Best method for thick leg assembly

[mjcisme (Michael Caputo)]

Hi. Wondering if you could guide me on best or better practice for this operation. The photo shows a leg assembly - 8/4 maple. I am using a 1/2” diameter bit in the 80mm spindle. 1” cutting length for cutting from top to 1” deep. Then a 1/2” diameter bit with a 2” cutting length for the next 0.84” of depth. Usually it gets a bit gnarly on that second step as it approaches nearly through cut. The bit will grab at the transitions of grain direction and try to move the piece. Luckily today I had enough crush it clamps in place to resist that.

I’m cutting 1/8” per pass and about 75 inches per minute speed. 18,000 rpm. So this is over an hour and like I said gets a little sketchy near the end.

I’m considering would it be better to just cut that first inch, then bandsaw the waste and then pattern route to finish. Not ideal as I’d rather the CNC do the whole job. But maybe that’s the smarter way. Thoughts??

[WillAdams (William Adams (Carbide 3D))]

Are you cutting a slot just as narrow as the tool?

[mjcisme (Michael Caputo)]

Yes, the curvy perimeter shape is a slot. The wood to the outside is waste. I gather that’s a bad thing?

[WillAdams (William Adams (Carbide 3D))]

Where possible avoid slotting and add geometry and cut as a pocket

Making vacuum hose adapters

While cutting up vacuum extension wands for this is expedient, it’s a bit problematic given that Shop Vac recently filed for bankruptcy, was bought at the last minute, and production hasn’t caught up. I need a receptacle for the Sweepy 2.0 dust fitting — one option would be to purchase one from Woodcraft, but Carbide 3D sells blocks of HDPE: which looks to be just barely big enough for things to fit. Measuring the hose fitting I get a diameter of ~63.5mm — offsetting that twice we arrive at…

and/or

Adding geometry to cut as a pocket with a finishing pass

One technique which is often suggested to avoid slotting is to add geometry around a part which one wishes to cut out and cut as a pocket down to tab depth — here’s one technique for that. In this case, the project is a bevel gauge which will be cut out of 0.0625" (~1.5mm) thick aluminum: [bevelgauge] Due to the narrowness of the angles, an 0.03125" endmill has to be used, so after importing and scaling the file (we will be cutting out one which is 3") we select the perimeter and offset it tw…

and consider leaving a roughing clearance and taking a finishing pass.

Best Bit for full cut through

One which has a cutting flute length equal to or greater than the thickness of the stock — pretty much any tool should work. Big thing is the toolpaths — if cutting out, rather than just cutting a slot: [image] Offset to the outside by endmill diameter plus 10% or so: [image] [image] [image] Then cut as a pocket: [image] down to tab height or the penultimate pass: [image] then move the contour down to below the pocket and start cutting at the bottom of the pocket: [image] and…

[Tod1d (Tod (with 1 'd'))]

You’re clamping the offal. Any tension from the clamps is being relieved as it cuts through and the tool is getting pinched. I suggest clamping front/back (blue) and let the offal… fall off

[mjcisme (Michael Caputo)]

Read the links. Thank you very much, Will. I understand.

[mjcisme (Michael Caputo)]

Thanks Tod. I understand. I put a lot of tabs in and with 3/8” height to try to resist that. Maybe still an issue though. For putting the clamps where you’ve drawn them, the only trouble is I’m going all the way through at top and bottom of the piece. Guess I could put big tabs where I put the clamps to have the CNC climb over them. Not sure that’s a good idea. Hmm.

[Tod1d (Tod (with 1 'd'))]

2 ops? Cut the bottom & top first, then move the clamps.

[mjcisme (Michael Caputo)]

Ah gotcha. Thanks, Tod!

[mjcisme (Michael Caputo)]

@WillAdams thank you so much. Did the offset with 0.55” for the 0.5” diameter bit. It made a world of difference. Much happier bit and spindle and woodworker! Thanks!!

[Emmess (Matthias Solga)]

for thick stock lately I cut a pocket (offset of the contour), then cut out the piece with a band saw (I use a scroll saw due to lack of space in my shop for a band saw), and then get the rest with a straight flush router. I do not have such a powerful spindle for 1/2" bits, so 8/4 stock is too thick for me to cut directly. It took me a while to understand the dynamics of chips in a narrow contour slot: upcut bits pull the bit out of the collet, so the bit cuts deeper and deeper, ends in a stuck machine and destroyed machine bed, and downcut / compression bits get stuck in the compressed chips. I paid some tuition fees in bits, stock and wasteboards…
Wills recommendations cannot be taken seriously enough.

[mjcisme (Michael Caputo)]

Yeah I’m learning a lot! Surprised how much difference the relief of only .05” (10% of the 0.5” bit) can make. Sure was a huge impact making that pocket vs slot.