I was hoping to show this little thing that had come to life on my rotary module.
Especially with the engraving added to it:
I didn’t try creating it in Luban as I had my doubts that the engravings would come out nicely, so I figured why not try and convince Fusion360 to work with the rotary module. As then I could project have a real engraving onto the curved surface. (which isn’t just a cylinder or something.
Unfortunately, it ended like this ( I was so close…):
It does feel silky smooth though.
What did I do?
I created the project in Fusion 360. imported the STL and then added some helper bodies:
- The see-through blue (with yellow arrow) is the cylinder that is my base for milling. I was using one of the snapmaker provided cylinders for this.
- The cylinder at the bottom (indicated with the dark blue arrow) is the “dead zone”. i.e. if you start milling in that area, you’re likely to hit the rotary module damaging at least your drill bit, probably the cnc module and the rotary module itself. Don’t go there! (this is just a visual helper)
- the two tiny cylinders (red arrows) at the top and bottom which are small tabs that I created manually. to keep the piece in place.
- I also ended up adding two rectangular sketches to limit the milling area explicitly to that region so I wouldn’t go out of bounds and hit the rotary module or tailstock.
When using Fusion, you need to create a setup that defines your stock material and which milling operations you’ll be doing and where you put your origin. The origin point define the XYZ-axis and starting point. This is where the fun begins. You can put that origin in a lot of places ANd you can even flip it around etc. If you’ve ever done 2-sided milling, you’ve probably used this before.
So I ended up creating multiple setups for different types of operations and different directions.
The first one looks like this:
Note that I have put the origin point at the top of the stock. (Not sure if I would do that again, putting it in the center, like Luban does is probably better)
The head of the swan is the part that sticks out. So the rotary module clamps the stock material at its butt. Make sure the Z points up, and the X in the right direction (to the right if you look towards the rotary module)
An important detail is the "Model"Section where I selected both my workpiece (the swan) as well as the to little cylinder tabs I created earlier. That’s important to do, or they will be milled away and well, everything will just fall down.
For the stock material you choose “From Solid” and select the cylinder that was created for the stock. Note that you could use any shape of stock material in this case and then Fusion would take that into account.
For the job itself, it’s basically what you always do in Fusion:
What I did do explicitly was create a region for the Machining boundary. Option “Selection” and select the rectangular sketch. This is mostly to make sure it doesn’t create any paths too close to the rotary module itself. (That gets scary really quickly).
I also checked rest machining, which isn’t important for your first setup, but is convenient to already have selected once you start copy pasting.
On the heights tab it’s probably the best idea to have the depth limited. otherwise, the generated paths will go all the way down and most likely your milling bits aren’t long enough for that.
I’ve set that to from the top, go max 18mm down. The stock material has a diameter of 35mm, so 18mm is more than half that (17.5mm) so it’s enough to have everything removed if I mill from multiple sides.
If you’re doing roughing passes, it’s usually a good idea to leave some excess material:
But if you’ve been using Fusion360 before, that’s most likely something you’ve been familiar with already.
And then Fusion will happily generate the toolpath for you:
(in this case not the most efficient one, mostly because of the rectangle constraint I had put in place that could be wider as there isn’t anything to run into on the sides.)
Anyway, at this point the copy-paste fun starts. You can easily duplicate the entire setup (ctrl-d) or right click and duplicate. and you’ll have a second setup. Now modify this one a little bit by setting the work-origin to the correct place and orientation.
In this case to mill from the bottom up. It’s easier to rotate the image obviously when doing so. If you’ve put the origin in the center, then you just need to change the direction of the axis and not the origin point.
And next on the stock tab you choose “from preceding setup” and check the “continue rest machining” option:
This way, Fusion knows there is already some material gone and it doesn’t have to clear that anymore.
And now repeat for each direction you want to mill from. And that way you can easily see how it’s proceeding and your workpiece is appearing from the stock material.
Although you could probably create all toolpaths under each setup, I decided to separate the roughing and finishing passes. But it’s pretty easy and straightforward to duplicate them and to copy toolpaths between the different setups. Only thing to watch out for is to make sure to use the right sketch to control the toolpath boundaries. Other than that, you can just copy-paste.
And this way, I was sure that I could use the project toolpath for the engraving. Unfortunately I didn’t get there.
But there is still one step to do: actually create the gcode files. You basically have two options:
- Run each toolpath separately and in between jobs rotate the module to the right position.
