It probably isn’t worth it for a lot of projects, but I was wondering if anyone has tried a multi-bit project on the X-Carve where after using a normal straight bit to make edges you’ve changed bits and had the X-Carve run a round-over or chamfer bit over the corners? The fancy approach would be to add the bit to the Fusion 360 tool library and model the final operation.
Usually it would be easier to just mount the bit in a router table and do this manually, but maybe someone was curious.
I’ve definitely done this to put a chamfer on edges. Some of us don’t have router tables.
Another idea is to use the X-Carve as a sort of inverted router table. Putting a round over bearing bit in the machine and lowering the Z-Axis so that you can push the work piece up to it.
I actually use forming bits on my router all the time. Most of the time before chucking the bit I walk it around my piece to see if there will be any obstructions or areas that dont need to be cut. With the bit in place, I am able to take it nice and slow and move the router around the area to be cut. May not be the best method but Ive figured out how to do it safely and slowly. I also use Vcarve Pro and it has instructions on how to add forming tools and use them with toolpaths. Just remember to be in the moment when working near the moving bit, safety glasses/shields are good too!
James
I haven’t played with a roundover bit yet (still pretty new with my x-carve actually) but last weekend I just used a groove bit (1/2" half circle) to carve a drip channel into a cutting board and it worked out pretty well. I would imagine that as long as you zero your machine carefully - and it’s definitely more challenging with an odd shaped bit - and as long as you manage your feeds and speeds properly you can probably use any router bit within reason.
Someone with more experience please jump in if I just suggested something that could turn a project into kindling, but from my limited experience this should be possible. Have fun!
If you use a chamfering bit that comes to a point, just load it into the spindle and tell it to cut on the line down to the depth of the chamfer you want.
I have not tried it yet.
However I think it is possible. You just need to make sure you create a tool path for the bit to follow that is the right distance and height from your part.
I think the first question to answer is whether you “model” the roundover/chamfer/profile in the model and then select a bit which fits that profile, or do you have to figure out on your own how deep and in what position to cut and just tell Fusion to follow the line. I’d like the answer to be the first approach because that would let the simulation and rendering tools work well, but it could be the second way.
Of course the question after this one will be about doing this with bits that narrow towards the shank like keyhole or dovetail bits…
Also… this is what I would use if I had a lot of round over stuff to do that was more complex than a router table could handle.
Point Round over bits:
http://www.toolstoday.com/showProduct.aspx?SEName=beadboard-router-bits&ProductID=6208
With a pointy bit, it’s the same as a chamfer, just have it cut on the line down to the proper depth of the radius. You might have to fake Easel out with another bit selection.
I have in mind doing this with Fusion 360, this is all probably beyond what Easel can deal with.
Yeah, that’s why I said you have to fake out Easel and cut on the line. Totally doable…
These days I’m designing everything in Fusion, but then using Easel just as the gcode sender. Tonight I did a triple bit carve using the machine’s limit switches as a reference, and took advantage of rest machining to make things pretty quick and eliminate air cutting. I’m still learning all of this, but I’m starting to get comfortable with the process. The carve in the picture was done with 1/4", 1/8", and 1/16" bits in about 3 hours total including setup time.
what is the process for using the limit switches as a reference in Fusion?
How do you tell Fusion the relationship between the limit switch position and stock 0?
Sorry for the slow answer. The machine limit switches are actually pretty precise and repeatable. So I put a hardboard auxiliary waste board down and an engraving router bit in the machine that has a sharp tip. Then I homed the machine against those switches and then instructed the machine to move to a convenient position, in my case 100,100mm, then lowered the Z until the bit made a tiny point in the waste board. I then moved to a few spots at X+N, Y+0 and marked a few dots parallel to the X axis, then did similar for Y. Then I put down two thin straight wood strips with double sided tape with the inside edge on those dots. So now I know that if I secure a blank against those stops, all I have to do is home the machine, then go to 100,100 and I’ll have a consistent reference at the front left corner of the stock.
Now for the Fusion side. I wanted to home Z off the waste board and not the top of the stock, because if I’m doing a 3D carve the top of the stock might not be there for the second bit. So I add an extra body to the model which gives me an artificial home for the model. You can see it here:
That front block is 50mm from front to back and 25mm high. The 50mm is more than the width of those wood strips I taped down to the waste board, and 25mm is higher than my stock. Note that the back edge of that body lines up with the Fusion stock dimensions (including any offset (20mm in the above example), and I have the top left corner of that body as the CAM home point. The reason I mention that the 50mm is wider than the wooden strips is that the strips won’t be in your way when you set the Z height of the bit.
