First project - Hexagonal staircase newel cap

Smorgasbord · July 15, 2021, 4:47pm

Carbide Create Pro (which you can get a trial version of) adds features for simple 3D modelling and toolpathing

I was surprised to find out that the Pro package wasn’t included in the price of new machine. Maybe time to learn Fusion360.

Or you could use a wedge/tapered jig to hold your base,

I had thought about that, but given the size of the base, I’ll likely run out of vertical room under the gantry trying to make the bevel horizontal unless I cut holes in the spoilboard,

One question I’ve had about VCarve inlays is that if don’t mill them right then you might have a gap between bottom of the top piece and the top of the bottom piece. You’d need a gap-filling glue, right?

But, since this inlay is a simple wedge, as long as the angles match I can simply slide the wedge into the opening and push it as far as it’ll go. I’ll be trimming the center opening later anyway, so I could make the wedge slightly longer than needed.

GJM · July 15, 2021, 5:58pm

Folks here have shown cursive script inlaid using the vcarve mechanism and it’s pretty flawless. @Julien has a great set of tutorials on it that you can look up (or he can graciously share the link to )

Julien · July 15, 2021, 6:57pm

From the drawing in your original post I see the part is about 1" thick, if my math is right the jig angle would about 11° bringing the flat part to b milled at around 2" height, a Shapeoko has about 3" of Z clearance, that should work ?

That’s the beauty of vcarving for me, you make the female part slightly deeper than it should be (to account for glue, and for some margin), you make the male part slightly taller than it needs to be, then glue in the male part, it will stick out and then you sand or mill down to the surface of the female part surface. This allows one to not be very precise in the depth/height of the female and male part, as long as the wall angle is the same (that of the vbit), it will fit perfectly.

(from the ebook)

True! So if the jig approach is not practical, I guess you’ll need to do some 3D modeling and toolpathing. Happy to help modeling this in fusion if you need.

GJM · July 15, 2021, 7:37pm

Thanks for sharing that pic Julien! I was looking for it and couldn’t find it. I think that explains it well.

Smorgasbord · July 15, 2021, 8:14pm

Julien, you’re right that the angle is low enough that the part should fit, even with me going to a 1.5" thick base now. But, getting the angle right is tricky since the angle isn’t one of the bevel angles on the triangle, it’s something in between the two.

I understand about the VCarve geometry; I guess the question comes down to how controllable the gap between the pieces if and whether your glue can span that gap with enough strength. Traditional woodworking glues don’t span well, but epoxies and cyno glues can.

I do think that since I’m making both pieces on the Shapeoko I’ll have enough accuracy, and like I said the simple wedge shape gives me an easy out on the fit. Are there any good getting started tutorials for Fusion? Otherwise, I’ll do the usual YouTube search…

Oh, and I still haven’t figured out the best way to make/attach the center piece, which is a hexagonal cap that to the completed base:

Originally, I was going to mill the center of the base with a hexagonal hole, clean out the corners, and insert the hexagonal cap like an extrusion. But, I think that leaves me open to gaps, even with CNC. It might be better to build the hexagonal cap such that it sits on top of the base, maybe screwed in from underneath the base or glued.

I could mill the hexagonal sides conventionally or with the Shapeoko. I would then need to mill the bottom with a recess so that cap only makes contact on the outside edges. Ideas for that? For the top, I could mill that conventionally, because on the CNC it would involve ramping accurately and would definitely need some sanding clean-up anyway.

Thoughts on the center cap milling would be appreciated, as always.
TIA

Julien · July 15, 2021, 8:40pm

I learned the CAD part from this guy, it was an excellent start to make sense of the UI, and then once we master the basics/design principles, the rest is easy to learn as you go. The CAD part I learned by doing and with the help of folks here on the forum.

I have never been a woodworker so I tend to think in terms of “I have a CNC, it’s the answer, whatever the question is” (which is a bad approach obviously, but I just love CNCing stuff). So I would do that as a two-sided job

start from a square stock
mill the top
mill a jig that is a negative of the top
flip the part and attach it onto that jig
mill the underside/recess.

