Not Sure reason for tear out and burning

[Captive]

I was cutting out a round maple plaque and when cutting out the perimeter I got some real bad tear out on the edge... not sure why.

Material thickness 0.85
Cut with Straight cutter
3 passes
Rpm 12k
Feed 0.7 ips
Climb cut
Material: Maple
No vacuum

The circle is about 24" in Diameter and I don't have a vacuum so I just left a large tab at the top and bottom and was just going to remove it with a flush trim router... it looks like the tear out is just before when the tab starts..

And also getting some burning with the V-Carve "king".. but I am suspecting this is just a matter of dialing in the RPM and feed speed...

120 Deg V bit
0.7 ips
RPM 18k

Any recommendations would be much appreciated..thanks

[knight_toolworks]

cut is pretty slow I don't usually go below 1ips. but I only use 18k when I am cutting really soft woods that are prone to tearout on v carving. maple is pretty easy so get the rpms down to 12k or less. using a downcut bit to cut the part out is best. if you don't have wood on both sides of the bit then only use a climb cut.

[Bob Eustace]

Try a 1/4" down or up spiral bit and bump feed up to at least 1.5. You are being toooooo cautious! With the V bit drop to 13K and again up the feed. Try not to use low end bits as this markedly affects results. you can learn about chip loads etc. by doing a search plus its built into SB3 but the easiest way is just listen to your cuts as you quickly learn just by sound. You do need more tabs though. Your router idea is sound. Amana have a magic trim bit with a 3/16" ball bearing. (Cheapest price is on Amazon) This fits easily into 1/4" slots and its very, very quick. We have a table permanently set up just for this and use the Bosch Colt for sheet work. Did you get the tool starter kit with your machine? If not order one as its great. The most common bit used for CNC has to be the humble 1/4" solid carbide spiral cutter. Its amazing what you can do with these. Top cutters equates to surperb minimum sanding finish.

[Brian Harnett]

Yes feed is too slow maple burns easy you want the cutter making chips not fine dust, spiral bit will cut smoother.

[dlcw]

Like has been said, feed rate is to slow. Think about using a router table or hand router. If you move the router/material to slow, the bit will burn the wood. Same principle on the CNC. Same principle on the tablesaw.

Believe it or not, I use a 1/4" compression bit for cutting hard and soft woods. Don't use the mortise compression bit which has a smaller up cut section at the bottom.

I first do a climb cut at about 4ips with 13K rpm leaving a 1/32" skin. Depth per pass is dependent on the wood type. Harder woods like maple, hickory, etc. I use no more than 1/4" per pass. For softwoods I will cut 3/8" per pass. The climb cut will significantly reduce tear out, just like with a router table or hand router. I then do a full thru conventional cut pass. I'll slow my feed rate to about 3.5ips and use the same bit rpm. The beauty of this setup is you can save both toolpaths to one file (if you use the same bit from the tool database) and have it all done without starting a new cut file.

It is important to remember that with a compression bit, you need to plunge down about 3/16" at the start of your first climb pass. The upcut spiral on the bottom of the bit will cause tearout if you do a regular ramp cut into the wood.

Make sure the bit is VERY sharp. I tend to NOT resharpen bits as the bit is not nearly as sharp as a new bit. Just my opinion and about 7 years of trial and terror. LOL......

[Captive]

Thanks your for the advice, it is much a appreciated, I will increase the feed speed on the next one... but just a quick question with regards to material burning when V-Carving is a matter of just dialing in the RPM and IPS or does any one change anything in the VR settings as well

[genek]

Who is the King???