I've seen in a few threads people have put pictures of large plywood construction folded horns where they did CNC manufacture. I'm going down that path with one of the Woden designs horns for some Alpair 10P that I've been breaking in. There's a couple local shops that do custom CNC plywood work and claim to have a decent supply of good voidless plywood since that's usually what you want for CNC anyway. I'm doing the CAD work and things like board thickness, cutting tool size (for dogbone corners) are all constrained so I can adjust after they bring in the material and let me know what tooling they'd use. Generally I'm interested in any advice from anyone who has gone through it, but I did have a couple specific thoughts/questions:
Any advice on how much tolerance to add to the board width when cutting slots? I'll try to ask them to check how much variation there is in the material once they get it, but there's also how much to add just so I'm not having to sand or hammer stuff together. I can't decide if it's worth adding much tolerance on the board length (at each end of the slot) as well, since presumably the CNC itself cuts the length quite precisely.
Any thoughts on how deep to go with slots? It seems like really it's just to align them, the glue is doing the work. I was thinking only 3mm or so deep out of 18mm thick plywood. Going deeper would probably just weaken the sides and would make it more sensitive to aligning the other side when gluing up.
Any advice on how much tolerance to add to the board width when cutting slots? I'll try to ask them to check how much variation there is in the material once they get it, but there's also how much to add just so I'm not having to sand or hammer stuff together. I can't decide if it's worth adding much tolerance on the board length (at each end of the slot) as well, since presumably the CNC itself cuts the length quite precisely.
Any thoughts on how deep to go with slots? It seems like really it's just to align them, the glue is doing the work. I was thinking only 3mm or so deep out of 18mm thick plywood. Going deeper would probably just weaken the sides and would make it more sensitive to aligning the other side when gluing up.
If you're talking one of my horns -if you want good performance, don't round over or smooth out the internals. The edges & changes in expansion are specifically designed-in as functional parts of the low-pass filter, so smoothing those out will significantly raise the acoustic low pass filter from the design frequency (potentially moving to a shallower slope also) & increase audible GD as a result.
For my last project I used CNC cut sheets, 18mm birch ply, and ended up with wobbly 21inch subwoofer cabinets. It turned out the machine was not calibrated or tuned or whatever, so for a complete y movement the cutting head moved 1-2mm in x direction. They hadn’t checked the squareness of the machine, because for all their precious work this deviation of squareness apparantly wasn’t a problem. The discussion is still ongoing on how we solve this and stay friends 🙂. Don’t make the same mistake and make sure they know what they are doing and what you can expect on accuracy in all dimensions, x, y, z and diagonally. Good luck with your project!
Btw, I used 8mm slot-depth for 18mm ply.
Btw, I used 8mm slot-depth for 18mm ply.
"Its a pet peeve", but many designers with varying levels of experience interchange the words "tolerance", which is the feature based
allowance of deviation, typically specified by reference to a "mean" dimension ... where what they really mean is "clearance", or
a "fit" between members.
I think you are asking about the "fit", resulting in a clearance between joined members. Of course, that, too is "feature specific". But to get
the ball rolling, in 18mm {11/16" actual, 3/4" spec} plywood, when joining a male feature with a through hole {full depth} with an allowance for glue,
I would normally specify 1/64" per side, or 1/32" total clearance, max. This gives enough "room" for the glue to flow into the joint without
being "wiped out" by the construction method. Its also called a "slip fit" in wood.
If using a "biscuit system", e.g. Festool biscuit joiner, one can significantly tighten the fit between pin and hole, while "relaxing" the true
positional accuracy, a.k.a. "tolerance". If combining a CNC placed feature and an oval section biscuit, one might argue that the
joint can be improved while the "accuracy" is unaffected -- when compared to CNC produced "custom" male and female features.
On a blind hole, which is what you've asked about, without "corner relief" of the inside "abutting" feature {e.g. "chamfer"}
... perhaps +/- .004" {.1 mm} is about right. Tighter than that, you risk "hammering the tongue" into place. IF you need aligning features
{e.g. multiple "timed" tongues, e.g. a LEGO block} you need to tighten up your "locational accuracy" and loosen your clearances,
allowing all the male features to "float" a bit into true position.
The "machining tolerance" is a function of a) the specific work-holding method and its accuracy, b) the capability {repeatability and
accuracy} of the machine itself, and the dimensional accuracy obtainable without using pre-selected materials, as there is
variability in the thickness of materials -- which can affect the design and accuracy of work-holding. This is controlled mostly
by the feature selection and relief required to assemble them into sets.
The machine accuracy {"minimum tolerance"} on a typical CNC wood router is +/- .002" or less ... which is almost irrelevant, since mounting a typical
sheet to that alignment can be very challenging, especially when using clamps.
Hope this helps. Not trying to be a "know it all"; rather helping the conversation onto a more productive plane.