CrookedWoodTex · July 16, 2021, 12:08am

Ben, the VCarve method described uses the fixed angle of the Vbit.

Smorgasbord · July 16, 2021, 12:20am

the VCarve method described uses the fixed angle of the Vbit.

That’s not the angle to which I’m referring. It’s the angle at which the base needs to held to have both sides of the inlay opening parallel to the CNC bed. Each side runs along a different bevel cut into the top of the hexagonal base.

Smorgasbord · August 2, 2021, 7:40pm

OK, I’m still working with Carbide3D support on getting my new Shapeoko Pro Std up and running (they’ve been great, but it’s kind of drag having multiple issues), and in the meantime I’m modeling in Fusion360.

To recap, here’s the part I hand built:

And as of last night, here’s the model in Fusion360:

I decided that since my staircase posts aren’t perfect hexagons, that I was first going to mill the thing traditionally in the lighter wood and then use the Shapeoko to both make the darker wedges as inlays and to cut out the inlay recesses. This way any gaps in the traditionally made base will be completely covered by the CNC made inlays.

What’s the best way to about this? I can probably make another component or body (not sure of my Fusion360 terminology) that represents the wedge, but then how to I design the cut-out inlay? And I don’t want to cut all 6 recesses at once, my plan is to rotate the “base” for each recess cut since the sides won’t be identical. I’ll reference off the point of the base, which is also the point of the wedge inlay. I just need to design for one inlay recess, since I’ll run that job over and over for each of the 6 inlays.

The dark wedges aren’t just flat veneer inlays. If you look closely at the photo and the Fusion360 model, there’s a peak running down the middle of the wedge. My plan here is to cut the wedges thicker than I need and then sand them down using a disc sander. I’d love to cut the whole shape using the Shapeoko, but given the non-regular hexagonal base that doesn’t seem practical.

To summarize my questions:

How do I model/design the recess (after I construct the wedge body)?
How do I use Fusion360 (or Carbide Create) to construct the tool paths to only cut the inlay, since the base will already be cut?
Is there anything special I need to do when modeling the recess given that the wedge will be designed to stand proud? I’m assuming not since the recess will have flat bottom as will the wedge.

Any other suggestions?
TIA!

Julien · August 2, 2021, 8:35pm

You don’t necessarily need to. Once you model the wedge, you could use the outside contour of that wedge as (one side of) a selection for a toolpath milling the recess.
If you do want to model the recess, you could use the Combine function to do boolean subtraction, using the modeled wedge as the part to be subtracted from the base

It’s all a matter of selecting the appropriate contours in the toolpaths. If manual selection is too tricky, a good way is to use projection onto a sketch of the contours you want to use for the toolpath, and then use that projection as the selection in the toolpath

Potentially, a little tolerancing/margin between the recess and wedge? but given the wedge shape, it’s probably not necessary anyway.

Smorgasbord · August 2, 2021, 9:02pm

Thanks. On modeling the wedge, I need to somehow build that off of the hex base body I’ve just made. The wedge is really a trapazoid connecting these 4 points, as indicated below:

I’m not clear on how to create this recess, and since it’s going into two surfaces that are angled with respect to each other, as well as angled from the “top view,” I’m kind of at a loss. I think I have to create some planes to intersect with the base body, but I don’t know how to go about orienting them properly. I guess what I do know is that the wedge definition will have two planes that are each perpendicular to the base plane (top view), and that each of the planes will go through 2 of the 4 corners in red.

I’m still learning Fusion360 - I should have recorded my screen for the few hours I spent building that hex base, I’m sure it would have been a facepalm sequence for many here.

