Cut length of bits questions

[skintigh]

I'm a little confused on a basic concept: the cutting length of bits. Say I have a Onsrud 57-260 with 3/16" diameter and 3/4" cutting length. I believe I'm only supposed to cut plywood around 3/16" deep per pass.

So what is the rest of the cutting length for? Is it re-cutting/cleaning the cut from the previous pass? Is it just removing material and not cutting (maybe that's more applicable to an upcut bit)? Is it there just in case you want to cut something soft at 3/4" per pass, but otherwise it's doing nothing at all with plywood?

I think the shaft on that bit is as wide as the flutes are, so theoretically I could cut much deeper than the cut length, but I assume that would be bad for the bit and/or burning the makerspace down. Is that correct?

Thanks!

[Chuck Keysor]

Hello Bob..... You are referring to a general rule of thumb, which is used reduce the chances of snapping off a bit. If you are cutting Styrofoam, you could of course take much deeper passes. If you are cutting brass, well, you could only take cuts of maybe .01" per pass. But for cutting run of the mill wood, plywood, plastic, well, not having the pass depth not exceed the diameter of the bit is a reasonable starting point. And, I am no expert. Many people here are experts, and this topic has come up many times before.

I order to search this form to look for the information you want do a google search for: bit cutting depth site:talkshopbot.com
Well, the general format to do a google search on this forum is: SUBJECT XYZ site:talkshopbot.com
You can put quotation marks around important phrases, or use * as a wild card.

Anyway, even what I just told you here, is what I have learned here on the forum. And, I have a notebook for Shopbot, where I write down important things I see here on the forum.

Good luck, Chuck
PS: I didn't know your name, and I have never met a Bob I didn't like, so I called you that...……….

[steve_g]

“Bob”

Some of us cut very thick material… 3” solid pecan is not uncommon for me. You’d like your cutting length to be as deep or deeper than your material so that you can do an “onion skin” cut. When stepping down 1-bit diameter at a time through thick material, you’re left with a cut edge that has “water marks” or horizontal lines reflecting each step down. You can eliminate this undesirable look by making your last pass very shallow and a few thousandths inside (or outside depending on the situation) the original path.

If you were cutting 2” material with a bit with 1” CL, if doing an onion skin cut, you’d be rubbing on the shank and either break the bit or get a tapered cut.

A bit properly sized to your material will last longer… you don’t buy all 3”CL bits in case you might some day need the length. A very long bit cutting ½” material is likely deflecting.

A 1”CL bit is less costly than a 3”CL one…

These are three quick reasons for using properly sized bits… I’m sure there are more!

SG

[skintigh]

Thank you both!

Steve, if I'm not doing an onion skin cut, is there a danger from cutting deeper than your length? Most of what I'm will be sealed, primed and painted anyway. I searched online and half said that cutting deeper than the cut length was fine and half said chips would get caught in the slot and rub against the shaft.

I ask because I need to cut a lot of thick exterior corbels, some 3ish some 5 inches thick. I could cut them out of 4x6s, or glue up douglas fir 2x12s and cut them, or cut 2x12s then glue them. I'm leaning towards the latter, but either way I need to buy a new bit, and I don't have a jointer so I'm worried about the 2x12s warping.

Thanks again and I have a name now,
Seth

[steve_g]

Seth…

What I do, and what works for me isn’t necessarily gospel!

I don’t go deeper than CL when using a down cut bit. There are enough members here that have experienced fires when using down cut bits, especially when chips are trapped, that it would seem unwise to do so. Trapped chips are a certainty when drilling…

I do cut deeper than CL (when cut diameter is equal to or greater than shank diameter) But carefully watch for good chip evacuation. I’ll use an air hose to assist them if I’m not happy with how they are ejecting.

It sounds like it wouldn’t matter much if you got a little bit of chatter from chips getting caught between the shank and the material.

Those are nice corbels you show in your other thread!

SG

[coryatjohn]

If you're not doing production work, you can certainly go deeper than CL. As SG mentioned, just keep an eye on the cut and have an air hose standing by if the chips start to clog up the kerf. Forget downcut bits for this too, unless you like the smell of wood smoke.

[dlcw]

I use down cut spirals all the time in my work. The material I'm cutting depends on the depth of each pass. Ash and hickory are VERY hard woods. With a 1/4" down cut spiral I will cut about 3/16" per pass. This allows for good chip evacuation and reduces the risk of breaking the bit. For woods like alder or poplar, software woods, I cut 1/4" to 5/16" per pass. For 3/4" plywood, with a 1/4" compression bit, I climb cut in one pass leaving the onion skin. I then do a conventional pass to clean up the cut cut thru the skin by 1/32".

I tend to cut, leaving an onion skin, in the climb direction with the step downs. The climb cut will tend to force the bit AWAY from your cut line. But like SG says, it will leave tool marks. The way I fix it is to make one final conventional cut at full depth 1/32" thru the onion skin. This conventional cut pulls the bit TOWARD your cut line and cleans up the tool marks from the climb cuts.

This has worked well for MY setup over 9 years of cutting plywood (several thousand sheets) and solid wood. I've only had one problem. I bought a new set of ER collets and the 1/4" collet let the bit slip and the bit cut all the way thru the plywood and 3/4 of the way thru the 3/4" spoil board in one pass. And this with a compression bit with a CL of about 1". Didn't break the bit. I was really surprised! I went back to my old 1/4" ER collet.

The important thing is to figure out what works for YOUR machine. The experienced users on this forum have spent a long time perfecting what works best for THEIR machines. What works for one won't necessarily work for someone else. Each machine is different has has its idiosyncrasies. The challenge is to figure out what those area and learning how to compensate for them. Trial and terror!

[skintigh]

Thank you Steve!

Don, it sounds like I could have save a ton of work doing it your way. I've spent 10-20 hours so far puttying and sanding all the spots that tore out from the bottom of my porch bracket cuts, and damage from tabs. Just to clarify, you are plunging the compression bit in 3/4 deep into the plywood and rough cutting in one pass? Wow. Though I was cutting pretty fast at the end -- I got it down from 45 min per bracket to 15, and was cutting cleanly at 324 IPM, or 360 IPM but with 2 flaws, always in the same mirror-image locations. It was uncanny. I don't understand why. Actually, I took pictures, maybe someone here can tell me why...

20180620_170634.jpg20180620_170515.jpg

It made a ga-BANG noise when it did that, but the rest of the 2'x4' sheet was cut cleanly. I thought a chip just got caught and it was a fluke. Then it happened again in the exact same spots, so I went back to 324 IPM.

[Chuck Keysor]

Seth, on the vector drawing of your bracket, zoom in on the location where you got the little bit that chipped out, and see if you have some small, knot in the vector, or lots of nodes......... The fact that the same thing happened a second time would suggest there is something in the drawing used to generate the tool-path. Chuck

[skintigh]

Ahh, good call. There were roughly 10,000,000 knots after my scans and I got good at removing them, first manually then with some curve tools, but I bet I missed some. It's weird it would only happen at the highest speed though.

With later scans I found if I paint the object white before scanning it I got far less knots. From there I converted groups into single curves/splines, and was able to convert some of my corbels from ~10,000 vectors to around 8.