Cutting OSB not going to plan

[v3juggler]

Hi!

I tried cutting some stuff from OSB, as I’m preparing to cut Ryan’s table base + torsion box for when I will convert my LR3 into LR4.

I think I understand everything about feed rates, flutes and DOCs, but still things are going sideways! So irritating!

Eventually I used precisely settings (and bit, new!) from Ryan’s post here: Full size LowRider table base - #77 by vicious1 and it didn’t work too!

Makita was really struggling. Taking RPMs up did not help a lot and it lost steps at some point and I had to stop the job. Result below:

My ideas:

• cheap endmills I’m buying from Aliexpress are shit from day 1.
• belts are too tense (coz they are definitely not too loose)
• my LR3 is shit coz I build it wrong?

Gimme some wise words, folks!

Thank you!

[vicious1 (Ryan)]

Please show us your

Picture of your build.

Feedrate, spindle rpm setting, depth of cut.

exactly what endmill are you using.

[vincentw56 (Vincent Wright)]

OSB splinters pretty easy (which can cause it to catch) and just like plywood, the glue is usually harder than the wood. So, a very sharp bit is usually recommended. Any time I have issues, it is always a dull bit.

[v3juggler]

OK, here is my build:

I started 2 on Makita dial. Then I tried 3+ when things went south. 6mm single flute upcut.

[vicious1 (Ryan)]

1-What diameter is the endmill, 6mm? 2-How far out from the end of the collect does it stick out?

9mm/s feedrate @ 8mm DOC, ~2 on the makita dial rpm. I assume the finishing pass is something like 12mm @ 18mm/s, but 3- what is your finishing pass step-over? (sorry I have zero concept of 540mm in 60 seconds).

One issue with your build is you absolutely need to secure the vac hose to the top of your core, 100%. Not doing this is going to jack up your accuracy in every direction. Slap a zip tie on it.

Your numbers should be simple for the machine to do. So either that endmill is garbage, or the vac hose is pulling harder than you think.

I would do the same thing just use a 4mm DOC, increase the rpm to 3-4 if you have to, use a 0.6mm finishing pass with at full depth.

[Tokoloshe (Philipp)]

DOC of 8mm is pretty optimistic though with a 6mm endmill on a LR3, rather speed the feedrate up and reduce the DOC.

[v3juggler]

I copied settings Ryan used to cut his table base, BUT! I have forgotten there is machine difference - I’m on LR3, him on LR4.

That said, should there be difference in router struggle?

I will try to use new bit from another factory, and connect my pipe to the core and go down to 6mm DOC as Toko suggest. I will keep you posted.

[Tokoloshe (Philipp)]

Ryan used MDF though, not OSB, didn’t he? That’s a huge difference.

[v3juggler]

No, check the link I posted in the first post:

Full size LowRider table base

[PXL_20251022_202153125] 55 minutes, and I am not pushing it very hard. Router was at 1.5-2.5 on the dial. 1/4" single flute upcut. [image] [PXL_20251022_203123177] [PXL_20251022_203157639] Diagonals are far under what I can measure. [PXL_20251022_193619155] Working. I am going to drop the plunge rate 1mm/s, increase the feedrate 2mm/s and finishing pass probably 5mm/s Estlcam said 1:04, it was done in 55min. That is pretty accurate.

[Tokoloshe (Philipp)]

Oh, apologies. Interesting.

[vicious1 (Ryan)]

@vicious1

I would do the same thing just use a 4mm DOC, increase the rpm to 3-4 if you have to, use a 0.6mm finishing pass with at full depth.

Start here and work up. Always best to start light.

I have gone much faster, but it is very machine, material, and cutter dependant. Also, the heavier cuts seem to do better with conventional milling, instead of climb.

[Terry_O_Sullivan]

i run 18 mm pine treated ply which is bloody hard cutting at 4.5 mm dep’t of cut at 850 mm/m 6mm 2 flute down cut no finishing pass if i know the sheets are fairly fresh out of kilm ill run them at 5mm

which is on safe side for those really hard knots on lr4

untreated ply i run at 1050 mm/m same depth , ive done fair bit of time comparing setting’s

and over all ,dropping back to theses settings over say a 5-6mm doc is only few mins dif ,but upside if does hit hard pieces it will still cut through , not stall and ruin my tool and have LR walk of the rails, ive learnt patience is key in this game

[vicious1 (Ryan)]

@Terry_O_Sullivan

2 flute down cut

A two flute down cut is extremely slow as compared to a single flute upcut. downcuts pack the material down into the cut, and a two flute has very little room for chips. Single upcut can hog material out and throws it up and out of the way.

A single flute with a finishing pass should get you the same edge quality faster.

[Terry_O_Sullivan]

agreed i did try that but some of the ply we get is just rubbish

even with finish pass of .5mm would blow out top edge , this way i know I’m not getting damaged edges