I mainly cut Baltic birch plywood and would really like to develop reliable strategy for reducing tear-out on the bottom side of the material. By “reliable” I mean will be mostly successful even when a tool isn’t “factory sharp”.
Feeds & speeds don’t ever stray far from each brand’s recommendations.
I have a vacuum system to hold down full 4x8 sheets but the waste board has scars that leave briefly unsupported traverses during final passes. But this shouldn’t be a huge issue I’d think…
Drilling -
Surprisingly even Amana Brad Point bits leave bottom side tear-out. Increased rpm + decreased plunge rates help but those are maxed to either end of their respective scales as dictated by the brand.
A partial drill with a final peck through the bottom side laminate with an up-cut endmill still seems problematic.
Standard Cuts -
I’ve tried offsetting the outside toolpath by 1/16" leaving that materials for a final pass with a compression bit with some success, but lining up all the tabs for those parallel (adjacent) cut path will be a bear on some of the more complex pieces…
Is this the best approach in the end?
And I’ve been using 1/4 bits to cut out shapes in 3/4" BB ply in effort to minimize material waste. Would using 3/8" bits have any advantages as far as bottom side tear-out? - like the cutting edge having a slightly reduced angle of attack due to the increased radius… ?
I run it at 18000 RPM and 30-60 IPM. I haven’t noticed any overheating but I do clean it frequently especially after cutting MDF. Its not going to last forever without getting dull but at this low price I always have a few on hand if one gets dull enough to break. The only one I broke was when I tried to cut 3/4" HDPE which was a really dumb idea even with a brand new sharp bit. The one I used had over a year of use on it so the increased density of the HDPE quickly did it in.
I run a vacuum table and I cut quite a bit of 2 sided UV coated maple plywood and the tear out from routing is minimal to non-existent. I use the Whiteside 2602 compression bits in 1/4" diameter. 300 ipm 2 passes (.375" DOC). I feel this is a bit conservative, but the bits last and sound great at this setting. I will usually cut .010" - .015" into the spoil board to be sure I do not leave any onion skin which tears way to easy.
Drilling on the other hand, I have found nothing that works. Brad point bits just splinter the veneer on the backside. I have gotten to the point where I do not drill all the way through or if I have to, route the hole instead of drilling if finish on the second side is critical.
Thank you Hack.
All great info. I’ll give your setup a try.
And comforting to know I’m not the only one that struggles with drilling.
I’m drilling 100+ 6mm & 8mm holes in 3/4 bb plywood per run so cleaning up the bottom side splintering gets tedious.
I may try partial drilling and then pocketing the last depth with an 1/8" upcut…
Consider the Amana 46170-k (1/4” compression bit). It’s my go to bit for BB ply and haven’t had any tear out on the underside. Runs at 18000rpm & 100-150 ipm. Use a hurricane vac system for holdown with a phenolic plenum board and LDF spoilboard.
The material I use for my bread and butter work is 9mm BB. I use the Whiteside 3/8" compression bit with 3/8" shank. I run it at 18000RPM at 200 IPM. I don’t ever get any pullout unless there are voids or other defects in the material… I don’t have vacuum hold down but I do use a pretty powerful dust collection system. I need to use tabs to keep the pieces in place.
Thank you all for the various tool/setting combos.
Many of your suggested cutters on the way for trial.
DRILLING…
I’m often poking 100+ 1/4" & 8mm holes in a single sheet of 3/4" BB ply.
It’d be awesome to solve the bottom side splintering issue. Fresh spoilboard for every sheet isn’t realistic for anyone.
I’m totally cool with multitool strategies.
In the same work discussed above there are dozens of holes and pockets per sheet. For the holes I drill with a 3/16" up cut, no pecking, whatever the recommended plunge rate is (50-60 IPM?). I find it best to drill right through, into the spoil board by about 20 thou. For pockets, I use a 3/8" downcut, 18K RPM 200 IPM. the downcut minimizes pull up on the edges and also results in smoother pocket surfaces. The tools and feeds/speeds for these I arrived at very iteratively.
Interesting considering most references I’ve encountered consider it a no-no to drill with end mills so I was steered away from this practice early on - perhaps the “rules of thumb” are usually based on metals machining where things are less forgiving?
I’ve always wondered how flute count and helix angle might assist in this scenario.
I see advantages to increasing and decreased both those variables… with tradeoffs for each choice obviously…
Ive had burning of the bit using straight bits to drill. Also, any time i’ve taken a short cut and tried to drill with a compression i,ve had burning. But the upcut bits work fine for me. This is in 3/8" (9mm) material. I’m not sure if it would be any different with 3/4" material.
I say Just give it a try. You would want to plunge as fast as you can imagine the bit being able to cut through. I just use that bits plunge rate from the database. If you go too slow it will burn for sure. I don’t want to peck drill if I don’t have to because my production runs on the machine are 88 sheets at a time. That’s why I take the effort to try anything that can save cutting time. Its the same for hold downs, sheet changes, everything! The machining times add up.