@Scottmoose Yeah I'm definitely making no modifications to the internal dimensions or angles. The only difference is some pieces being slightly longer/wider so they can slot in on the sides to help align and support everything.
@franklynb That's fair, I do want to be careful with language. It seems like I need to factor in three thing when choosing the width of the slots:
@franklynb That's fair, I do want to be careful with language. It seems like I need to factor in three thing when choosing the width of the slots:
- The actual desired final clearance, to have an appropriate amount of friction and precision in alignment but leave room for glue.
- The tolerance of the CNC machining process. Ideally the person doing the CAM work and who knows their machine can help account for this.
- Variation in the thickness of the boards being cut. Just have to measure the material once it's delivered and account for the maximum thickness.
Wow, I don’t get it. I use a tablesaw and a hand router. I don’t seem to have any tolerance issues. If a CNC can’t cut material to size then don’t use it. I thought they were super precise, enough for rocket parts and F1 cars.
Yeah it's because they can be so incredibly precise that you need to think about adding an appropriate amount of gap in places so that they aren't ridiculously tight when slotting together. But it's one of those things you don't normally have to think about so it's a little weird to come up with numbers out of nowhere.
That's the difference between doing your own woodworking versus farming it out to a CNC shop. When doing it on your own you can test the fit of various pieces together as you go and make any adjustments necessary. And if some boards have a slightly different thickness than others it's easy to compensate for it.
Charles G.
Can't tell from these posts if you have your own woodworking tools or not. But for what it will probably cost to farm it out you might be able to pay for some or all of the tools required.
A small portable table saw is all that you really need. And there are some in the $200 to $300 range than can probably do the job for you. Plus, another $65 for a stacked dado blade to cut the slots and you should be all set to go.
Can't tell from these posts if you have your own woodworking tools or not. But for what it will probably cost to farm it out you might be able to pay for some or all of the tools required.
A small portable table saw is all that you really need. And there are some in the $200 to $300 range than can probably do the job for you. Plus, another $65 for a stacked dado blade to cut the slots and you should be all set to go.
Last edited:
I have some limited tools, but for a variety of reasons my best bet for being successful making some large back horns is going to be getting a CNC shop to help. Everything from ability to handle full sheets of material myself, to the equipment to cut it out, and the ease of glue-up when using slotted CNC designs. Price-wise I'm still hopeful it'll be reasonable because I'm capable of doing the CAD work myself.
The questions come down to the practical & learned experience of having done it before which was why I was reaching out here. You could go down the rabbit hole of 'Do I need to account for X, Y, and Z?' or just trust someone that has done it before saying 'Give about 0.25mm extra clearance.' That sort of thing.
The questions come down to the practical & learned experience of having done it before which was why I was reaching out here. You could go down the rabbit hole of 'Do I need to account for X, Y, and Z?' or just trust someone that has done it before saying 'Give about 0.25mm extra clearance.' That sort of thing.
Sorry for the derailment, I’m just trying to learn.
If the tolerance is 0.10mm does that take into account what the tolerance is 1,500mm away? Is it the same or does it increase by the distance? Is it 0.10mm across the table?
If the tolerance is 0.10mm does that take into account what the tolerance is 1,500mm away? Is it the same or does it increase by the distance? Is it 0.10mm across the table?
Most lumber yards will cut up full sheets into pieces the size you can easily handle for a very reasonable cost. And you can cut your own slots using a stacked dado set
However, it's still a lot of time and labor and paying someone else to do it for you also makes sense.
A "lift" from a class on "Geometric Dimensioning and Tolerancing" as taught {by me} to metalworking designers a few decades back might help:
I can think of four typical ways to make a 2" round hole in wood {there are others}:
1) drill using a 'hole saw' which has its own 'centering drill bit';
2) cut, using a self centering 'forstner' bit;
3) cut, using a single point boring tool;
4) 'articulate' using a 1/4" bit and a CNC generated routine.
Each method has an associated manufacturability rating, typically called a "capability" w.r.t. the geometric concerns:
1) "ovality', or surface drift along some set of virtual axes
2) "size control"
3) "true position" of the virtual center
4) roundness, which is not the same as #1
The TOLERANCE is a composite statement of "what can be tolerated" in ALL of these concerns; typically specified in some
orthogonal fashion along some "possibly measurable" feature axis. "Possibly" because, for instance, one cannot measure the
"true position" of a center of a hole that is not absolutely round. It can only be estimated, to a degree of accuracy, by
sweeping/probing the perimeter at few/several points and doing the math.
The tolerance on that 'true position' takes that measurement's possible accuracy into account, among other issues that represent the manufacturing
METHOD of choice, and the accuracy of the measurement method {plug gage, dial indicator. micrometer split, tri-mike, etc,
etc, etc}.
