I am trying to do deep cuts on hard wood for both pocket and contour toolpaths. For reference, I like to use thick pieces of maple and birch, and I route out the center for a piggy bank, then cut out the outline. I am also trying to make cribbage boards with these thick pieces, which mainly involves a contour cut on the outline. Sometimes (not always), I end up with chatter, and I know I’m doing something wrong, or I’ve managed to dull my bits. I am trying to find the right cutting parameters so that I get rid of the chatter and don’t dull the bit. I have a Shapeoko Pro XXL with a VFD spindle.
For the deep cuts, I use Amana 46421-K (1.25" flute) or 46416-K (1.125" flute).
I have been researching how to figure out the right parameters, but I don’t have a good head for calculations (math/engineering are not my strong suit and I’m running short on time b/c these I’m trying to make Christmas presents). Can someone help me with where to go for the next attempt, what parameters to use? Currently, I have it at:
Cut depth: 0.040in
For the cribbage board holes, I’m also having issues with burning… I think I did too much at once. First I did a peck depth to .06, then another pass to full depth at .5. Would it make sense to do three passes, one to .1, another to .25 and then a third to full depth? That one is just a trial/error thing I think, but I couldn’t find much on toolpath details for cribbage boards in the myriad of posts about them.
Thank you! I have been using a 1/8 bit, and that one actually came out really nice, but I like the cribbage pin kit, and I’ll look into it. Those pins are nice!
Question, though, does the length of the flute make a difference for these calculations? Now we’re getting into physics, but wouldn’t the force put on the bottom of the flute cause more problems if the flute is longer and therefore is further away from the base of the spindle?
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.
Short answer. The cutting flute length, stick-out (the length of the tool sticking out of the collet), tool diameter, chipload (feed), pass depth, and stepover all can effect chatter.
Long version. Chatter can be tool/machine deflection (flexing into the cut) or material movement.
For deflection these are based on the cutting forces which change based on the tool geometry and the material being cut. For the same material and and tool it increases by the cubic material removed per flute per revolution. So any increase in feed, stepover, pass depth or tool diameter increases the cutting forces. However, going too slow or small in those can have other issues.
For material movement this is basically just your hold down. If the material can move in any direction (including up and down) then it can chatter. It's one of the reasons I'm not a big fan of double sided tape for hold down. Something like blue tape and CA is pretty easy to do and in my opinion fairly reliable for most applications. Not sure how you are holding down the material though.
If you want my quick guess at it I’d say you are actually cutting slow. The normal rule of thumb I use for soft material is no less than a 0.002" chipload. Which at 18KRPM works out to 72IPM. This changes based on the tool geometry, size, and material. But it’s an okay starting point as it will cut chips for most tool geometries. If there’s a lot of rapid direction changes then this will need to be higher. If memory serves, Amana recommends a chipload of 0.005" for most of their 1/4" cutters. However you need to balance “recommended chiploads” with cutting depth, material, and machine deflection.
The quick things that I’d check for are:
Make sure that you are inserting the tool as far into the spindle as possible without bottoming out the tool or clamping on a cut out section of shank (flutes, carry out).
Ensure that your material can't move in any direction when held down.
Make sure you are snapping your collets into the nut (for ER and like spindles).
If you are still getting chatter a good practice is to leave the material slightly larger than your finished size and do a clean up pass. How much you need depends on the material and tooling but it needs to at least be more than your chatter.
Any time you are burning your chipload is tool low or you have a very wrong tool. I don’t know what you are using but either increase your feed or reduce your RPM.
Hope that’s useful. Let me know if there’s something I can expanded on or help with.
Thank you for your advice! I’m just going to fiddle with it. First and foremost, I know I was using a downcut bit for the pegs, which is probably not a great idea. So I’m switching that up. I think I’ll just be playing with things while I work on these and see what happens.
The best I can say is that it seems like, even with the standard parameters provided by Carbide, the bit is almost slamming into a corner. I do tight corners and you can see the chatter there a lot. That seems to be the feedrate, I guess?
When I design something that will be cut out on a mill, or my shapeoko, I will put fillets in my inside corners with a radius larger then the cutter I plan on using to minimize the chatter that you are seeing.
The only thing I would add is to use a pocket toolpath on the outline cuts instead of contour. This takes a lot of pressure off the end mill and can help with the chattering. Just offset the outline slightly larger than your tool diameter and use a pocket toolpath.
Thank you for the suggestions! This will definitely help.
One more question, if I have a fast RPM and slower feedrate, given the equations, if I slow down the RPM and increase the feedrate, it could be better for the wood, especially maybe a harder wood? I’ve mainly been using 18k RPM on my VFD spindle, but I wonder if slowing the RPM but increasing the feedrate will help the chatter, thus producing a better result?