Really bad cut, wrong bit? What happened?!

I used a high grade baltic birch plywood, but yet the wood splintered badly.
I was shocked, bc my first attempt on the same plywood went fine.
The bit was the 1/4", #201 bit.
Maybe I should’ve used a up/down cut bit instead? Any tips?

Thank you.

oof that splintered badly

few things that I can think off

  1. wrong F&S… like too much force
  2. dull bit?

Sometimes plywood does better with a straight bit but…

… even with bit 201 there are things you can do for splintery wood like plywood
for example, it can be very interesting to take a very shallow (say 0.01") pass first, to basically
just touch the upper layer without heavy forces on the deeper parts, but enough to not get this splintering…



All those things.

How did it sound? Was it vibrating and chattering?

Were you trying to cut that full depth or in a series of passes?


A downcut, or a compression endmill cutting deeply enough to engage the downcut upper portion will work better, or a straight endmill.

Also, please add geometry around the toolpath so that rather than a slot you can cut as a pocket down to at least tab depth — leaving a roughing clearance and taking a finishing pass will help.


There were some similar issues discussed in this thread which might help;

1 Like

If the cut is not through then a down cut bit might work better but looks like the splintering may just move to the other side. Baltic Birch can vary in quality widely. You could try masking with painters tape, Easy Liner Adhesive Shelf Paper (Available at Walmat, Lowes, or Oramask 801 from Amazon and other sources. The masking may not help but it is cheap enough to try with the shelf paper. You could also try adding Dewaxed Shellac on the plywood before cutting. The Zinzer brand of dewaxed shellac is called Universal Sanding Sealer and is available at retail locations.


The Waxed type Shellac is ok if you are not going to put a top coat on but can cause oil and water based finished to orange peel or just not stick. Dont get this type if you are going to put a top coat on.


1 Like

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.


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

Which Amana single flute bit is that?
Please send me the link via Tools Today site.


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:

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)

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.

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?