I decided to mill half of a propeller that I generated in Onshape right after I retired.
I was bored out of my mind, so I made profile gauges out of thin mdf, cut a 2x4 into 1.5 x 2 x 12, then proceeded to 1" belt sand the block into a propeller. It was an exercise of futility, but consumed enough time and energy to survive.
Now, with my new S05 it’s time to try again. One side only, no flip yet.
I attached the setup sheet from F360. Any comments/warnings or words of wisdom are welcome.
I plan on using Carbine Motion for the machine communication.
I’m not an expert in 3D carving (which is effectively what your propeller is), but if I was machining this, I would do:
Adaptive #201 to clear the bulk of the material
Bore for the center hole if it was too small for the adaptive to clear it, or a contour pass to clean that up (tool depends on the hole size)
Parallel operation to clean up the contours, 1/8" ball nose might be good for that, simulation would help tell you if that’s the case
If you find that the #201 is leaving too much extra material, you can add in another adaptive pass with #108 to get that closer and make the ball nose end mill’s life easier.
I am interested to hear what you end up doing for fixturing and indexing to be able to flip and machine the second side of that propeller.
No expert here as well. That’s why I floated this by the group.
I will not touch the face of the hub. I was going to drill the center hole (1/4") and use that to hold down the stock and use a fillister head screw in case. I was going to butt a couple clamps to the stock to keep it from rotating.
Three Adaptive passes.
1.) Conventional 1/4 flat end mill. Max DOC 0.1 , Max stepover 0.1, Leave 0.010 material, 10k rpm
2.) Conventional 1/4 ball end mill. Max DOC 0.005 , Max stepover 0.08, Leave 0.005 material, 10k rpm
3.) Climb 1/16 ball end mill. Max DOC 0.06 , Max stepover 0.03, Leave 0 material, 10k rpm
As I recorded this I think I could do better, but lessons will be learned.
I think I can increase the Feed rates, I am using the Carbide defaults as shown in the Setup sheet.
I am using a 2x4 as the stock material.
I have been thinking about the flip. I will need dowel pins to realign the part.
I have a concept, but no reality.
For flipping here is what I would recommend (by no means the be-all-end-all)
Extend stock so you have full height stock left out past the ends of the propeller
Run a surface pass (with a fly cutter possibly) so that when you flip you have a good surface on the waste board
Drill holes in the ends of the excess stock for dowels (I would drill these holes on the centerline of the propeller). These holes can either be spaced for use with existing holes on you waste board (if you have some) or go into the waste board for your dowels - this is totally dependent on your waste board & your preferences.
While you should still check your origin after flipping, given that your model origin is center of the hub, dowels on the propeller centerline (along the x-axis) should put you dead on.
I got an education today. Some success, a “O sh.t” and the realization I can’t mill the geometry with the tools I selected.
Success = After some reading on the forum I got Fusion to spit out gcode that I didn’t have to edit.
Fusion seems to need to be restarted to get settings to execute as expected.
I got the first Adaptive path to run and produce expected results.
Start to run the second Adaptive and it all went down hill due to lax oversite on my part.
Sent a 1/4 ball end mill into the screw I had holding the stock down.
1/16 ball end mill on the Hub stock. Flutes not long enough. Changed 2nd pass to 1/8 ball end mill. No crash but it will miss a little stock right at the fillet between hub and blade . I will run that today.
Other than getting a bit with longer flutes, if the part allows it you could have that central hub wider in the middle and tapered to top and bottom instead of purely cylindrical?
Would be quite a bit slower in terms of toolpath though, I might just buy a longer fluted cutter.
You are correct, but the goal of this project was to get anything 3D from Fusion and try to mill it.
I don’t need the part, just the education. And that has been successful, just hope it sticks.
Additional issue
1.) I got a Carbide tool library that was converted to Fusion tool library from the forum.
I used that to generate a tool path using an 1/8 ball end mill with no collisions
I was inserting the 1/8 tool into the ER11 collet and noticed the collect was probably going to hit the Hub.
I checked the Tool library data and noticed the Overall length and Distance below the holder was the same. Oops.
I changed to a 1/4 ball end mill, just to finish the cut. Hopefully run that this afternoon.
I attached a Zip file containing a Propeller.zip (1.6 MB)
ACIS .sat, Parasolids and .step files of the propeller if anyone wants to play with it. I doubt it is very functional and it looks a bit clunky, but something to play with.
I saw your upload too late, so just grabbed one from GrabCad. I would start like this, with the workpiece 2" longer than the finished part. Offset the outline for the 3D milling, except on the ends. Offset the hub inside by half the cutter. Then use the 2 offset vectors to boundary your 3D cuts.
The biggest issue is the Hub is 1.5" in the Z and the blade is maybe 1/4", centered on the Hub .
The Hub diameter is too big and should have a draft angle.
Flat ugly and out of proportion. I was more focused on the blade.
This maybe tonight’s brain burn while watching the LLWS.
I did just learn in Fusion to Edit → Geometry → Incude Setup Model means to EXCLUDE the model, so that the User selected Surface, Face, Body is the only thing that gets a tool path.
That solved my confusion as to why additional geometry was being considered for paths. RTFM
One option to support those thin sections is to use the machine to mill out a fixture which is a matching ‘socket’ for the part when you flip it. You can put holes for the alignment pins in the fixture and a reliable ‘hard point’ to zero off too. Creating the matching fixture is an easy boolean operation in CAD, followed by a little offsetting by a few tenths of a mm to create clearance for the part.