Julien · August 2, 2021, 9:56pm

It’s midnight here so I’ll call it a day, but the Fusion360 crowd here should be able to help.
I would look into projecting that trapeze onto the base plane, then use the loft tool selecting the projection at one end and the trapeze at the other end, and see where that gets you

Smorgasbord · August 14, 2021, 5:30am

OK, I think I crossed the Fusion 360 threshold. Here are some screen grabs:

The finished piece (only 1 of 6 wedges shown):

FullRender1920×1079 35 KB
The Wedge itself:

Wedge Component1108×918 52.4 KB
The Base milled for the wedge:

Base Component1920×1073 34.2 KB
And the center hexagon:

Center Component770×638 27 KB

Here’s my Fusion 360 file:
LargeNewell v3.f3d.zip (257.6 KB)

Since my plan is to make the Base using conventional methods, what I need from CNC is:

Toolpath to cut out for the wedge. I’ll run this six times, rotating the base for each.
Toolpath to cut out for the center hexagon.
Cutting the wedge. The top faces should be left with some excess so I can sand them down flush.
Cutting the hexagonal center piece. This isn’t too tall, so I think it can be done with the piece vertically if I can figure out workpiece holding.

#1 and #2 will probably need to be cut using a combination of ¼" and ⅛" end mills. Since I’m still on the free version of fusion, I think that means creating two separate .nc files, one for each tool, but then this means I can’t use the BitSetter to align heights, right? Or, is there some other way?

I did figure out how to import Carbide3D’s tool library, but I’m not sure it’s updating the correct feed speeds and such (it doesn’t update spindle RPM, for instance). These piece are all hard wood (softer than maple but harder than cherry), so input on tool configuration would be appreciated.

Also, help on how to proceed on the toolpaths would be appreciated. Do I do a 3D adaptive contour for the inlay cutout followed by a 3D contour finishing pass? Something else? How much material to leave after the first pass?

Just realized that I did not do the “wedge” thing for the inlays, which requires using the “V” bits, right? At this point, I think I want to just mill the pieces straight up and see what kinds of gaps I get. With contrasting woods a few thousands of a gap would be tolerable - and probably inevitable given wood movement after several years anyway.

Thanks again for all the help. I’m excited to see the components come alive in Fusion.

Julien · August 14, 2021, 9:51am

If your version of Fusion won’t generate a multi-tool file with M6 tool change commands, yes you’ll need to generated one nc file for each. Carbide Motion can’t utilize the BitSetter in that situation, so you could either:

re-zero manually between jobs. Of course there is the matter of not milling away the zeroing point with the first tool. On the case of that hexagonal base, and since I understood you are going to be using some kind of jig/pegs to align the base (and later rotate it), it would make sense to a) model the jig in Fusion too, and b) set the zero reference somewhere on that jig, so that it’s still accessible after any job
if you really, really wanted to use the BitSetter, you could consider using another G-code sender (CNCjs) and the associated BitSetter macros, in that setup you can run individual BitSetter probing between runs. But having to learn how to use a different G-code sender just for this may be overkill here.

What specific 1/4" and 1/8" tools are you going to use ? Feeds and speeds will depend on their number of flutes. A good starting point would be the feeds and speeds recipes in CC for hardwood, and there’s always Winston’s MaterialMonday video for wood.

So the first thing I realized upon opening you model is that the center hexagon hole is going to be difficult to CNC:

it requires to cut through 36mm of wood, which mean that ideally you would want an endmill with a length of cut of at least that (to avoid rubbing the shaft against the walls when cutting the final passes), and most of the common 1/4" and 1/8" endmills don’t have a 36mm length of cut. You could still go ahead and do it with a smaller LOC endmill anyway, it’s a little awkward but sometimes one can pull it off. You will still need to have ~40mm of endmill sticking out of the collet

image956×593 65 KB
but the bigger problem is to inside corners of the hexagon. A 1/4" endmill is going to leave large rounded corners, a 1/8" endmill could make smaller corner radius but it’s going to be hard to find a 1/8" endmill with such a long reach and LOC. And that would still leave you with less-than-pointy inside corners. Maybe having the center hexagon “cap” the top of the base could allow it to have a circular lower part and a hexagonal top (but then it becomes a 2-sided milling job).

