Cutouts on Thick Stock

[lasereyes]

Hey All - 

I'm very new to CNC.  Yesterday I was running a test job on 1.5 inch thick Cherry, and ran into issues on the final cutout (profile path).  During the cutout there was substantial noise & chattering, and by the time I got to the shutoff my clamps had dislodged, dust shoe fell off, and workpiece was badly damaged and tossed off the table.  Scary, but lucky no damage to the machine (except the dust shoe was chewed up a bit).

I thought my settings were okay based on my experience with handheld routing, but obviously not.  In addition to the initial disaster, when I finally got running again, I noticed additional chattering and poor cut quality on the "separate last pass."  Here's what I was doing:

AR16 - Profile cutout
1.5 thick cherry
Brand new Whiteside 1/2" downcut 2-flute spiral bit
1/4" deep passes
Spindle at 18,000 RPM
Feed Rate at 200 IPM
Separate Last Pass at 1/16"

I'm thinking 200 IPM is probably my primary problem.  Honestly, I want to also believe that the bit is not as sharp as it should be, but I've never had a problem with Whiteside before so that's probably just my ego talking.  Clearly I also need to tighten my clamps better; I'd been trying to lighten up a bit but I guess I went too far in the other direction.

I will be doing cutouts on 1.5"-2.25" stock pretty regularly in the future for furniture builds, and I really need good, clean, precise profiles for joinery.  

Can anyone with a lot of experience with cutouts on thicker stock share some advice on where I went wrong ?  Would love to hear what produces the best results, whether settings, bits, , whatever you got.

Thank you.

- Theodore

[dadealeus]

Personally, I believe your issue might be with your downcut tool. Downcut tools are not great for deep pockets and, generally, should only be used for the first pass to prevent tear-out on the top of the stock. Then you switch to an upcut for better chip clearing.

Basically, that downcut tool is jamming all the chips into the work-piece. The deeper your cut, the less chance the chips have of escaping and your profile paths are going to get jammed with sawdust that the tool has to plow through with each subsequent pass (again, further jamming that same sawdust back into the path). This is especially true of the last pass that forces all of that debris out the backside of the stock - it will look for an escape path which is likely the small space between the back of your stock and the wasteboard. This will cause the workpiece to lift upwards as debris is forced under it - making the piece warp and press against the sides of the tool and increasing chatter as it starts cutting more stock - generating more debris, generating more lift, until failure or the cut is able to power through.

This not only prematurely dulls the tool, but also builds up a lot of extra heat as the chips are not able to be evacuated. Those two things together will definitely cause the chattering and additional friction that might have dislodged your holding clamps (speaking from personal experience here).

One way to tell for sure is if your tool has any darkening on the cutting end - that would indicate a lot of heat buildup.

It's a pain, and most of us want to lazily cut with a single tool (at least that's true of me), but I would either use a compression tool (https://www.amazon.com/Whiteside-Router-Bits-UD5122M-Compression/dp/B000K2CCIG) or I'd run the first path with the downcut and then switch back to an upcut for the rest of the job.

I think that will take care of your issues.

In short, if your spindle mount is trammed properly, and your workpiece is secured sufficiently, there shouldn't be a limit to how deep you can reliably cut outside of your Z-axis travel constraints and deflection that may occur in a long, thin tool.

[lasereyes]

That is super helpful dadealus, thank you very much. After thinking through it a little more today, I was starting to come to the same conclusion about the downcut spiral. I think you are spot on with your comments, and great advice on switching bits after the first pass; I will definitely start doing that for deep cuts in the future.

[dadealeus]

Sure thing. I hope it helps.

One other thing that might be worth trying would be a straight cut endmill:

www.amazon.com/gp/product/B000K2EAIG/ref=ppx_yo_dt_b_search_asin_title?ie=UTF8&psc=1

I use that exact one for a ton of my cuts and it leaves a great finish on both the top and the bottom of the stock. Straight cut tools tend to dull more quickly than an up or downcut tool, but for the price, you can buy a few to spare and save your up/down endmills for when you really need them.

You might still run into the same issue with thicker stocks (1.5" and up), but I've cut plenty of 1.5" deep profile paths (1/4" DOC) with that tool without issues.

I'd give it a shot; it might save you some tool changes.

[joeblow]

I cut a lot of wood on my machine ranging in thickness from 4/4 - 8/4+. I typically only use downcut bits with a 1/2" 2-flute endmill or a 1/4" 2-flute endmill. Keep in mind that during a profile cut you are experiencing both a conventional and climb cut at the same time. A lot of forces at play here that also lends itself to quite a bit of heat buildup.

I first cut a pocketing toolpath with a width 1.5x the diameter of my bit and depth about 75% the thickness of the wood I am cutting. This will act as a relief pocket for chips and also gives me the choice of conventional vs climb cut. I will then cut the remaining thickness out with a profile toolpath. Not a big deal as I save both toolpaths as 1 file. The relief pocket gives me the opportunity to keep chips vacuumed out of the cutting path and keeps the bit cooler.

When I started with a cnc I had the same problem you are experiencing. After switching to the pocketing followed by the final profile cut, I have had no problems with thick stock. Keep in mind too that solid wood is an entirely different animal than HDU, plywood, plastics, etc.