- Paste them all together and insert between each job the correct rotation command.
Obviously I went for the last option. You can select all toolpaths with the same tool that you want to execute. For example all roughing passes in the 4 orientations and then click the PostProcess option:
This will create one file with all toolpaths. Fusion will give you a warning that it includes paths for different orientations. but that’s why we will insert the rotations manually. It’s convenient if you give the different toolpaths unique names, because then you can search for them in the gcode file. and before those you can insert the gcode line to rotate.
You should then get a file similar to this one: (I reduced all actual toolpaths to only two lines)
;1001 ;Machine ;vendor: Snapmaker ;description: Generic Snapmaker Marlin v20180725 M3 P100 G4 S2 G21 G90 ;When using Fusion 360 for Personal Use, the feedrate of ;rapid moves is reduced to match the feedrate of cutting ;moves, which can increase machining time. Unrestricted rapid ;moves are available with a Fusion 360 Subscription. ; make sure you are at rotation 0 degrees as the top ;Top Rough Adaptive1 G0 X10.907 Y29.267 Z15.000 G1 X10.907 Y29.267 Z15.000 F400 ;Rotate manually ;First go up a little bit (actually not necessary as Fusion already does this, just to be sure) G0 Z35.000 ;Next rotate to the right place G0 B180 ;Bottom Rough Adaptive1 2 G0 X10.907 Y29.486 Z15.000 G1 X10.907 Y29.486 Z15.000 F400 ;Rotate manually ;First go up a little bit (actually not necessary as Fusion already does this, just to be sure) G0 Z35.000 ;Next rotate to the right place G0 B270 ;Left Rough Adaptive1 3 G0 X-10.963 Y4.619 Z15.000 G1 X-10.963 Y4.619 Z15.000 F400 ;Rotate manually ;First go up a little bit (actually not necessary as Fusion already does this, just to be sure) G0 Z35.000 ;Next rotate to the right place G0 B90 ;Right Rough Adaptive1 4 G0 X10.963 Y55.381 Z15.000 G0 X0.000 Y0.000 M5
Et voila, you have a single gcode file you can run. Obviously, you still need to create one for each tool you’re using.
Is this real 4-axis milling? Obviously not, but it gives you an easy way to do multi-sided milling and you do get the advantage of being able to use the more advanced toolpaths Fusion360 can generate. The effort needed is obviously a bit more than the easy way to start your job from Luban.
Ok, cool story, but where did it go wrong for my job . I’m not sure yet. I think my tabs were not big/strong enough and I was a bit too aggressive with my finishing pass. I started conservative, but those cylinders seem to cut so easily and I increased the speed. A bit too much I guess.
Other things I’ve noticed/remarks:
- working this way means that the origin point needs to be exactly spot on. a tiny bit to the left or right and you get two halves that shifted a bit. (it’s either that or my module wasn’t perfectly perpendicular) to the base plate. It’s this border that you see here that’s caused by that:
- I’ll have to measure closely, but I’m not sure that supplied v-bit is really 20 degrees. Either that, or there is a wobble in my cnc head or I didn’t specify the tool right in Fusion, or Fusion is bad at calculating slopes for this type of tool. because it seemed to have removed too much material in the finishing pass in the slopes:
The green is actually before the finishing pass and the red after. The green looked better. Easiest solution is probably to not allow to do slopes this steep with that tool.
- I forgot to tighten the set screw in the tailstock, as such, that didn’t give all the support it could have.
- I only did 4 sides. Nothing is stopping you from milling from multiple angles. But if you deviate from quarter turns, you do need to create extra origin points manually. Once that one is set (e.g. with rotations at 45 or 30 degrees) it’s just the same way of working. This video shows how you can create extra coordinate systems: Creating and Using UCS (User Coordinate System) in Fusion 360 - YouTube
- If I do it again, I’ll probably set the origin points at the center of the stock, like Luban does. Once set, it doesn’t have to change (same if you put it at the top) but at least the gcode previews will make a lot more sense. When it’s not at the center, the previews don’t make any sense (when opening in ncviewer for example)
Other than the little issue I had, I think this way of working does have a lot of potential and I think I will try it again. I’ll probably make a base template document that could be easily reused for multiple projects.
But maybe I should have tried Luban first. At least I would have made it before Valentine .
Hope this helps someone.