For the wedge pocket, I have not played with it for long but I wonder if you could use a “Parallel” toolpath, selecting the bottom of that pocket as the boundary, first with a 1/4" tool (tool containment = “tool inside boundary”, with some radial stock to leave:

Then a second parallel toolpath with a 1/8" and Rest Machining (“from previous operation”), still with with some radial stock to leave:

and finally a “Pencil” toolpath with no stock to leave to finish up the sides with the 1/8" endmill

Just rough ideas.

I agree that it’s worth trying a “straight” fit first, which you should be able to pull off even if it means creeping up on the correct dimension of the wedge (which is trivial in Fusion: make the part initially oversize, cut, measure/fit, adjust “stock to leave” to a small negative value, recut, re-test, rinse and repeat until you get a perfect fit). Doing the V-bit thing in 3D brings some complications (however it may still be interesting, for a more error-tolerant perfect fit of all wedges.

LiamN · August 14, 2021, 3:58pm

Well that just saved me £120

On the machining front, I also took a look (as how best to machine this on a 2.5 axis machine is an interesting question).

If I was making this, and willing to mess about with 6 setups to machine each wedge pocket separately, I would probably use my table saw to create two large angle wedges to let me mount the main hexagon at an angle such that a wedge pocket was flat.

I don’t have that sort of patience though so I thought I’d try out how to machine the main hex in one setup to avoid re-zero-ing and all the risks of messing up that come with that.

First thing was to create a stock body to use adaptive clearing against

That allows me to make one setup for the whole main hex thing which assumes the central hole and wedge slots are occupied with stock and need to be cut.

A 3D adaptive clear is frequently the easy way to start

0.5mm stock to leave axial and radial

Then a 2D contour to face the central hexagon, I would just come back with a sharp chisel and square out the corners on this. I would also consider only making this hexagonal for the top 1/2" or so and then making it circular or with rounded corners, depends on how I was planning to make the central hexagon.

You could come back with the 1/8" bit and do the top 20mm or so to get squarer corners near the top to make the hand finishing with a chisel easier.

I’d then run a 1/8" ballnose to get a reasonable ‘flat’ on each of the wedge slots, 3 separate jobs here at 0, +60 and -60 degrees pass direction, 0.25mm stock to leave radial to avoid dinging the walls.

Finally I’d come back with a pencil toolpath to clean up the edges, note that even the 1/8" is too fat for the ends of the slots so those are likely manual with a chisel too. I might leave the outer edges with extra stock to control breakout whilst machining and do a final finish with a plane or table saw.

Sneaky tricks inluded sketches on the wedge inlay faces to provide toolpath boundaries and guides for the pencil toolpath

As well as making a surface through those and a patch across the top to provide a surface to ‘touch’ for the parallel toolpath with the ballnose.

For the wedge inlay I would run a contour (or just use a table saw to cut the wedges to fit) around the edges and then an adaptive clear on the top with at least 0.5mm stock to leave, glue them in and then use a plane / sander to flatten them flush with the hexagon.

HTH

LargeNewell v3 v5.f3d.zip (1.2 MB)

So, that’s basically the same sequence of ops as Julien, but with the 6 aspects all being cut in the same job to avoid doing 6 setups and zeroing.

Smorgasbord · August 14, 2021, 5:55pm

WOW, Julien and Liam - I’m still digesting, but I am most appreciative.

My first note is that because these sit on top of hexagonal posts that themselves aren’t perfect (off by more than 1/16"), my thought was to not mill the whole thing in one setup. My idea was to build the base without wedges, trimming the sides manually as needed to fit the posts and then beveling on the tablesaw. I’d then screw two pieces to the spoilboard to “capture” one of the points, which act as registration for the wedge inlay cuts. The “zero” point would be fixed relative to the registration pieces and so would not change for each inlay cut once set up.

The base shouldn’t be from one piece of wood since then the grain wouldn’t run the way it needs to (which is parallel to the outside edges for both appearance and wood movement purposes). A 10" wide board will expand and contract a lot with humidity changes. I really do think I need to glue six pieces to construct the base. My cuts don’t have to be perfect since the wedge inlays cover all those base joints.

