Speeds and Feeds seem slow

I have been running my Shapeoko Pro XXL for a little bit over a year and have been using fairly conservative feeds 45-70 ipm for most of my cutting. Recently, I have been looking into more accurate feeds and speeds and it seems as though the cutters are made to go quite a bit faster. I ran a piece of walnut today at 97 ipm/ 18,000 rpm with a doc @ 0.08. with no issues.

Just wondering what some of you run typically on the Pro, lots of information out there for the SO3.

0.08" is a very conservative depth in any carbon foam matrix product (wood). You should be running at least 75% the width of your tool if not double.

The stock F&S are always conservative. You could bump up in the CM interface or duplicate the stock libraries and change them permanently. You can also change them when picking the tool. So there are a lot of options for customization.

1 Like

So your saying 75%-150% of the tool width for depth? I thought I had read that 50% of the diameter of the bit was a good starting point.

2 Likes

I don’t think that I have ever used the stock F&S. I am just thinking a lot of what I read seems low and trying to find out what others use. I mostly cut oak, maple, hickory, walnut, etc. After reading DiscoJon’s post maybe I just need to increase DOC.

I’d start at 75% DOC with a conservative feed and push the feed until the machine complains. Be sure you are making a good chip and not dust. For slotting you will need to be more conservative. For adaptive or even pocketing, go full ham.

For wood (especially hardwood): My experience has always lead me to use ~50% of bit diameter for DOC at a slightly faster feed rate. Going 150% of the diameter IMO will lead to premature bit life, burning, hard on the spindle and bearings and much slower feed rates. If you are using a CNC for speed, it’s probably the wrong tool. YMMV

There has to be a trade off between DOC and feed. Increase one, decrease the other. Find a happy place for your setup. If you want to run conservative that’s fine, low DOC but ramp the speed up so you are making a good chip. Personally I prefer deeper cuts and then I’ll push the feed. I’m pretty sure you have more than 1x width of cutting length. If you only use the tip of the tool you will Increase deflection and wear only that part of the tool out. If I’m paying for cutting length, I’m using it.

1 Like

Don’t disagree with what you have written in theory. Many ways to skin a cat.

For an example of what I am doing, I have a .250” bit that is 3” long and has 1.75” length of flutes. I cut through guitar bodies that are 1.5” thick. Part of the flute length is to help extract the chips above the top of stock even though my doc per pass may only be .125”. I am running the perimeter (slotting?) of the shape and cutting all the way through. My max feed rate is around 75ipm. Could go faster? Maybe. I control the router rpm manually while making the first pass until it sounds and looks right.

May not be text book, but so far it works.

1 Like

Slotting is a whole different beast. Proper slotting technique is to have great chip evacuation via air blast or strong vacuum. When slotting you absolutely should be conservative on everything other than very rigid machines with strong fixturing and tools. As a matter of principle, I tend to avoid slotting when at all possible, even on my HDM. Mill an offset at least 1.5x tool diameter to assist with chip evacuation, or use an adaptive tool path, and leave some radial stock you can clean up with a full depth pass at the end.

4 Likes

Thanks for all the replies, this kind of input is super helpful.