can comment or maybe you found a pearl.
2019-08-10 Vince Speeds and Feeds Workbook.zip (162.8 KB)
It’s a Microsoft Excel workbook, which can’t be uploaded. So I sent it to a compressed (zip) file for uploading. But you need Excel to use it.
Thanks, I just downloaded and installed Open Office on a Windows 10 computer and opened the Excel file with OpenOffice Calc. Other than the text for the warning about exceeding speeds etc. everything seemed to work fine. I’ll try to find a more compatible font for the warning. Note that the light flesh colored cells are for inputs. The others contain calculations and links that probably shouldn’t be messed with!
Here’s the latest version of the workbook which makes the warning font compatible with OpenOffice Calc and shows SFM for RPM entries. It also allows entering a machining force value as an option (along with the previous chipload and direct entry options) for feed rate determination. IMO, entering a force value makes the most sense. I didn’t update the usage guidance (yet?), so I hope it’s a logical extension of the old one. Let me know! 2019-08-11 Speeds and Feeds Workbook.zip (155.8 KB)
Definitely would look into the more exotic endmills if I came into another really big steel project but the sfm of 1/4 at 10k is kind of up there for comfort. Also that machine force is wayyy up there, dunno if that .750 doc would be possible.
The calculator should be really nice for smaller tools and keeping deflection in check.
1/2 DOC = 1/2 MRR and 1/2 Force. Your custom machine (with linear slides) could probably handle the ~18 lbf if you feed along the X-axis, since the two Y-axis steppers should support 36 lbf. You could minimize deflection by decreasing the spindle stick-out (raise the work-piece) to reduce forces on the slides. You could also reduce cutting force by reducing the feed rate (and chipload). The workbook enables you to easily evaluate such tradeoffs for whatever material you’re milling.
@Vince.Fab posted some really impressive results using his 60,000 RPM spindle with aluminum. I added fields to the attached workbook so he/others could also log temperatures for the endmill. workpiece, and chips if they can and care too. I could also add one for noise level (SPL) but it seems that might be best done in the cutting videos(?). Note that the VFD currents entered may be inaccurate because they suggest a K factor twice what was expected.
2019-09-11 1345 PST edit: I just noticed that I forgot to put the K factor sheets and Hooby’s cool wood hardness sheet into that posted file - sorry! Here’s the corrected version.