I discarded the “angle the base so the inlay is horizontal” idea because of the imperfect nature of the base would literally required shimming each cut to get it perfectly horizontal, and then also require re-zeroing for each.

The points you both made about the center hexagon are spot on - sorry I didn’t disclaim that aspect, which I didn’t do because that’s not my focus. I was planning on something similar to Liam’s idea of cutting just a tad deeper than the center piece is visible for, and glueing it in. I could use a screw from the bottom of dowel it, but it’s not load bearing and there’s lots of surface area so glue should be fine. Slightly rounding the center piece so it fits the 1/16" radius corners from the ⅛" bit is probably the right way to go from both fit and feel to the hand as you climb the stairs perspectives.

Smorgasbord · August 14, 2021, 6:09pm

Some other thoughts:

I’d want to cut the center hexagon cut-out after the wedges are glued in place, rather than try to make those perfect from the get-go. This way I can cut the wedges longer and simply slide them into place as far as they need to go, knowing that my subsequent milling operation will trim off any excess.
I’m really worried about re-zeroing with all the bit changes. Autodesk offers a 30 day free trial, so I’m thinking of doing that for this project. I could then decide whether I want to buy a year subscription, or maybe even just do a month whenever I really need it.
Yes, as Liam noted, the tight end of the wedge is smaller than ⅛" so I’d have to use a chisel or small dovetail saw to finish the cut-out.
I had thought about leaving more base material, cutting and inserting the wedges, then trimming to fit the posts, but since the wedges taper to that narrow < ⅛" dimension, one’s eye would see any deviation. This is why I think I need to cut the wedge inlays after getting the base to overall dimension, and indexing from the “point”, since that’s the critical dimension.
Which makes me realize there’s another critical dimension here where the wedges meet the center hexagon. So I think need to mill the center cut-out before trimming the base to fit the imperfect posts, and then cut the wedge inlay, and then trim the fat inside part of the wedges to match the center cut-out.

And now the most important part. Thanks for sending your modified Fusion 360 files back to me. I’ve been struggling with toolpaths in Fusion and don’t understand many of the parameters or what to do. Hopefully I can make sense of what you’ve sent back.

I have the Carbide3D starter set of bits:
#201: ¼" end mill for stock removal
#102: ⅛" end mill (½" LOC) for corners
#202 & #101 ballnose mills (¼" & ⅛")
#251 ¼" spiral downcut (which I don’t think I need for this job)
#301 & #302 V-cutters (also not needed)

I also have a collection of router bits from my normal woodworking activities.

Thanks again!

LiamN · August 14, 2021, 7:12pm

Ask away on the CAM questions.

WRT Fusion, there is the free hobbyist license which I use, if you’re not using it professionally.

As for re-zero-ing between bit changes I leave the workpiece in place so the X and Y don’t change and always zero the Z off the spoilboard so it’s easy to re-zero after a bit change.

As for cut order and doing the inner hexagon afterwards, that’s all just down to the order you do the toolpaths, the payback for the CAM being a bit dumb and needing lots of guidance is you can make it do almost anything you like.

Smorgasbord · August 14, 2021, 11:23pm

OK, I’ll open your file and see if I can isolate the toolpaths for a single wedge and for the center hole.

LiamN · August 15, 2021, 12:29am

One thing I’d suggest is, given that you want to machine thing which is not regularly shaped, to think carefully about where you can set the X, Y, Z zero for each setup and have them align reasonably at the center etc. There’s a decent risk of things being visibly not well aligned when you get to the hexagonal center otherwise. Setting zero reliably across a multi-setup job is one of the hardest things to learn.

One option might be to put a center hole through the newell to allow you to locate on a pin in the spoilboard as X, Y zero and then just rotate newell to set the angle to match that side. Or that might not work at all, I’m not quite sure which parts of your process will be irregular.

Anyway, if you get stuck on the toolpaths, here’s a crib sheet

LargeNewell v3 v6.f3d.zip (1.3 MB)