I’ve seen posts of wood CNC projects that have claims of flat no sand pocket cuts. My pocket cuts always need some sanding, even with 30% crossover. I’ve looked for, and bought, bits that were to be flat bottomed, The Jenny Bit, but they are not truly flat. I understand the geometry to reduce heat build up. Perhaps an end mill with offset flutes that would cancel each other’s angle. Anyone have a source for truly flat bottom end mills?
Vozy, I think it’s probably more of deflection of the wood as an upcut bit will pull the wood up and a downcut bit will deflect the wood down against the spoil board, particularly if you make passes at .25 DOC or more. The only suggestion I have seen and it seems to help me, is to make a last pass in depth of about .003 inches, and it’s such a thin cut, I don’t get the deflection regardless of the bit used.
If you use V-carve, you can edit the pass depth on the pocket mode on the right side when setting up the pocket, just tick the “set last pass depth” and enter your choice.
Just read this and have been using Vectric for quite a while and not seen this option, I will exercise this from now on.
Thanks for the tip
Thanks for the advice. I’ll try this on my next project.
Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.
Just to caveat this, technically it depends on the geometry and chipload if flattening the tip will help, in general it won’t or won’t by a useful amount. Other than when you plunge you are always cutting through the material with the edge profile of the bit. Think of it as you are cutting from a hole (your previous cut or plunge), then moving the tool from that position by your chipload. So the missing center section does not effect the cut other than potentially making the edge slightly weaker. One of the other issues with a true flat tip is that the tool would not be able to plunge.
There are multiple issues for why you get different cutting artifacts in the bottom of the cut. What you are seeing is probably related to one of 3 things.
Deflection as Jim pointed out is one. This is basically the machine and tool bending into the cut due to the cutting forces. You can reduce the chipload (feeds/speeds), pass depth, stepover, or tool diameter to reduce the cutting forces. Keep in mind that reducing your stepover will lead to chip thinning when cutting less than 50% of the tool diameter. Additionally, there is a minimum chipload for every material and tool geometry combination.
You may also need to tram your spindle/router. This is where the bit is at an angle relative to the X/Y and will cause steps. It will make one or more sides of the bit cut at an angle instead of flat.
The last thing is the tip geometry but not the way you were thinking. Any bit with a “sharp” corner can leave some artifacts behind. This is due to a number of reasons and partially related to the material being cut. A solution to it would be to look for a tool with corner radius (bull-nose). These when properly designed with have more of a sweeping edge at the corner rather than a sharp point and will leave a smoother cut. Keep in mind though that they will also leave that radius in the in bottom corner of the design.
Hope that’s useful. Let me know if there’s something I can expand on or help with.
Thank you for the information. Lots of good stuff. My tram is good. Flattening leaves surface dead flat. The surface of my pockets remind me of plowed field but not so extreme, rows of barely raised surfaces. Using a bull nose bit is intriguing. I hope there’s a difference between bull nose and ball nose because using a ball nose bit will produce the opposite profile on a pocketed surface. Bull nose, like a small bowl bit? I’ll look into this. I don’t fully understand chip load but I keep mine above .002 and below. 003, usually. 0023 to .0028.
One other thing to consider with deflection is that as it bends the tool/machine it’s also pulling it out of tram. Think of it as if you were leaning on the bit until the machine bent in that direction. That would change the angle of the tool relative to the cut.
I can’t really even take a guess as to if you are deflecting as I don’t have enough information. I’d need to know the tool geometry, tool diameter, material being cut, feed/speed, and plunge in addition to what you have already listed.
I can say that with a 30% stepover and only a 0.002" - 0.003" chipload you are probably starving the bit and potentially rubbing. So some effects of the poor bottom finish may be due to that too. Part of the issue here is that you aren’t really cutting that 0.002"-0.003" chipload with a 30% stepover. With chip thinning you are only actually cutting 0.0018" - 0.00275". In addition to that those are rule of thumb starting numbers for 1/8" cutters in soft material and it won’t maintain that in direction changes.
If you are using a downcut bit that can be an issue too as the chips are forced down the flutes and can be recut or forced through the tip marring the bottom surface.
Corner radius or bull-nose bits are not ball-nose. I’ll give an example of one that I know, a 1/4" tool with a 0.060" radius. To be a ball-nose it would have a 0.125" radius. You should see them listed like that with the actual radius of the corner of the flute. That radius is also the radius of the rounded edge you will get in the bottom.
Let me know if there’s something I can help with.