My cnc after 7 months is comming under my control. I have had ups and do
wns. I have these little flaws that I think is deflection from a .25 compression bit. Do you guys think its the mach4 setting too fast acceleration?
Did the part shift?
Did you make the same cut on the other side of the board? If so what did it look like?
What was the depth of cut, rpm, and speed?
Is the bit worn?
Were the two cuts made in the same direction?
If you grab the spindle by and and tug as hard as you can do you feel any play?
It is a brand new amana mortise compression bit. I was running .21 deep at 180ipm. It is an old bosch router on for now with an older collet. It seems like no play anywhere. This was same the same board conventionally cut. I’m pretty sure it’s not moving under the vacuum and is not skipping steps.
A few questions:
Based on the photos, it looks like it could be that the second pass came around that corner too fast and the machine “flexed” away from the wood. But that assumes it’s cutting from the good edge to the bad edge? which direction is your X direction? On my Avid, the gantry can twist a bit, meaning fast stops in the Y direction cause deflection (in Y and Z) more than fast stops in X.
A few comments:
If you’re running servos, they might need tuning to stop faster and harder.
If you’re using steppers, you can check for lost steps by moving to a known location before and after the job, where you can measure the bit location precisely, to see if the measurements change.
You might need to reduce acceleration to allow the machine to stop without overshoot.
Make sure your job is set to “curve” around the corner, rather than make a sharp 90.
Most folks who use compression bits cut in one pass, so the compression bit can do its job. At least, the depth must be enough to ensure the “down” spiral cuts to the top surface on the first pass.
To see if the problem is deflection, you could change your job to do a faster pass, but move it 0.050" away from the final edge, and add a full depth finish pass at half your original speed. This might even give you a cleaner edge. If you see worse results on the rough pass, but the finish pass is correct, it’s deflection.
Try a climb cut instead. The CNC has no problem doing this, and it may reduce deflection due to the cutting forces. Or at least it will deflect away from the wood into free air, instead of digging in. Climb cutting also reduces tearout.
Also, take a moment to check that all your bolts are still tight 
Thanks for the input. I am sure it is the x movement, long the gantry direction on my machine. I have been bringing ccp created parts into vectric and leaving .02 offset for a final pass with a .03 onion skin.The dado was cut first with .3 depth at 100ipm. That seems straight after the cut. I’m not sure what pass the dip is happening. Does the climb cut not chip the melamine?..
This is 5/8 material, what speed and depth would you run. The bit im using is an amana tool spektra 1/4 compression 46350k.
This could also be defection on the dado i guess. Going to check the bolts now.
Chipping…
The compression bit deals with most of the chipping. In a conventional cut, the cutting edge is pulling away from the wood (and pushing the bit into the wood), where in climb milling the cut pushes into the wood (and pushes the bit out of the wood). The only area you should still have problems with are corners, where the cut (due to the bit’s rotation) is pushing away wrt the corner’s opposite face. In my case, I have one counter-rotating bit I use just for such corners, but that assumes you have a spindle that can rotate in either direction.
A climb cut also has a slightly less risk of chipping a corner, because that “nub” it produces just before it finishes is being pushed towards the corner, instead of away from the corner’s far side.
Even with just one bit, you could pre-cut all the “towards the corner” edges, then go back and cut the “away from the corner” remainders. I.e. do most of the outline, leaving a bump at each corner on the “chips out here” side, then go back and remove the bumps.
Combining that with a climb cut means that bump is always pushed towards the wood.
You could also do a skim pass with a down-spiral bit, only 0.020 deep, just to cleanly cut the melamine while it still has support under it to help reduce chipping. Again, this assumes you have a system with an ATC, because bit changes take time and can change your relative Z height.
A little bit of veneer tape over problem corners might help too.
Of course, a lot of this is YMMV and “try and see” what works for you, plus the usual time-vs-perfection tradeoffs
If you think you’re getting deflection wouldn’t it be wise to use a 3/8 in bit?
A bigger bit won’t help if it’s the machine that’s deflecting, of course. It also reduces your cut space efficiency.
A bigger bit also means less depth of cut if you have a less powerful spindle, meaning more cnc time per job.
Doesn’t a compression bit only makes sense if you do the whole stock in one pass?
I dont think a compression .25 could cut .625 very well. I have a atc sitting on the bench but no time to install it so I am manual tool changing every bit. Would a down cut for everything but the final pass be wise?
Would you use climb for the pockets and profile? Also would you use the same feed and speed between the two?
A compression bit makes sense as long as the top surface is only ever cut with the down spiral, and the bottom surface is only ever cut with the up spiral. An 0.25" bit will typically have 0.25" of up spiral and the rest is down spiral, so as long as your first pass it more than 0.25" deep you’re good.
If you have an ATC or you’re willing to spend the time to change bits and do passes, it might make more sense to get a 0.25" corn cob rougher and use a single pass with the compression bit for a final. Just leave enough for the final to account for actual chipping. The corn cob rougher might be able to go much faster and earn back some of the lost time.
I use climb cuts for everything, and I adjust the feeds and speeds according to the quality I need, not the shape of the cut. Most people cut way too slow. I rough at 200 in/min (1/2" corn cob) and finish at 60-120 (1/4 spiral usually), with carving at 30 for the smallest bits.
This particular bit has .15 upcut. I was running it 180ipm at first but have slowed it down. What brand and number Cobb are you using? Do they last longer? …The moving away from conventional mill all but got rid of the dip . It seems to leave the surface material a little fuzzy though.
The rougher I’ve been using is this one: The "RIPPER" High-Performance Pro 1/2" Roughing Endmill, 1/2" Shank – IDC Woodcraft
but I haven’t used it enough to wear it out yet, so I can’t speak to that.
I have the 1/4" and 1/8" version of that and they are awesome. Just noticed the other day they have the 1/2" one you mentioned and so I’m gonna get that too. They are super fast cutting, but they cut a lot cleaner than I expected as well.