think carefully about where you can set the X, Y, Z zero for each setup and have them align reasonably at the center
That’s a really good point. I had planned on using the outside “point” of the wedge (where 2 sides of the base hexagon meet) as the zero point for cutting the wedge inlay, but you’re right that this could create problems at the center.
It would be simpler if I could just mill the whole thing accurately on the Shapeoko and at least it would all be aligned. Maybe I should build the topper a bit larger than the post, and have a ⅛" gap between it and the post. I could then have the overhang be the same all around, just that the centers wouldn’t align, which one couldn’t tell anyway.
In terms of my irregular post, each side is supposed to be 5" across (hexagon inscribed in a 5" radius circle), but in actuality some sides are 1/32" or more shorter while some are the same amount longer, and some are pretty close. Just looking at the post, it seems fine and if I did a simpler topper design it wouldn’t matter, but I’m kind of proud of this and want to see it through.
Thanks again for all the tips and techniques, and advice! This is a great community!
Liam, I’m going to try to build the thing via your idea of doing it all on the Shapeoko. I’m taking your v5 file, but I need to change the center hole so it doesn’t go all the way through. Not sure how to do this without messing things up.
I can push/pull the bottom of “Center Hexagon:1” up as high as I want (a delta of -32mm seems about right to me). That’s the easy part.
But the “HexWithInlayCut:1” component still has the hole going all the way through. How do I fix that?
What I’m doing for the try-out is gluing two pieces of MDF together to get the 38mm thickness. Then I’ll cut out the triangles and glue them up just as if they’re real wood (yeah, I know I could just start with a single piece of MDF that big, but I want to mimick as many of the actual steps as possible on this trial run before committing it in the exotic woods).
Once I have the hexgonal base glued, I’ll want to mill the center hexagonal pocket and 6 wedge inlay pockets. This is what I’m most concerned about doing on the Shapeoko.
Then I can explore cutting the wedges and center hexagon on the Shapeoko. On interesting thing is that if I cut the center hexagon on the Shapeoko, I can design it with 1/16" radius rounded corners to match the pocket. Liam, are there toolpaths in the file you sent that will do that, or do I have to somehow derive those?
I’m going to owe you more than a beer when this is done!
Yes, that would be a smart way to go about testing out your toolpaths, I generally brutally murder some old plywood or MDF testing toolpaths before letting the real wood go for surgery
There’s a bunch of stuff to learn to get right here from zeroing to ensuring the machine is fully square, that your belt tensions are even and your X, Y are calibrated close enough to each other etc.
Be aware, the speeds and feeds selected on these toolpaths are about what I run on my machine, subject to my ears telling me to reduce feedrate or change the DoC or similar in the CAM and re-run, don’t just expect they’ll all be good for your stock on your machine
OK, this is quite easy, once you think in the boolean and sketch verbs that Fusion gives you. There’s lots of ways, here is one.
Hint - Use the timeline at the bottom of fusion to replay the actions somebody took to build or modify the Fusion file, it lets you see their steps and figure out the order in which they did things. If you select a component the timeline only shows actions for that component, if you select the root “LargeNewell v3 …” then you see the timeline for everything.
Make a sketch on the base of your main hexagon and project (P) the outline of the hexagon into the sketch.
So now we have a main hexagon with no hole in the bottom. Next I used the combine feature to cut the bottom off the Center Hexagon using the newly filled in part of the HexWithInlayCut
It occurred to me it might be useful for zero-ing and also for attaching to the post to have a bolt / screw hole right in the center, so I extruded those too, just delete those two extrudes from the history to remove them.
Now onto the tricky bit, the insert wedge, this has an undercut where it meets the central hexagon and also needs to be a really clean fit into the wedge slot machined in the hexagon and then has to be flush with the surface.
My suggestion (awaiting better ideas from the more experienced woodworkers here) is to cut this over length and over height so that you can push it into the slot until it ‘bottoms out’ on the walls and rear face then trim the ends and finally face the surface down (with a plane or sander).
I created a new component to give us this larger body to glue and trim in place. In this new component I created a sketch on the bottom face of your existing wedge, projected the outline of the wedge and then extended the sides forward and backward to give some extra to cut off later.
