Tooling and Settings for Machining Laminated Particle Board on the CNC
Chip load - size of chips produced by the feed and speed (rpm). The right size is needed to remove heat while also producing a quality cut. Higher rpms and multiple flutes need higher feed rates to remove the right size chips.
Achievable feed rate - how fast are you going to be able to cut when considering acceleration and deceleration; if you're cutting mostly long straight shapes you'll be able to physically achieve faster feed rates than cutting small or parts with curves. If you're doing a lot of long straight shapes, you can use over two flutes to achieve faster feeds. If not, the extra flutes won't help much.
Depth of cut - how deep you are trying to cut in one pass; usually depends on the thickness of material, but also the diameter of the tool. You can use high up shear compressions or mortise style tips depending on the thickness of material. I prefer mostly mortise tips unless I'm cutting thicker than 3/4 inch material. Larger diameter tools can cut deeper in one pass.
Carbide - there are different grades of quality when it comes to carbide, and in most cases you get what you pay for.
Brands I like include Vortex, Lueco, Onsrud and Amana. Maybe start out with the cheap stuff so you won't feel bad when breaking a bit. Collets, tool holders and the spindle need to be properly maintained to get the best performances out of tools. Onsrud and Vortex have some basic feed and speed charts available online to give you an idea; you'll have to fine tune to your application.
Start out with a double edge (two flute) 3/8 compression running 16000-18000 rpm at 500-600 ipm. Don't plunge with compression bits if you can help it; use a lead in and lead out. For 1/4 diameter bits use 400 ipm.
It takes some experience but eventually you'll get a feel for it. Just remember, loud noises are bad in most cases, and something needs to be adjusted (feed, speed or depth of cut).
Depending on the size of the finished part and all of the other factors, machine condition, hold down, collets, you could expect to run at 16,000 rpm at 400 to 600 IPM. Most people do not need to run at 18,000 RPM. We [Southeast Tool] also have a free excel spread sheet that you are welcome to download from our web site. Keep in mind that these numbers are only starting points. The scientific way (LOL) that we tell people is to start with a number and start increasing feed rate until the quality of cut decreases and then back it off 10% and that is your optimal feed rate. This feed rate will usually be different for everyone.
From the original questioner:
We are running 3/4" and 1" material. 4x8 sheets nested by Cabinet Vision. We have a 3 flute compression bit for the cut outs and a 3 flute down shear for the dados. We aren't getting very good life out of either one, especially when we run it on one sided plastic laminate material. Currently running it at 18,000 rpm and 12 m/s.
From contributor L:
That is way too slow for a three flute. HPL material can be a pain though. I cut in multiple passes with a slower and steeper than normal lead in so it wears out more evenly and gets through the plastic before cranking up the feed. You also need the higher grade carbide for this type of material; and have one tool that's only used for a specific type of material. Straight flutes work okay on HPL if you're in a pinch.
From the original questioner:
Our laminate material is on the bottom 95% of the time, so it will be that last cut where it is being affected. So we may be burning our bits up running them too slow?
From contributor L:
With a 3 flute compression you should be going at least 800-900 ipm (20-21 m/m) when cutting laminated particleboard core, maybe a little slower for plywood and MDF core. It's hard to tell with particleboard, but you want tiny curly chips and not powdered dust. It's much more apparent in MDF and plywood. Heat destroys carbide and quickly dulls tools.
On the other hand, HPL has a nasty problem of chipping carbide where the plastic and carbide meet. Look at your worn out tool and see if you notice a tiny nick in the tip. Sometimes when the laminate is on the bottom, a small piece will get stuck to the tip when you cut through. You'll notice scorch marks on your spoilboard when this happens. The only real way to prevent this is to adjust lead in and lead out and number of passes at different depths until you get better results. Try using a rough pass with another tool if possible, so you're trimming the laminate rather than trying to plunge through it.
Sometimes when dealing with HPL board, it's best to just go through a bunch of cheap straight flutes at a lower feed rate, or in your case, keep the feed rate the same. Disposable tooling basically. I can get through about 10-12 sheets of hpl with a diablo 3/8 diameter/ 1 inch cel from using 2-3 passes. Not an ideal solution - people will probably laugh at you, but it works and it's cheap.
Maybe look into insert tooling if that is the primary material you're cutting and you cut a lot of it. These tools have a larger diameter and increased kerf, but you can replace and/or flip the carbide when it wears down.
I can usually get away with using a high quality 2 flute compression, but I'm not cutting more than 15 sheets at a time for most jobs.
Some people swear they can run 60+ sheets with Vortex Xp 3 flutes or similar, so there must be some combination of feed, speed and cut depths that works for them.
I tried one of the budget brand 3 flute compressions and the noises it made scared me enough to put it away until I get desperate enough to try it again.
From contributor O:
We finally switched to a pcd bit for our laminated panels. It seemed that within the last 6 months or so there was a certain change in how long our 3/8 compression bits were lasting. Our feed has slowed a little, but the cut quality is great and so is bit life.
We cut laminated particleboard all day. Make sure you're using a good grade solid carbide tool, not high speed steel. We buy from Leuco and have had really good tooling from them. We use 3/8" 2-flute compressions at 16500rpm and 800ipm. We're cutting 40-60 sheets per tool depending on the laminate grade. We try to use vertical grade laminate (as opposed to post form or general purpose) when possible because it's thinner, cheaper, and much easier on our tools. Make sure you're getting a good solid vacuum to prevent the sheet/parts from vibrating. Sometimes we have to wrap the edges of our sheets with 4" shrink wrap just to get the best possible vacuum. Also read contributor L's first post carefully - it has a lot of good information.
Would you like to add information to this article?
Interested in writing or submitting an article?
Have a question about this article?
Have you reviewed the related Knowledge Base areas below?