I cut hardwood (maple and walnut laminated together) for the first time today and experienced a lot of tear out. I figured since I was using a 1/8th mm bit (I mostly use a 1/4 bit) increasing the spindle speed would help. The next cut had more tear out. So for the next cut I decreased the spindle speed and had even more tear out. I’m using a quality bit that I got from bits and bits and its almost new. Not sure what’s happening should i slow down my feed rate? I’ve got it set to 70 in/mm which is less than I usually use for ply or mdf.
What kind of tear out? Is it at the top of the board tearing up as it moves along or bottom of the cut tearing chucks up or when entering or exiting the wood?
I’m doing a 2d contour cut with an 1/8th inch down cut endmill and the sides are rough like its tearing through the wood rather than cutting through it.
feed: 70in/min, speed: between 3 and 6 on the Makita, DOC: 1/8inch
The bit is basically new. I think I used it 1 or 2 times previously on some pine.
Sometimes depending on the piece when I cut along a curve the fibers tear a little bit regardless of direction. What I generally do is run a final pass .02” inside my profile at full depth. Run it twice, once in conventional and once in climb. It’ll be like glass. Go like 50ipm on the first cut and 100 on the second with an 1/8” end mill. Works for me every time
2 Likes
@BillSpencer86 I’ll give this technique a try. I often just give up and just use a little radial “Stock to Leave” on the rough pass and do a finishing pass with a downward end mill that takes it to spec. It means I have to change the bit but it’s better than tear out on hardwood.
Let me know how it works for ya, I generally do this with a compression end mill as well to prevent the bottom tear out and eliminate the bit change. The spetools 1/8” compression on Amazon are like 5 bucks a piece when bought in a 5 pack and cut very nicely (compared to Jenny at 30 ea.) hope that helps
1 Like
Jim’s suggestion is a good one - you will get a better surface finish overall.
I generally do DOC=0.0625 @ 80ipm @14K RPM (2 or 2.5 on the Makita) with a 0.125" bit without problems.
If I’m not cutting too deep, then I bump up the feed rate to 120ipm.
I’ll note, Amana recommends derating their recommended feed rate by 50% to 100% if you are cutting >1x the diameter of the bit:
† Depth of Cut:
1 x D Use recommended feed rate
2 x D Reduce feed rate by 25%
3 x D Reduce feed rate by 50%
Just something to consider that some overlook.
1 Like
I did job of 100 identical pieces at 1.5" deep with an Amana 45426 straight cutter in Hemlock. As far as feeds go, 18K RPM and 150ipm. I did chase the cuts with a screwdriver and vacuum to clear them for the next pass. PITA. I love that 45426, it still wants to work for me, I use it for area clearance too.
There is a way to split up your toolpath in VCarve, instead of cutting a full profile you would cut the vectors, then cut the endgrain first, and only then along the grain.
Takes a bit more time in the CAD, but in some of my projects I completely eliminate any tear out.
Man, wish I’d have read this earlier. Thanks for the tip!