Then I made another new component for the stock, no idea how you plan to prep the stock so I just made a wedge that was a bit bigger (user params again). Same trick, sketch on the base of the Wedge Inlay Machined Blank, project, add extra, extrude thicker.
Then a new machining setup for the wedge using the stock body for stock, note the choice of zero location, may or may not be what you want depending on how you prep the stock.
I’ve assumed blue tape and superglue workholding here as clamping this stock would be a pain and need tabs and other complexities, that’s all up to your preferences…
First is a 3D adaptive toolpath with the 201 1/4" cutter, then a contour around the edges, this is where you find out if your Shapeoko is square and whether your X, Y calibration is good.
Finally an optional 1/8" ballnose to trim the top surface down, not sure this is really useful as you’re going to plane / sand this down to flush with the main hex once glued into place.
Beware, you will need to get the workpiece zero exactly the same for this, you might be better off not cutting the center hex at all in the first machining and only cutting it once in this step. Try it out and see.
Yep, using the same 2D contour toolpaths in the main hex with smaller radius bits will get you a smaller corner radius.
As for the central hex, try it out, make a stock component of the blank you want to machine from and then try a setup using your stock component to do stock “from body” and then the adaptive clear, followed by an outer contour and probably parallel over the top with a ballnose?
Wow again - will take a look later today after I get the parts in glue-up. Some overnight thoughts:
I was also thinking about hold-down options. My post is hollow, so a center hole won’t help there, but now that the center hex cut-out is a shallow pocket, I could easily drill a center hole manually and screw that into a T-nut in the track of my hybrid table. I could also “add” the tape/superglue around the edges for additional security. For cutting the wedges themselves, definitely need the tape/glue. For the center hex, since it’ll be standing up, I’ll probably screw a piece of plywood to the bottom and then clamp the plywood to the hybrid table.
I’m thinking the new center point should be the bottom center of the main hex body. I would do this in two stages: first I’d set the Z-axis to zero at the spoilboard, or maybe a piece of paper higher. Then I’d mount the blank and zero X-Y at a pre-marked center at the top. I don’t want to zero at the top since I don’t want to have the stock thickness be a critical dimension for me to achieve.
Routing away all that material for the main bevel seems like a waste of time, router bit wear, and dust bag. I should probably cut a rough bevel using the tablesaw - just keep it say 1/8"-3/16" away from the final surface. This means modeling the original stock to have that bevel. I’d probably model the stock to be slightly larger than I expect to manually cut the bevel and live with the tool spinning in space for a couple rounds.
You wrote: My suggestion (awaiting better ideas from the more experienced woodworkers here) is to cut this over length and over height so that you can push it into the slot until it ‘bottoms out’ on the walls and rear face then trim the ends and finally face the surface down (with a plane or sander).
Yes, this is exactly my intention, although since an extended “rear face” is in the hexagonal pocket, my thinking was that I’d do all the milling, then, leaving the base attached to the spoilboard, glue in every other wedge, letting the rear ends stick into the hex pocket (if I did adjacent wedges they’d interfere with each other in the pocket), and then, when dry, re-cutting the hex pocket. Then do the remaining wedges, and re-cut the pocket once more. There might be some hand trimming of the wedges in the corners due to the 1/16" radius from the ⅛" end mill.
I started another thread in the Shapeoko Pro category (Squaring and Calibration of Shapeoko Pro - #8 by greg5 ) for my machine setup adventures. I need to re-run the procedure again for the $100/$101 factors, but I think the squareness I’ve got is pretty decent (when gantry is slid forward there’s a 0.006" gap agains the end plate on one side, which is across 20" or more). I might try to re-square, but the only way I’d get better is to loosen not just all the bolts (and with the hybrid table there are a lot, but also loosen the belts (which I didn’t do last time).
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 .
OK, watched that. Winston’s great at many things, but apparently spreadsheets aren’t his strongest suit. Here’s my version of his data: Feeds And Speeds For CNC.xlsx.zip (7.6 KB) which I find a more logical lay-out.
One question I have is why both the ⅛" and ¼" cutters are run at the same rpm? Traditionally, woodworkers slow down the rpm for larger cutters. I know the desired result of how much wood each mill cutting edge takes per revolution is affected by rpm, DOC, and feed rate, but since we’re setting all those, why not choose optimum rpms for the bit cutting diameter and number of flutes and then calculate DOC/feed rates?
