Downcut or Downcut/Upcut Compression Bit for Plywood?

Hey fellow CNCers!

Just got my Shapeoko Pro machine up and running! I did my first cut in MDF and looks great. Grabbed a piece of cheap plywood to do the same cut using the .25" upcut, 3 flute endmill and it cut easily but tore out the veneer badly.

After some hunting, I’ve found some advice about using a downcut or downcut/upcut compression bit to avoid the tearout.

Do any of you have experience with plywood and these type of bits? Would you have to make any changes feed and speed changes using a downbit?

Any advise is appreciated.


1 Like

Compression bits are cool but that first pass has to be deep enough. The up-cut flutes need to be completely submerged in the wood and the down-cut flutes must be cutting the top grain. This Depth of Cut (DOC) is something you can control in your toolpath setup. Pay particular attention to the dimensions of the compression bit you buy, especially the distance from the tip to where the cutting blades change direction.

I’ve been doing a lot of cutting over the last two years and TBT I never use an upcut anymore or compression. I can’t stand the tearout with an upcut on plywood (which I have done a lot with) or really with any type of wood. It is true though that you have to slow down to allow the chips to clear. I use GWizard for my feeds and speeds and after hundreds of cuts it has not let me down (sorry Jerry it’s true. :slight_smile: ). Get the free version and get ready for the spam flood.

If you want to use a compression (have a couple really good ones that I never use) you have to think about how it is configured. When you do the first pass it is essentially an upcut and will result in tearout. The way to be successful is to leave a small amount of material, do the cuts and finish the profile with a finishing pass of the full cut. With the bit in this position you get the full benefit of the compression. The upcut on the bottom surface of the material and the downcut at the top. Or you could just use a downcut and keep close track of your machine bed Z. Btw, this only works if the upcut portion of the bit is shorter than the thickness of your material.

Here is my plywood process for a profile cut.

  1. Start with a downcut. Get the feed / speed from G-Wiz to program the toolpath.
  2. Set the machine bed as Z zero. I have the touch plate but it’s faster to do it another way. I have a machinists brass reference block that is a .5 inch “stick” that I set on the table. I lower my DC bit to just a little lower than the block and raise it 1 mil at a time until the block just slides under the bit tip using this device. Thanks Howard! This gets about as close to exact as possible and is faster than using the touch plate. I also like leaving a few thousands of material (it’s called onion skinning) on the bottom of the ply. You can push through the skin with your finger and then run a sand block across and it does not tear the material out. This also saves your spoilboard from looking like a war zone.
  3. I can’t remember if you have the ability to do this on ShapeOko but I set my first pass and last to .032 and use the 1/2 bit dia DOC for the inner passes. I’m not sure if this is necessary but it always works and I’m never in a hurry. Plus it’s so cool to see the clean line that this process cuts in the ply.

Anyway good luck! Congrats on your new toy…


1 Like

Love the suggestion of a full-height finishing pass to get the most out of a compression bit!

And yes, pendants are pretty cool too!

Perry, how do you hold down the workpiece?

Hey Tim,

At first I tried placing a heavy object on the material, but she kept moving when I turned on the spindle. When that was not successful I used a variety of “creative clamping” strategies and blue tape / CA glue. I never drill into my spoilboard except when using dowels for double sided part cutting.

  • First of all note that I have locked in X and Y fences that I can push one or two edges of the material against if necessary.

  • Plywood with tabbed cutouts are easy to clamp around the edges. Just verify before starting the cut that you will not hit the clamps. Then verify it again…

  • In some situations I had internal circle cutouts in the plywood (full cut depth) where I would clamp the outside of the ply and cut the inner circles (or whatever shape). When that was complete I would move the clamps to the inner cutouts and cut the outer profile.

  • If I have a large piece that I want to do a profile cut out on I will clamp one or two sides and do a partial profile. Then move the clamps to the cut profile sides and cut the rest. Keep in mind the direction that the cut will go and clamp accordingly. In other words if I am cutting in the Y axis direction I want a fence or clamps along the X axis to keep the ply from sliding. If you are using finished ply this is even more important as it is a little slippery on the MDF.

I am also a big fan of blue tape and CA glue. It’s amazing how well this holds. You can also use shelf paper in the same fashion for larger areas. Yeah really, it does work! For larger pieces I could use tape squares around the corners to avoid having to tape large areas of the table.

I can clamp to the front of the table as well for a simple way to do end joinery…

Let me know if you have questions!


1 Like

At first glance I understand you to be saying your hold-down technique is your cat?! :rofl:

1 Like

Not quite ‘tiger claws’ but ‘kitty claws’ might work too.
I was thinking the same thing when I saw the pic and started reading.

1 Like