Does anyone else observe that cuts in plywood or soft woods almost always come out .005-.015 PER SIDE from the toolpath (exterior features are oversize, interior features undersize). I can always make an offset when I need two parts to go together, but I’ve been seeing this for some time now and have never been able to pin it down…it spans multiple machines, bits, cutting strategies (finish pass/no finish pass).
Am I going crazy or is this something yall deal with? My working theory is some of the wood fibers compress before actually getting cut, then spring back, but I don’t have proof of this. My cuts in polycarb seemed to be more accurate, and I havent done much aluminum testing since my rebuild.
I cut mostly climb milling…something I saw suggested was to rough with climb milling then finish with conventional. I’m going to try that on my next cut.
Climb milling produces deflection perpendicular to the tool path, but conventional forces are parallel to it.
I had the better experience with conventional and a little bigger finishing pass. I never really achieved great (but still good) results with climb milling.
Conventional really didn’t change much. Definitely need multiple finish passes too…but I guess it’s time to bite the bullet and start offsetting.
I really wish marlin, grbl, or any hobby grade fw supported g41 cutter comp. I guess it’s too taxing for hobby grade processors? Idk. Been chasing these ghosts for far too long…
I’ve found that when finishing soft woods with conventional, I need to leave a little more for the finish pass to grab. About 0.03" works OK for me on 1/2" stock, a little less for thicker and a little more for thinner. This is assuming I am doing a full-depth finish pass.
But 0.005 is pretty good for these with no compensation, I think, especially with how often I ended up going through mine to check whether bearings had gotten loose (AZ summers over here). Any more than that and it was time for another tune-up.
I presume you’ve already done all the things like measuring the movement at the gantry to confirm your steps, belt tension (had more impact than I thought), measured that your endmills have the diameter that they claim to have, etc, and done everything you can to maximize rigidity like moving the workpiece up closer to the gantry, working in a corner where you have more support, ensured there are no loose-fitting parts, and on and on?
Honestly, this is kinda what is sticking in my craw…my machine should be good. I attempted a project a few years back that required simple wood joints and I had such a hard time I blew my whole machine up for an all metal, screw driven rebuild (New DIY CNC (not MPCNC)). While I haven’t cut much since, my first project was in plastic and as I recall the results were really good, dimensionally.
While I don’t regret the rebuild, I guess I was expecting perfection right out of the gate which is probably pretty unreasonable. Everything needs tuning and offsets, even the Haas I used to run at my old job. Also, wood is freaking weird…I probably get too bent out of shape over a material that is inherently dimensionally unstable, non-homogenous, and frankly sometimes hard to even measure properly.
I went back and measured the part from last night and its really not off by as much as I thought, I was just really annoyed when it didn’t fit first try, after all this effort. While the mortise is pretty uneven (there seemed to be a knot in one of the layers), the overall dimensions were not far from the target. I think I just need to put in the work to make some offsets until my wood joints fit together and just be satisfied with that. I will be doing some aluminum in the future and that will be a better benchmark than plywood. Thank you everyone for the input!
I’m gonna be super honest…if you were running a haas for your day job, there really isn’t much I’d expect you to take away from my experience.
It IS encouraging that you were satisfied with its performance in plastic, which is also really stable.
But yeah, wood DOES move a lot, especially softer woods. I remember facing a pine glueup for a flag (still hanging on my wall), and by the time I got to the end of the path it had already moved. Run the same path at the same height, all of a sudden it was cutting another 60thou off the top lol. You can tell how far off it was by looking at the stars. I keep it because it’s the first flag I made and it didn’t turn out NEARLY as well as I’d expected. More like a country mile away.
I KNOW I don’t need +/- .002 for wood and don’t expect it. What I did expect is when I designed a joint with a certain clearance, which I believed was generous, that I should get parts that fit off the machine first try.
In a way that’s rediculous. I brought up the haas because they have offset tables for a reason, and perhaps I’m expecting more of my hobby router than I even did from the haas. Why? I don’t really know. Perhaps my expectations need as much adjustment as my machine.
I had trouble with fit at first. I think there are many topics about “parts too big, holes too small”
A few calibration cuts and what I found was that telling my CAM that my 1/8" (3.175mm) nominal bit has a cutting diameter of 3.0mm gets me a consistent fit. Parts fit into slots, dovetail joints fit, and part size accuracy stays good.
I cut 3 squares, inside and outside. 50mm, 75mm and 100mm. (What I could use calipers on.) None of the outside cuts fit in the inside cuts with the tool defined onside dimensions were small, outside dimensions were big. My conclusion was that the bit is cutting a narrower than nominal kerf, so I adjusted the tool definition to reflect what I saw. I rounded the 3.0 something something to just 3.0 and it works. I use 2.95 for some very soft woods or a looser fit. Even if hard and stable materials can be better, and might work closer to 3.175, it’s close enough for the tolerances thst I need. I did that a few years ago, and it still works.
Yeah, I also wanted joints to “just work” and… now they do.
Yes, this has been brought up MANY times here. Measure the cut and program that, not the bit when tolerances need to be concise!!! And different materials change it too!
Upside, since you’re using Fusion 360 it has a very extensive tool library. I’m sure other softwares can do the same as I’ll describe, but I know for sure Fusion can.
Set up a library for Soft Wood, another for Hard Wood, another for Plastic, etc. Then create your 1/8 endmill and define the diameter as Dan suggests. The setting can be different for each material you cut, and since you’d do this with new tools, you’ll only have to do it once and you’ll have it as long as you use Fusion.
That would be WAY easier than just guessing a negative “Stock to Leave” like I do.
Yeah, thats a good idea. I also use the negative stock to leave option as well. thats a great option if you dont want to apply the offset to EVERY toolpath on the part.
Again, it would be AWESOME to have g41 cutter comp…making an offset with a simple g10 code then re-running without going back to fusion to re-post would be next level.
That’s a fact. I’d use it ton just setting up the tool.
You could just select the tool from your aluminum library or a “no offset” library for those paths…I don’t know, at some point it does seem like more work.