This has been debated here a few times, and basically the conclusion always is that while surface speed matters for metalheads (and even then, mostly for those who cut something more challenging than aluminium), for wood and given the endmills typically used on a Shapeoko (nothing larger than 1/4" in 99.9% of the cases), surface speed does not really matter. Or we could say that wood is tolerant to a very wide range of surface speeds (as long as the chipload is in check)
So for RPM as far as I am concerned it boils down to “set the RPM to the highest value you can bear”. @gmack once taught me that maximizing RPM minimizes cutting forces, so maxed out RPM should be the target. But I also used to have a trim router on my machine, and could not bear the screaming sound of a Makita at 30.000RPM for very long.
DOC is a different beast, and there was not much beyond experimentation to determine what’s a good value on a Shapeoko. Folks who know their deflection math concluded that shallow DOC and fast feedrates work better on a Shapeoko than deep DOC and slower feedrates. I like to use the “50% of the cutter diameter” rule on my Shapeoko. I hear the lucky SO Pro owners get to go deeper than that.
If you can’t sleep at night, here’s a thread where we discussed the matter of how to determine feeds and speeds on a Shapeoko (spoiler alert: there is of course no definitive answer, but that thread is basically where the stuff in the ebook’s feeds and speeds chapter comes from)
That all sounds sensible, I’ve never said “dang, I wish my workpiece was moving around more whilst I cut it”
It’s worth thinking about what happens after you machine that zero point away at the top (unless you adjust the toolpaths to leave the central portion of the hex untouched. Otherwise when you turn the machine on after leaving all the glue to dry you may not have workpiece zero any more.
Setting Z off the spoilboard is the sanity preserving option in my experience.
Sounds sensible, as you get better at CAM you’ll do more work to avoid ‘air cutting’ above the workpiece but that’s optimisation for later.
Again, sound sensible.
I might set the radial stock to leave to 1mm on the first big adaptive clear and then not run the 2D contour finishing passes on the inner hex at all until this stage to make sure if there’s any work zero offset there’s spare stock.
Sounds like you have the machine pretty square, time to cut things and see how it works. It’s never the problems you plan for that get you
Ugh. Power went out for over 36 hours, so I didn’t get much done. But, since this is obviously an odyssey, I decided to document my steps.
Cut 6 identical equilateral triangles to make the hexagonal base:
I have a largish tablesaw sled that I built a while back, with pivoting fence that attaches at the far end. This lets me make small adjustments at the far end to fine-tune the angle.
I had cut the triangles out of a single length of MDF (glued together to get the thickness I needed), but now I needed to cut them accurately to size. I used the remaining piece, turned around and clamped as the stop. I put each triangle into place and trimmed to size:
This was good in that I could adjust the tension on any of the 3 clamps to force the pieces into alignment.
The next day I decided to surface the bottom since I hadn’t aligned the pieces that way all that well. Well, somehow I screwed up either in Carbide Create or in setting zero:
You can also see my angular errors here. Glue fills that with strength, and there will be a bottom plate glued on anyway. And, my design has those wedges and center hexagon covering all those glue lines anyway. BTW, the tiny center hole there was done on purpose with a hit of sandpaper on those corners before assembly.
Since we had so much discussion on my existing posts being imperfect, here’s a piece of hardboard that I double stick taped to the top of one of the posts and then flush trimmed with a hand held router and measured. It’s on top of the MDF assembly.
You can see the MDF is larger than the post. I did measure and label each post’s side’s dimension (by eye). I’m going to leave the topper this much larger than the post and will have a ⅛" bottom plate that’s recessed ⅜" or so to create a ⅛" shadow gap between post and newel topper. This will help hide the differences (you’ll feel an overhang with your fingers all the way around), and besides my intent is that the newel topper is so pretty that’s what you look at.
I did get the assembly flattened, so the next step is to cut the big bevel. I’m going to do that on the tablesaw and hopefully will be able to leave just enough that after the wedges are glued in I can sand things smooth and to final size. Note that I’ll be doing 6 bevel cuts and if they don’t line up properly, you’ll see it in that the crease won’t go down the middle of the wedge (which aligns with the current triangle gaps). Make sense?
