I just went through and tightened all the bolts for the v-wheels and then checked their tightness to the rail. The bottom two X-axis bolts were not quite fully tight, but it didn’t seem to make a huge difference. However, I did notice that the lower right X-axis v-wheel appears to move the slightest amount relative to the plate when putting a lot of force on the spindle mount. I wonder if maybe the wheel ID doesn’t match the bearing (either a part quality issue or damage from running the machine like this).
Check the V wheels — remove each one and use the bolt for leverage to disassemble them — each is made up of:
- Delrin wheel
- a pair of 608 bearings
- an eccentric spacer
Makes sure that the bearings rotate freely, and that the space is well-centered in the wheel and supported by the internal race — if you have a caliper, measure it and the race and let us know what you find out.
3 Likes
I realize it’s been a while since my last update, but after some more testing with the machine, I really think the issue was mostly due to my overestimation of what the stock machine could do and how hard I could push it.
Yesterday I installed my new HDZ and I’m extremely impressed with the results. I can now take much more aggressive cuts and still have better surface finish than before. The only weird thing I did notice while disassembling the machine is that it looks like my belt guide bearing flanges (on the original carriage) were rubbing on the X axis bar. I’m not sure how this can happen exept if the tolerances on the machining for the XZ carriage were off, but there’s quite a bit more clearance now with the HDZ and the machine is much stiffer.
I’ve also since received and installed steel reinforced belts and they also made the machine seem to behave better. I can tell the machine changes direction much more smoothly. Overall, quite happy with the results. I really wish there was an option to buy the machine as new with HDZ, because from my experience it seems like a requirement to do any serious Aluminum machining (one of my primary reasons for picking the Shapeoko over its competitors).
To address some of the questions above, I did look into the following items and found no issues:
- Tool wear - took photos with a microscope and the tool was not damaged (may be getting dull by now though).
- V-Wheel fitment - everything seemed fine here. When I removed the old v-wheels from the stock carriage there was no wobble between wheel and bearing. The only play in the system was between the threads and the inner race of the bearing. One thing I think could improve the system is using tight tolerance shoulder bolts here instead of fully threaded fasteners, but I realize that would probably cost 10-50x more than the current hardware.
5 Likes
I’ve finally had a chance to start a real project in aluminum so i thought I’d document my findings here for others to see. Only changes from a stock Shapeoko 3 XL here are steel reinforced belts & HDZ.
Here’s what the first part looks like. It’s part of a seat bracket for the racing seat going into my '89 Turbo E30 track car:
2D Pocket:
- New Amana 51459-Z (1/4" single flute ZRN)
- 20krpm, 1000 mm/min, DOC = 0.7 mm, WOC = 3 mm
- Going to push harder on the next one, this cut very easily
2D Bore:
- New Amana 51459-Z (1/4" single flute ZRN)
- 20krpm, 800mm/min, Helix Angle 1.5°
- These holes are only 8mm so not really the ideal end mill for this operation
2D Contour:
- New Amana 51459-Z (1/4" single flute ZRN)
- 20krpm, 1200 mm/min, DOC = 0.7 mm, 2 finishing passes (0.5mm) to prevent wall rubbing
Facing:
- Online Carbide 1/4" 3 Flute ZRN
- 10krpm, 1500mm/min, DOC = 0.5 (rough) 0.2 (finish)
- Single direction pass gave much better surface finish (still haven’t 100% trammed my spindle)
Chamfers:
- #202 1/4" 3 flute Ball End
- Combination of hacked together 2d contours and scallop operations, didn’t work very well, but in lieu of having my chamfer cutters (in the mail from China), it’s acceptable. Lots of chatter and I don’t really recommend this.
I attempted a finishing pass in the pockets with 0.3mm DOC/WOC full depth w/ the 3 flute ZRN and it did not go well. Lots of chatter and I ended up gouging the floor of the pocket. In the future I will completely eliminate this tool path and just run to size w/ the single flute end mill, surface finish was acceptable.
Note on 3 flute cutters - I’ve found they are really only good for facing. In all other cases the single flute has given me a better surface finish and been way less scary to run.
8 Likes
Thank you for sharing, and that piece looks fantastic. I’m with you on the single flute bandwagon, they are basically unjammable (if that’s a word ?) workhorses, and I certainly appreciate the piece of mind that comes with using them.
Yep, I’m on the same page. I tried making a 3-flute endmill work for aluminum and found it only good for facing. However, I do find 2-flute endmills worthwhile occasionally as ball endmills come in 2-flutes and some other specialty ones are easier to find in 2-flutes than 1-flutes.
Edit: My knowledge is incorrect and I need to revisit these parameters again.
1 Like
Awesome looking part!
The single flutes require so much less tq and work so well with high rpm routers, plus wall finishes are usually better because runnout matters less.
Now if anyone made one with a slight corner radius…it would be indestructible! If you ever have a chance to try some Datron 4-1s I highly recommend it. The balance plus wiper really make a big difference. They also make a single flute ball mill 
Was there a reason you didn’t try a 3d contour with just the touch area of the chamfer selected?
Again, awesome part and I hope you’ll be posting up more!
3 Likes
@The_real_janderson Hey Jon, thanks to some coaching from @Vince.Fab I got some pretty good results with 3flute coated bits from C3D using adaptive toolpaths, you might remember from last March. Need help testing cutters
1 Like
@Griff no problem with the 3 flute over here either…as long as you account for the extra chip evacuation needed and machine load/tq. Plus they are capable of awesome speeds!
1 Like
Thanks @Griff and @Vince.Fab for this correction to my memory. I glanced back at the parameters people used and it looked like less than 0.002"/0.05mm for chipload for 3 flutes was important. I just need to go back to that again.
Let’s put it this way then: it’s just easier to get in trouble with a 3 flute when you don’t fully know what you are doing (yours truly), the single flute is more forgiving. It’s like having training wheels.
3 Likes
I don’t have an enclosure or air blast system yet, so preventing clogging on a 3 flute is definitely an issue. Hopefully by New Year I’ll have a table and enclosure welded up and can start running a mister or at least a blast.
2 Likes
Absolutely, no question! 3 flutes are definitely for later in the learning curve.
Just didn’t want folks to not use them based on broad statements. I certainly gummed up a few before I learned how to use them.
1 Like
The only reason I didn’t try a 3d Contour is ignorance of Fusion 360 best practices and because a video I saw from Autodesk about using scallop. Not sure why that was recommended when your way works so much better 
. Much better surface finish, quicker tool paths, and simpler CAM setup, thanks!
2 Likes
I’m glad it worked out! I’m no fusion wizard but know how to cheat sometimes lol. Just wait until you get proper chamfer mills… nothing beats a perfect chamfered part!
1 Like
Where do you buy Datron endmills? Directly from Datron via a salesperson?
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.