2

I have a question about the optimal number of passes for cutting 3/4" plywood with a CNC machine. I've been using 3 to 4 passes, but I've noticed that only the head of my bit seems to be doing the cutting, while the rest of the bit looks almost new. As a result, I've had to replace my bits frequently, typically every week or two.

I haven't tried a full cut because I was not sure if my spindle can handle it. Most of the videos on YouTube that I've watched recommend using the same method I'm currently using.

Can you offer any advice or share your own experiences with me?

Mironline
  • 289
  • 3
  • 7
  • Optimising cutting performance is all about the right feed rate | speed for the cutter in question, in a given material. As such minor variations in either the cutter geometry and/or material properties could have a significant impact, making generic advice only useful up to a point. So, regardless of any advice you read elsewhere or get here this may be something where you have to do some experimentation, and I suppose the first thing to try is cutting through in only two passes — since the rest of the cutter is apparently experiencing almost no wear, asking it do to more makes sense. – Graphus Apr 03 '23 at 05:32
  • ...typically every week or two... How much material is that? A week could be pretty respectable if your CNC is running all day every day, or it might be just a sheet or two if you're a weekend warrior. ...I was not sure if my spindle can handle it... That seems like something that you could figure out with a short test, no? Start very slow, and increase feed rate until you get a good cut with no burning and without taxing the spindle. – Caleb Apr 07 '23 at 20:58
  • What CNC do you have, and what are your feed speed and RPM? What bit are you using? – Triplefault Apr 07 '23 at 23:18

2 Answers2

2

Honestly, there are too many variables to give a simple answer.

Some things which affect your optimal cut depth:

  • Spindle speed (RPM)
  • Feed rate
  • Tool geometry*
  • Tool material
  • Tool diameter
  • Wood type**
  • Rigidity of your CNC machine

*Tool geometry can differ in the following ways:

  • Number of flutes.
  • Cutting angle/rake angle
  • Straight or spiral flutes
  • Special chip-breaking edges or other features of the cutter
  • Flute clearance depth
  • End geometry (if not doing a through-cut)

**Wood type - even with plywood, there are different kinds of ply. Your "standard" marine-ply may cut very differently to e.g. baltic birch ply.

More generally also, composite materials (plywood is a composite of wood veneers and an adhesive - usually a formaldehyde resin) can be quite wearing on cutting tools - moreso than even very hard solid wood species.

You haven't listed much about the type of cutter you're currently using, but generally, you can get improve cutting performance by:

  • Going from a straight-fluted bit to a spiral-fluted bit. Note however that a spiral upcut bit will cause tear-out on the top edge. If you are through-cutting the board in one go, you may want to choose a "compression" bit, which has an upcut at the bottom, and downcut at the top, which greatly reduces tear-out on the faces, particularly for laminated materials.
  • Going from HSS tools to carbide-tipped or solid-carbide, or at the top end, polycrystalline diamond (PCD) - these get more expensive as you go up the scale though.
  • Upping the RPM - so long as your CNC and other important components (collets, toolholders, etc.) can handle it.
  • Selecting chip-breaking or hybrid tooling for your router bits. If the finish on the edge of the pieces you're making doesn't matter too much, you could also use a "roughing" cutter - these usually have "serrated" edges which assist in chip-breaking and clearance, giving faster, more efficient cutting performance at the expense of finish quality.

Ultimately, unless you buy a router bit from a manufacturer who has done the testing specifically on plywood and can give you guidance as to RPMs and feed rates (which, if you were a manufacturer buying from an industrial tooling company, they would), then selecting the right speeds is usually a matter of trial and error.

I'd like to also redirect you to my answer about spiral router bits, which goes into a lot of detail about using router bits in general, here: When should I use a spiral router bit?

WhatEvil
  • 3,948
  • 14
  • 30
2

My boss had a Biesse Rover big-iron cantilever. It could cut 3/4 poplar-core ply in one pass using a 3/8" two-flute solid carbide compression bit. RPM was 20,000 at 19 meters/min, conventional cut. The spindle was 15-20 HP, up to 24,000 RPM. There was just the absolute slightest hint of deflection, a couple thousandths of an inch at most, which we'd counteract by a 0.01" offset, then take the rest during onion-skin removal.

My Shopbot PRT Alpha with a 2HP spindle used a 1/4" single-flute solid carbide compression bit. I ran 3/4" ply at 2 passes, 15,000 rpm, 10 meters/min, climb cut, then a final conventional cut during onion-skin removal. The structure of the Shopbot was much weaker and had 1/32" (0.03") deflection, which was used as an automatic offset during climb-cutting. The final conventional cut ended up on the line. I never tried a single pass because of the less-stiff structure.

Triplefault
  • 146
  • 1