I am rethinking this approach, and wondering if I should just use the tablesaw bevel cut as a stock sizing/roughing technique and actually surface the bevel with a rounded bit in the Shapeoko before cutting the wedges. Thoughts?
I’ve now come full circle, and not just talking circle-inscribed hexagons.
Since I’m going down this path of leveraging the accuracy/repeatability of CNC, and no longer trying to make something that matches my irregular posts, here’s my yet-again-new plan:
Cut and glue up the main hexagonal pyramid larger than I need it to be.
Cut the wedges and center hexagon on the Shapeoko while that’s drying
Tablesaw rough cut the main hexagon pyramid leaving about 1/16" to 1/8" extra all around (in diameter and in cutting the main bevels).
Tape/Glue the pyramid to a rectangular piece of 19mm MDF. This will prevent future wedge pocket cuts from going into the spoilboard AND provide me with a persistent zero point. Easy to clamp onto the splilboard, too.
Rough-cut (Leaving under 1mm of material) the main bevels and outside edges of the pyramid with the Shapeoko.
Cut the wedge pockets and center hexagon pocket.
Glue in every other wedge, let dry (may use cyanoacrylate glue here to speed things up)
Re-cut the center hexagon pocket.
Glue in the remaining wedges, let dry.
Re-cut the center hexagon pocket
Final cut the outside edges and main bevels. This trims the wedges and the less than 1mm of material left by Step 4. Doing this together ensures they are flush. This “final cut” needs to leave something for me to sand smooth, don’t know if that’s 0.5mm or what yet.
Remove pyramid from rectangular base. Sand it.
Sand center hexagon, test fit, then glue in.
Cut a ⅛" thick piece of hardboard that’s about ⅜" smaller than the bottom of the pyramid on all edges. This will provide the shadow gap.
Screw and glue some blocks to the bottom of that for inserting into the hollow posts.
Screw and glue the hardboard to the bottom of the pyramid.
Take pictures, post a brag-and gag here, then do the other one, then do two others that are somewhat smaller, and then do two more than are even smaller.
Have a beer, then start an easier project, like making elephant head rattles.
@LiamN, I started to modify the file:
A) First I wanted to enlarge the main hexagon from 127mm to 128.2mm. This will provide me with the desired overhang to disguise the imperfect post match. I think I got that right.
B) Then I went to add the rectangular MDF base/reference. I created that as a new component (Side Note: it took me 2 hours in Fusion to figure out how to get the alignment of the rectangular base to the hexagon right. I finally figured out to first align a corner of the rect to a point on the hexagon, then align a side face of the rectangle to the side face of the hexagon, then move the rectangle 25mm away from the hexagon point so my BitZero fits.)
C) But now I need to move everything vertically 19mm so the bottom of the MDF is at z-axis zero. EDIT: Or, do I? Since I set origin in the Manufacture tab, the design origin shouldn’t matter anymore, right?
D) I’m not sure how to best setup origin/zero for the center hexagon. I can screw a board to the bottom, clamp the board, and then mill tops and sides, but it might get tricky to precisely find the center of my stock, which will be rectangular. So I might want to do repeat the zero point thing again that I’m doing for the main pyramid. Thoughts?
Nice tablesaw jig, I might have to make one of those myself.
Like many woodworkers, I’ve made my share of jigs. This one is made from Incra T-tracks. I’m not happy with how the pivot ended up working - I should have gone with a standard miter gauge and just ignored the markings on it. But having the wide support locking and ability to leave a 90 degree locking piece in place has been great. I also have a separate off-shoot support sled on the right there.
Right, I may have more questions than answers for you at this stage…
I think many of us recognise that feeling
Great, figuring out where your persistent zero is really helps think through the rest of your machining. You’ve spotted that I had several versions of X, Y, Z zero in the CAM.
Question here, do you plan to have a flat hexagon and use the Shapeoko to rough out the pyramid shape of the overall element? If so we need some toolpaths for the main faces and we need to tell Fusion that the stock is flat and not pyramid shaped or it will get a bit optimistic about cutting depth at the edges.
Yep, makes sense to re-run that contour each time, so long as you don’t move or lose zero. As you’ve got a persistent place to put your bitzero, so long as you can get the board straight with X and Y you can even remove it from the machine, put it back and re-zero.