Without a {specified, or known} method, the tolerance specified by the 'designer' is just wishful thinking, a.k.a. design fiction.
Some reasons why that is true, using the above set of possible hole-making choices:
- a hole saw will grow in absolute size during subsequent use. So 'true size of the hole' will grow over the span of the parts made,
unless some restorative cooling is applied {e.g. wait and pay}.
- a forstner bit 'walks' a bit due to the flexural strength of its shaft; they make them in different "beefier" constructions to try and
control this "movement from true position'. Likewise, the chucks used are not very accurate w.r.t. "roundness", unlike a ground collet.
- a single point tool is very accurate {and typically adjustable} for absolute size control; and makes a very round hole in uniform
material {due to its consistent chip load}. Its also very slow when compared to any other method, therefore costly.
- an "articulated" CNC hole requires attention to size control, but its adjustment is very fast {e.g. keyboard} and therefore
quick to produce with appropriate attention to gaging {in process measurement}.
Perhaps this helps explain why "what tolerance?" is a question with an infinite set of possible answers. Unless, and until a process
capability is specified.
I typically do a test joint, in the real material; and then decide what "clearance" is appropriate to my target compliance, joint stiffness and flow
of glue. Can't say how much clearance is appropriate unless its specific to a "use case". But a 'good rule of thumb' by _MOST?
carpenters is 1/64" {.015" } ... which is the vernier capability of most of their tools.
A metal machinist would use 'about .003" ' which is the difference between a 'press' and a 'slip' fit. A 'slip" fit in metal is .002" per inch of thickness,
more or less. A 'light press' is .001 "/". An 'interference' fit is tighter, including 'zero clearance'. A typical metalcutting vernier is .001".
MOST CNC machines FAR outperform the patience of their operators and programmers, which is often an order of magnitude higher than the
patience of the owner.
CNC's do NOT produce better parts because they are more accurate. They do so because they are faster and easier to ADJUST to a particular target.
Ask any owner of a Bridgeport type 1 or 2 mill.
In wood, I rarely need to account for thickness variation. Flatness?
However, clamping is almost always an issue, as parts CAN and DO drift during setup.
In wood, you have very few fancy clamping methods. On a milling machine, I have a whole pile of special clamps, as the cutting forces are
a magnitude of order higher, requiring way more attention to clamping stiffness and workholding power.
As much as I love to make many projects out of wood for its beauty, there are limitations with it concerning humidity such events as warping/swelling. Metal has a much more consistent set of 'givens' if I can put it that way. Once you the basic dimensions you can count on them stay constant as compared to wood (and depending on the species of wood).
We did a lot of CNCed Frugel-Horns and a few others. @chrisb has the details, i just packed them. Hopefully he can chime in. With well over a 100 pair of flat-paks and a “time-series+ of plywood used, he gained a huge anmount of experience.
Note: FHs still require a pass thru a table saw.
dave
Note: FHs still require a pass thru a table saw.
dave
Only thing I can really add to the conversation is that with the numerous designs other than just the FH flat pack kits we produced, there was always a concern over minor variations of material thickness with the different brands and batch lots of BB plywood we used, as well as slight warpage due to varying humidity in the shop and other reasons. To attempt to mitigate for that, I always had the CNC operator adjust the tool correction parameter to allow for about .5 mm over cutting at actual run time. In the case if the woodworking CNC machines we used, the majority of the work was performed with disposable insert cutting bits whose cutting diameter could vary by decimal fractions of a millimeter, which was really only a problem when compounded by slightly warped or thick material on internal dadoes.
In my own builds, I generally attempted to be generous enough with the Titebond II glue and clamping/ mechanical fasteners that loose joints were seldom an issue.
As for the passes through the table saw that Dave refers to on the FH series, that was due to my personal kink of using a scarf joint on the bottom edges of the vertical internal and slanted external panels, as well as the top, bottom and front baffle that required a 5dg cut on at least one end. A 5 axis machine would eliminate that step, but I was lucky enough to get access to the big CNC for most of the work, so engineered the production accordingly.
In my own builds, I generally attempted to be generous enough with the Titebond II glue and clamping/ mechanical fasteners that loose joints were seldom an issue.
As for the passes through the table saw that Dave refers to on the FH series, that was due to my personal kink of using a scarf joint on the bottom edges of the vertical internal and slanted external panels, as well as the top, bottom and front baffle that required a 5dg cut on at least one end. A 5 axis machine would eliminate that step, but I was lucky enough to get access to the big CNC for most of the work, so engineered the production accordingly.
Last edited:
Assuming 3/4" thick material, let's say the Birch Plywood, about how many feet of milling could you expect from one CNC bit? Even good router bits don't last as long as I might have thought, even though to some extent they can be touched up for more production. Admittedly this becomes even more of an issue with MDF and the like.