Just a quick confirmation on some speed/feed related stuff. I know there are tons of resources out there (that ya have pointed me to already - much appreciated), but wanted to share a video to help gain a bit more comfort with all this stuff.
I have been using the recommended feeds and speed already in the carbide tool library and things have been good. I purchased a new bit and it had some recommended settings for cutting soft wood, so I put them in.
In doing that, the router took off and cut through the material faster than I had ever seen it move! Probably totally fine, but being completely new to this world and not having any point of reference, I wanted to share a video and just get some feedback as to…
Yeah, that seems fine
– to
Holy hell, slow that things down!
diameter: 1/8
feed rate, 125
plunge rate: 62.5
Video:
It’s just a simple little gnome cut out of pine, 19mm thick, step down of .125.
Just looking to help establish a baseline of expectation in my head as I continue to learn/work through this stuff.
Not unreasonable for Pine, it’s pretty soft. I’d run those with a 1/4 all day long, you could faster even with a 1/4 probably. 1/8 you’d have to look at the recommended feeds from the manufacturer or just test.
Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.
If you are trying to make sense of feeds and speeds I encourage you to start thinking of it in chipload as opposed to feeds and speeds. Chipload is ultimately what every feed and speed is trying to get to. A simple definition of chipload is it’s the widest part of the chip cut per flute per rotation. Chipload with pass depth and tool geometry will determine. The force that the tool and machine have to resist, tool life (number of flute impacts to cut a distance), with material determines the minimum needed for “cutting” and not rubbing, the failure method and source, cut quality, and how much heat ends up in the material and tool.
With that in mind…There’s no real way to tell how aggressive that is as there’s not enough information. As stated above what is really important is the chipload and we would need the flute count and RPM to calculate that from the feed (it’s probably still what I would consider low chipload). So let’s assume for the sake of argument that you are running at 18KRPM (~600 SFM) and it’s a 2 flute cutter. To find the chipload we would divide it by the RPM and flute count. So, Chipload = feed / RPM / number of flutes. In this case that works out to 0.0035" chipload or about a human hair. That’s not really an aggressive cut. However, if it were a single flute and you were running at 10KRPM that would be a chipload of 0.0125" or 10% of the tool diameter. That would be pretty aggressive for most tooling.
There are other things to keep in mind that effect or change this like runout (adding and subtracting chipload from flutes), chip thinning (from cutting less than 50% stepover), engagement time, surface speed, deflection, tool geometry, etc. However the chipload is in my opinion the one biggest thing to understand and is almost required to ever in the future grasp those other issues.
Hope that’s useful. Let me know if there’s something I can help with or expand on.