[lasereyes]

Definitely helpful, thank you dadealeus.

Thank you as well joeblow. Outstanding idea create a wider channel for chip evacuation. That seems like it will definitely help ease the cut & achieve a high quality edge on the workpiece.

Cutting a wider channel + bit change definitely get me pointed in the right direction here. I can't thank you guys enough.

[aluomala]

Nov 9, 2021 5:19:24 GMT -5 joeblow said:

I cut a lot of wood on my machine ranging in thickness from 4/4 - 8/4+. I typically only use downcut bits with a 1/2" 2-flute endmill or a 1/4" 2-flute endmill. Keep in mind that during a profile cut you are experiencing both a conventional and climb cut at the same time. A lot of forces at play here that also lends itself to quite a bit of heat buildup.

I first cut a pocketing toolpath with a width 1.5x the diameter of my bit and depth about 75% the thickness of the wood I am cutting. This will act as a relief pocket for chips and also gives me the choice of conventional vs climb cut. I will then cut the remaining thickness out with a profile toolpath. Not a big deal as I save both toolpaths as 1 file. The relief pocket gives me the opportunity to keep chips vacuumed out of the cutting path and keeps the bit cooler.

When I started with a cnc I had the same problem you are experiencing. After switching to the pocketing followed by the final profile cut, I have had no problems with thick stock. Keep in mind too that solid wood is an entirely different animal than HDU, plywood, plastics, etc.

I haven't had to do a lot of thick stock cutting (I mostly do 3D carves, using 5/4 and thinner wood), but I had to do a project that involved cutting 1.5" oak, and I wish I had thought of using this technique. I had to cut out 14 pieces (about 30" x 12"), and I used a 1/2" bit and I am sure I ruined the bit because I did it the same way I normally do my profile cuts on thinner material (usually with a 1/4" endmill, both upcut and compression) and it was screaming and the bit darkened. I was more worried about getting the project done quickly than anything else, and went full steam ahead and just did a regular profile (with a separate last pass of about .02"). The funny thing is that when I do my 3D carves, I always do a roughing pass that exceeds the model boundary by about .125" (for a .250" ballnose), just to give the following finish pass bits some "breathing room" when they plunge down to the edges/bottom (using 1/4" shank tapered ball nose (TBN) bits). Otherwise, these smaller bits end up rubbing against the walls where the 1/4" ballnose did its work (on the roughing pass).

So, it's basically the same idea: create extra space so the bit isn't working on 2 (or more) sides, allowing the bit to stay cooler, and the chips to be cleared out. Of course, it takes a bit longer, but as you mentioned, if you program your separate  toolpaths (pocketing and then profile) and save it as one toolpath, the time difference is negligible  and you save on expensive tooling (a 1/2" carbide bit runs about $150CDN), and end up with a smoother finish. 

Thanks for sharing this tip! 

Allan

[joeblow]

Glad this will help both of you out.

Lasereyes....keep in mind that your hold down techniques really have to be rock solid. If you use the hold down clamps from Axiom or somewhere else, you might be very surprised how they loosen up a tad during deep cuts. When I can get away with it I always shoot my stock down with a brad nailer or use #8 trim screws that are readily available at most hardware stores. The MDF for the spoilboard is much denser than the MDF from the big box stores and holds a brad or small screw quite well.

[dadealeus]

Yes, sorry; I had assumed that cutting a wider channel was the first thing that would have been tried if it was a possibility. A lot of times that's not possible (if you are cutting at the maximum dimensions of your machine already or don't want to waste any additional material on buffer space).

-but, yes, simply cutting a wider channel will work fine, too, if you're ok with the loss of extra material.

I do a lot of molds, for example. An extra 1/8th of an inch on a 1.5" deep channel around a 2'x4' cut path adds a surprising amount of volume to that channel that would then need to be filled with something expensive (silicone, epoxy, etc.).

Regardless of what material you're cutting, the rules are the same: reduce friction (heat) and don't re-cut chips. There's a reason why all endmills are not downcut endmills. While you *can* do a lot of things with the wrong tools, it doesn't mean you *should*, or you'll just have to re-learn a new cutting process when you meet a material it doesn't work well with. This applies to wood, metal, plastic, foam, you name it. Find out what chip clearing setup works for each one and you won't have many issues (on an Axiom machine) regardless of what you're cutting so long as it's non-ferrous.

As far as work-piece holding goes, if you're using the Axiom hold-downs, make yourself a wrench to tighten them with and you won't ever need to use screws or nails. I've never had an issue with a work-piece slipping when I've tightened with the wrench.

Here's one I made with a handle and, immediately below my post, Gerry included his (a knob format):

axiomprecision.proboards.com/thread/1085/axiom-holding-clamp-wrench

Caution: using the handled wrench can literally shear your clamps off if you over-tighten them (speaking from experience). If you do use a wrench, simply tighten by hand until it becomes difficult, then use the wrench to go another half-turn or so.

EDIT: That's actually my old design. On the most recent version, I included a hole in the center of the wrench for the bolt to pass through if it needs to:

Attachments:

[redwood]

I cut a ton of 1 1/2" material, albeit a much softer redwood. I use a 1/4 upcut end mill, running 80 in/min, and never in 6 years have I had a issue. And yes, I frequently check my holdowns. Occasionally they do loosen up.