Nice tips guys, thanks.
It’s a very new bit, but doing a score type initial cut might work.
How do I setup a .01" score type cut?
Is “stepover” the first initial cut depth? Stepover was set at .1250 in and depth per pass at .04 in.
Is that too much?
A straight bit is better than a downcut bit for plywood?
And coating the wood would work, just an extra step.
Will,
Do these specs look ok for my #201 bit to cut plywood?
How can I adjust it for a cleaner cut?
Thank you.
Amana makes a killer single flute compression that rips at 0.250 doc slotting
1 Like
V,
Which Amana single flute bit is that?
Please send me the link via Tools Today site.
Thanks.
The official feeds and speeds are:
Plywood .25″
Spindle Speed: 18950 (dial settings: 3.5 or 3)
Feed rate: 2540 mm (100")
Plunge rate: 1270 mm (50")
which seems pretty close.
You should test feeds and speeds in a piece of scrap using the technique at: https://precisebits.com/tutorials/calibrating_feeds_n_speeds.htm
you need to make your toolpath twice in CC; first time with 0.01’ as max depth
The Zinsser in spray can is also dewaxed but it has the same yellow label color scheme as the “clear” canned stuff. Very confusing.
1 Like
Yes a second tool path, makes sense!
Now, if I want to chamfer using a v bit, how would I do a .01” score cut?
use the inset tool to create a polygon 0.01" inside of the current one
and then do a contour cut “on the line” set to 0.01"
(assuming a 90 degree V… a different angle means you need to do a little bit of math of what the inset should be)
A,
Thx.
Polygon? How?
And how do I set the v bit to make a contour cut at .01 depth?
A polygon (or polyline) will be the result insetting.
To depth limit a V carving use the Advanced V carving feature — the technique @fenrus is suggesting will work, but won’t preview. To get a cut with a preview, if one has a line which one wants to V cut along and assuming a 60 degree endmill
- inset by half the desired depth of cut measuring along the edge of the cut
- offset by half the desired depth of cut measuring along the edge of the cut
- select the two offset paths and assign a V carving
It is left as an exercise for the reader to work out how to do that with V angles other than 60 degrees.
Will,
Do mean like this? I created 2 paths, and setup a V carve.
It seems like it also works with ONE path right up against the contour cut line too.
Side question:
Has the Amana up-down cut 1/4" bit been getting good reviews? Which is better, 2 or 3 flutes?
Thank you.
Looks great!
Not familiarity with that Amana endmill — probably 2 flutes is better than 3 though.
One other thing to check, I’ve had a couple of sheets of cheaper plywood that just had a very weak veneer on the top surface that splintered no matter what.
Does this ply you’re using cut cleanly with a hand saw or on a table / circular saw?
3 Likes
It’s a very good quality Baltic Birch plywood, fairly thick top veneer too.
It cuts cleanly on my SawStop table saw.
1 Like
OK,
That’s the ply ruled out then, that makes things easier.
With the HDZ and an 80mm spindle I contour cut baltic birch with these settings (from Fusion);
Roughing cut with a regular upcut (the Carbide 201 or Yonico 31215-SC 1/4 inch)
20kRPM
1500 mm / min feed rate
0.0254 mm per tooth
5mm depth of cut
1mm stock to leave
You could also try something like the Yonico 35314-SC low helix upcut if the top is still tearing badly
Finish cut;
Yonico 33310-SC compression cutter 1/4"
20kRPM
1500 mm / min feed rate
0.0254 mm per tooth
3 stepovers of 0.35mm each
Full depth
Repeat finishing pass
Those cuts are relatively conservative because I was cutting a fairly weak shape out of the stock and didn’t want the stock flexing during cutting. The cutters are mostly Yonico just because that’s what I got from Amazon, they’re not special but they’re fairly decent quality for a decent price. They are bulk Chinese cutters imported and marketed as a western ‘brand’.
Given the tear out you’re seeing my first suspicion would fall upon the machine setup, it takes a while to get the hang of the right V wheel tensions in the machine and get everything tight.
What Z axis are you running?
Z axis? I have the Z+.
How tight are your belts?
Great, the Z+ is pretty good, way better than the old belt Z which had to run much slower.
Check all the V-Wheels, I run mine tight enough that I can just turn the lower wheels with two fingers whilst the machine is stationary. It’s very easy to end up with a loose V wheel or two without realising.
On the belts, funny you should ask 
I run my belts at about 70-90 Newtons, too much is bad for the stepper motor shafts and bearings. It’s very easy to check with the phone app method.
I bought the Amana 46176 a few weeks ago. I do not care for it. With Baltic birch (9 ply 1/2" 5x5 cabinet stock…good quality)I have better luck with a down cut 2 flute as long as my piece is clamped securely to a clean mdf spoil board. I was told the Amana bits have to be sharpened much less but I haven’t had to have any bits sharpened yet. I am for work a “traditional” woodworker and am very new to CNC. Just my observation I cut Baltic birch very frequently.
1 Like
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.