So I put the material in the X-Carve against the wooden stops, then home the machine, move to 100,100mm, then move Y-50 and lower Z to meet the waste board, then raise 25mm and set that position as home. I can then carve with the first bit, then switch bits, follow the same procedure and carve with a second or more bits and they’ll all be lined up.
Now there’s another reason why I set home 25mm off the top. I’m using Easel as my g-code sender and when Easel finishes a carve it moves right to home after only doing a minor lift. If the home was actually set to the top of the waste board this would probably result in the bit crashing into what you just finished carving (ask me how I know this). So making the home artificially above the topmost point of the physical stock ensures that this will not happen.
I’m sure this sounds complicated as text, but once you try it in practice it’s pretty easy. I should probably make a video of doing this, but that’s probably not going to happen for at least a while.
it is interesting.
I have been carving art pieces into arbitrary stock using a split top table and one of the challenges is that I need to be careful not to lose Z, and have consistent challenges lining up the bit after the change.
so here is a screen shot of the stock for my current carve:
the output will look something like this when it is done (this is the last time I tried it…):
and here is an example of stock in the table, mounted for carving:
I am using Fusion as a modelling tool and Easel as a G-code sender.
My challenge is that the stock I use (firewood, basically) is irregular and oversized, so it ends up mounted in a different place every time. I am trying to carve the entire z-surface, which means by definition I am going to lose zero every time I do the first cut,and have no good way to re-zero after the bit change. If fusion had a bit position display, it would be easy. Without that, I am kludging it.
My current tack, which has not worked perfectly, was to try to expose a very small portion of the final surface through the top of the stock, and use that as Zero. I am mostly doing faces, so the tip of the nose seems always to be elevated. so in Fusion I poked it though the top of the stock, just a little, and made that point zero.
What I found was that it worked until I did the smoothing pass. That pass seems to have cut the marks out of the stock, so now I have a nose tip but not a good zero marker.
I was looking in Fusion to see if there were a way to define zero a set distance from a known point, like an offset, but could not figure out a way to do that.
I guess you are doing that with model parts, and that is interesting. I’ll have to think about how I could make that work, maybe by setting the stock, measuring by movement the distance from the stock to a known point, and then adding a block to the model to generate the offset. seems complicated, but I guess it might work… any thoughts?
Very interesting, what are you using to scan your stock (firewood)? BTW, if you scan every piece of your firewood you should get a job with the TSA 
I’ll have to think about how you could use some of these techniques. Don’t know if you use Easel as your gcode sender, but if you do you want to always use a home point that’s at or above the top of your stock, but that doesn’t have to be a “real” point, as I showed it can simply be a fixed distance above a point on your wasteboard.
What about making two L shaped pieces (maybe with ruler markings on top which could be used to make a bounding rectangle around the piece of firewood. The ruler markings would tell you the size to make the stock box in Fusion, and if you make the L pieces a known and convenient height a little less than the height of your log. You could use the top of them as a top surface to touch to and then raise an offset from for the Z height.
Couldnt you clamp a square piece of wood or something elsewhere on the spoilboard and use that as your zero reference? If that piece is the same starting height as your material you should always have a place to start and just adjust the size of the work area to fit both reference and material.
James
so the stock workflow I have developed is:
import that into meshmixer and fix any holes, using the analysis/tools features (this is a different piece of wood, but you get the idea…)
import THAT into memento and turn it into a .obj(quad) mesh with < 10k faces, so I can import it into Fusion
import the wood model into fusion. measure the model in fusion. measure the model in real life. scale the fusion model so the measurements match
set the actual thing I am going to carve into the model, and scale it into the face of the stock (different project, but you get the idea)
physically mount the stock into the x-carve, level it, and clamp it in place.
set the zero point: this is always a point on the top surface of the stock piece, to date, as I am using a model for the stock. To answer the question of another commenter, I have not to date used a stock box reference for anything, as the stock I am using is literally not box-like, and I have devised no way so far of recovering a reference to a point on a stock box after I start cutting.
create the G-code
start the carve.
I would hesitate to call any of this best practice. It is what I do right now. It consistently creates small errors in bit placement at the start of the second cut, after the bit change. I need to fix that, which is why I am seeking advice here.
the height and position of the stock changes with every new piece I mount. It would be very difficult to get any sort of consistent placement. so the challenge is to set a zero point and an offset to a known point on the stock, which the toolpath generator can then use to define the toolpath for the carve…