Yep, as for how much, try it and see, if you use a ballnose then 0.5mm or less is likely OK.
So, an adapter plate then?
Of course in a few weeks you’ll want to machine a pyramid ‘soft jaw’ to flip the newel top into and directly machine the post adapter in the bottom of the pyramid
Sit and look at what you made, criticise all the things you think were mistakes or you could have done better, try to resist the urge to make it again…
Yep, looks like it, that’s in the main sketch “127mm hex” ?
Ah, I’m not sure this is how you want to do that…
If I have worked it out correctly you made a new component “RectangularIndexableBase” - good, you sketched and dimensioned the base and then extruded it. Then I think you manually aligned that base with the hexagon and moved the component into place.
There’s a couple of problems with this, the first is that there’s nothing holding that component in it’s new position and the second is that there’s no cleanly defined relationship between the hex edges or center and the rectangular base. The warning is the two different origins which you can drag around by dragging the components.
There’s several ways to do this a bit more cleanly, one option is that in the sketch for the base of the rectangular base you could turn on visibility of the main hex, and then project the sketch “127mm Hex” into this sketch to give you the outer permiter of whatever your current hex is. This means it’s connected and will update if you change the dimensions in the main hex.
Once projected we can start to tell Fusion about how we want the relationships to work.
What I’ve done here is kept your square plate dimensions but I have told Fusion that the top edge is coincident with the top edge (Constraints - Coincident). That lines up the edge as I think you intended. Then I put a 25mm dimension from the corner of the main hex to the edge of the rectangle, again I think that’s how you lined them up. Finally I drew in the 60x60 Bitzero so we can visually check whether we have left space for it.
I told Fusion to reset the manual positioning to let dimensions define things instead.
What I would do now is “ground” the main hex and then add an “as built joint” between it and the rectangular base to make sure they stay aligned as drawn (separate components can be moved relative to each other as you’ve found out)
I would suggest using the top of your MDF board as Z zero. You can just select the bottom corner of the MDF as zero point instead though if you prefer.
Ah, saw your edit - correct, Z plane and zero are configured in each CAM setup so you can represent which way you’re putting the workpiece on the machine, not how you drew it.
So, we’re talking about machining the center hexagon out of a chunk of rectangular stock?
If the stock is slightly oversized then we’re not too worried about exact center, just ensuring that the final solid is within the stock. This also means it doesn’t need to be exactly square either.
I suggest drawing the stock as a component and then creating a CAM setup using that stock, then we can see what might work?
One key thing to spot here is that the Z plane is set to be ‘flat’ with the bottom of the wedge insert for machining, not sure if that was clear or not. Obviously you can put the zero point wherever you think it’s convenient for setting up the workpieces for cutting. As you’re making several you might want to make a jig to hold the raw stock, maybe mill an indent into a piece of MDF?
Ah, my fault, sorry, if you edit that toolpath and say no to clearing the selections you’ll see I’d selected the bottom of the central hex cut out before filling that in.
Question here, do you plan to have a flat hexagon and use the Shapeoko to rough out the pyramid shape of the overall element?
I keep going back and forth. My natural instinct is to rough cut the pyramid on the tablesaw, leaving like 1/8" to 3/16" of stock to be removed by the Shapeoko, as that saves time and wear on the workhorse ¼" bit (but I’ve got 3 of them now). But, maybe I should embrace the CNC way and do the whole thing on the Shapeoko. So, let’s do that for now.
If I have worked it out correctly you made a new component “RectangularIndexableBase” - good, you sketched and dimensioned the base and then extruded it. Then I think you manually aligned that base with the hexagon and moved the component into place.
Yup.
There’s a couple of problems with this, the first is that there’s nothing holding that component in it’s new position and the second is that there’s no cleanly defined relationship between the hex edges or center and the rectangular base. The warning is the two different origins which you can drag around by dragging the components.
That’s exactly right - it needs to be parametrically aligned/set. I still struggle with getting Fusion to do even basic things for me as its way of working is completely different than what I’m used to (such as Adobe Creative Suite, especially Illustrator & Photoshop). I keep hitting the space bar to get the hand tool, for instance. I clearly need to learn how to tell Fusion about relationships and such. For instance, even the spacer cube thing I created for the wedge sides is just out there. When I resized the pyramid from 127 to 128.5mm, that spacer cube should have moved 0.75mm out as well, but not doing that changed the wedge dimensions just slightly. It’s fine, but I’ll have issues when I do the other size (much smaller) pyramids.
So, we’re talking about machining the center hexagon out of a chunk of rectangular stock?
Yes.
If the stock is slightly oversized then we’re not too worried about exact center, just ensuring that the final solid is within the stock. This also means it doesn’t need to be exactly square either. I suggest drawing the stock as a component and then creating a CAM setup using that stock, then we can see what might work?
OK, so I should expect to have the origin for CAM at the top center of the stock, assume my stock is generously oversized, and mill from there. That’ll save me some milling on the tablesaw (you see, my tune is changing from doing things manually first and only using the Shapeoko for accuracy to just doing the whole thing on the Shapeoko).
One key thing to spot here is that the Z plane is set to be ‘flat’ with the bottom of the wedge insert for machining, not sure if that was clear or not.
Yes, that’s what I was expecting. I think that means the back face of the wedge, where it’s thickest, cannot be cut on the Shapeoko since top of it tilts away from the bottom (it’s vertical when installed, but that’s because the bottom is angled). That’s OK since the wedge is longer than it needs to be and will be trimmed after gluing in place. Will Fusion give me a warning about not being able to mill that face?
As you’re making several you might want to make a jig to hold the raw stock, maybe mill an indent into a piece of MDF?
I don’t think that’s going to be possible, as cutting the sides of the wedge accurately is just what the CNC is ideal for. Now the question becomes do I rough cut each wedge as a blank out on the bandsaw or do I just use the bandsaw to slice to approximate thickness and then cut multiple out on the Shapeoko using tabs? I think not having tabs on those critical sides is best. I can have a stop to register that unmillable back face against, and that works well for the zero point you’ve setup. I guess it’s just tape and cyno glue for stock holding.
So, when you say “do something about the center hexagon”, what needs doing here?
It’s what we discussed earlier, about screwing/glueing the raw stock to some kind of base plate and zeroing manually at the top center of the stock. The Shapeoko can cut both the 6 sides and the top bevels. I need to decide if the sides should be sharp edges on the CNC and round them over by hand, or design in a 1/16" radius rounding to match the pocket made by the ⅛" bit. The later is more elegant, right?
You’re right about the table saw being faster and the CNC being good at accurate finishing, but this isn’t a particularly large part so it won’t take too long.
You’ll need to adjust the stock model to represent the new stock shape and a toolpath to cut the whole surface down.
Yep, it’s a steep learning curve, Lars Christensen’s videos are great for getting the basics
I had a quick look and I think I’d put the hexagons and rectangle from 127mm Hex, 25mm Hex and SpacerRect sketches all in one sketch so that I could use dimensions to hold them in position.
I’ve been watch Lars, but honestly I think he needs a PIP window to show what he’s doing with the mouse and/or keyboard. I know how to dimension rectangles and such, but I never get it the correct field to highlight just at the right time.
You’ll need to adjust the stock model to represent the new stock shape and a toolpath to cut the whole surface down.
OK, challenge accepted - going to try that now.
I had a quick look and I think I’d put the hexagons and rectangle from 127mm Hex, 25mm Hex and SpacerRect sketches all in one sketch so that I could use dimensions to hold them in position.
Well, I certainly don’t know how to combine sketches, especially given doing that inside of an existing history timeline without messing things up later. I guess I’ll worry about those after getting these pyramids built.
Your use of the construction planes to slice things up is pretty strong CAD Fu so once you figure out where the buttons are in Fusion I suspect you’ll do rather well
Am I right in thinking the spacer rectangle is there to set the corners of the cutting planes for the wedge?
Yeah, I wanted the wedge to be between 2mm and 3mm in thickness at the edge of the pyramid on the vertical face (which itself is only 3.175mm tall). I did the spacer rectangles before I understood converting sketches to construction, but even that wouldn’t parametrically tie them to the pyramid size. The point of the pyramid should be on the plane of the near face of the spacer rectangle (which doesn’t have to be a rectangle at all, it’s just spacing so should be a line 2mm long).
So, I’m looking at how to model the pyramid stock in the Manufacture tab. A rectangular box is too big, so the Relative Size Cylinder seems the best bet:
