Hello all, thanks for reading. This site has been a Godsend for knowledge, so thank you to all contributors. I’ve been extremely slow getting up to speed since getting my original 1F, and am tackling tiling.
I’m running a J-man on a QCW (from below) and a Makita with a Whiteside RU2075 ~1/4” Ø upcut. The model & g-code comes from Aspire 11 using 1F post processor mm v2. I have it set up to do an offset pocketing (versus raster) function. I set the 1F controller to .01mm tolerance (I noticed the previous setting was .05mm).
I put a 3/4in (19.05mm) doghole in a plywood scrap I intend to use as an x-zero bound/fence to make placing big pieces (sheets) easier. The hole was intended to be used in a tiling practice run.
The hole came out at .7400” Ø (roughly .25mm off) measured using a Mitutoyo caliper. I’ve input the actual Ø for the bit (as measured in a cut piece of MDF….2475”/~6.285mm) into Aspire, thinking that was key to maximum accuracy.
Scratching my head…what am I doing wrong? Obviously the model thinks it’s .75"/19.05mm, but real life isn’t matching.
I am by no means an expert in wood working. I have used to be a machinist in metal. If you do not have any offset for your finish pass, I would say what you are experiencing is the wood contracting or releasing stress after you cut the hole making the hole smaller. I would run the hole and back the tool out, then bring the tool back in and run a finish pass to the same size.
Thanks, I’ll try the finish pass technique. I didn’t use an offset for my offset pocket (if that makes sense). I just wanted it to spiral out (not raster out) a 19.05mm Ø circle.
Since it’s plywood (with cris-crossed layers, not grown solid wood), I would think the stresses are minimal (additionally, the hole is round, not oval…so the assymetric internal stresses of which you speak–I would think–would be obvious. Having done my own porcelain tile installation not too long ago, I know exactly of the internal stresses you speak and how they can ‘curve’ a cut.).
From experience softwoods tend to ‘undercut’ as they tend to tare leaving microscopic “stringy bits” behind (yes that the technical term). In addition to that there could be some rounding going on as the circle is converted to a series of linear movements which is controlled by the tolerance you described. I would suggest a secondary finishing pass to clean up the wall of the hole after you pocket it out. I would use climb cutting for the pocket operation and conventional milling for the finishing operation.
For what it’s worth when I fit truss rods I will start with a known good tool path then test fit the truss rod and adjust the cut larger from there. Different wood cuts slightly differently.
You may need to make a mm/step adjustment. There are threads on the topic but I’m on my phone and can’t search very well. Basically what it boils down to is that there is a fudge factor that allows you to fine tune exactly how far your machine goes when you tell it to go a certain distance.
The standard procedure is to use MDI to move the machine 1" and then measure how far it actually moved. Repeat at mid-travel for the axis and then full-travel for the axis. There is some math to associate the measured delta with the fudge factor. Plug your numbers into the controller and repeat the test.
I was aware of the {edit} commanded move/actual move measurement. I’ll find out more about manual data input (MDI…had to BraveSearch it). It sounds promising!!!
When dealing with wood in general I think you’re going to find .010 is an acceptable tolerance. First the 1F doesn’t actually make round holes. It makes short little straight lines that make up a roundish shape. Then you’ll find that wood will compress some and it’s speed dependent. If you go too slow you’ll burn the wood. Too fast and the wood will compress slightly and spring back. Most woodworkers try for 1/64" but accept 1/32" (half of what a standard tape measure will read). You’re less than 1/64" off. Then there’s the bit. If it’s off even slightly it’ll make a difference.
I just ran into that when working with 3/8" dowels with hard maple. I had a Vermont American brad point bit and when I put a dowel into the hole it fit loose (dropped in and wobbled). So later that day I stopped in a different hardware store and got a different brand of dowels. While there I picked up a Milwaukee brand drill bit with the idea I could use a dremel with a sander on it and slightly reduce the diameter.
Turns out the Milwaukee but was just enough smaller that the dowels fit snugly. My Mitutoyo calipers say they are the same size but the dowels disagree. Was it the wood? Was it the bits? Not sure but the accuracy of the Mitutoyo calipers is about .002" so the bits could have been that far off. For a 3/4" hole made with a 1/4" bit if it’s under by .002" then your hole will be under by .004", or almost half of what your measuring.
I would do a couple tests. First try making the 3/4" hole in different species of wood. See if they are all off by the same amount. Then I would manually make a 1/4" hole by moving over a piece of wood and then just use the Z axis to bore a 1/4" hole. Then measure them. If all the 3/4" holes are off by about the same amount and the 1/4" is actually 1/4" then I would look into making a fine adjustment to the 1F to compensate.
My J-man on QCW was set to X 15.99 (not sure if 1.0.9 changed this from 16) and Y 10.00.
By using the procedure (h/t CyberReefGuru), I found my J-man on QCW was actually X 15.985 and Y 10.011. I hope that helps someone else (though I have no idea what the thread per mm tolerance is).
Thanks Derek, I cut the old hole with a finishing pass and got a slight oval that the notional .75" pin fit into.
So, I cut a new hole using climb for the rough and conventional for the finish. The pin fit, with no obvious oval. Calipers (as well as I can measure) show .7475-.7485" (18.9865-19.0119mm).
Interestingly enough, (for poops and grins) I re-measured the swath this bit (Whiteside RU2075) cut in plywood…getting a different result from my previous measurement in MDF! Operator error? Diff in material? I had thought it was .2475”/6.287mm Ø, but now see .2425”/6.1595mm Ø, which would explain why a 19.05mm hole ended up being a rough average of 18.9992mm in Ø.
So now the game becomes turning this into a ‘known cut+wood’ combo…in Aspire, do I enlarge the bit, or enlarge the hole (I’m guessing the latter)?
(As an aside, I power down because in 1F BB controller I can’t eject the USB drive on which the file sits, and I don’t want to just pull it…without SpinRite-ing the USB to find out what’s going wrong, all I know is that Windows 10 is intermittently objecting to the USB when I put it in from the 1F, and W10 has to “fix” it.
In regards to tiling and flipping pieces (2-sided carves), how do I get a consistent zero position between power downs (assuming I never moved the piece)? Does everyone just use previous zero X&Y positions–i.e., write down zero before powering down? “Peg it” before power down, then just re-clamp off of old peg?)
I’m late to this dance and perhaps you have solved the problem by now but I will offer a couple of additional suggestions that I didn’t see mentioned in the thread.
First and most importantly, measure the diameter of your bit to assure it is truly 1/4" in diameter. You are relying on this and I wouldn’t be surprised if it is off. If you get a different dimension that 0.250", then put that diameter in the tool database associated with the tool.
Second and less important, measure the runout of the bit in the router. Makita collets are poor performers at best. They use a split collet which can and typically induces more runout than you find in a ER type collet. This is a gremlin that you will have to chase every time you mount a bit. I chose not to engage in that chase.
Both these techniques require some good measurement tools (calipers and test indicator w/mount). For runout, check John Saunders YouTube here.https://youtu.be/fhAASA_VFDo
Did another test cut in MDF…looks like the RU2075 is more .2430"/6.1722mm, but the 3/4" hole differences in Ø seem to indicate it’s .2460"/6.2484mm…just goes to show you that chasing the last 3 thousandths of an inch (about .0762mm) is silliness and gets you bogged down.
#2 intrigues me. Is there a better ER type collet people are buying as an aftermarket upgrade? Short of doing a spindle/VFD, I’m all about doing what’s necessary to squeeze everything out of this system.
If using a trim router you are subject to how ever much runout that the manufacturer decides is acceptable. You are also subject to how much force can be applied before it flexes. A $100 trim router built out of aluminum and plastic is built to a budget. An all metal spindle that has better, larger, and more bearings is going to be, if spec’d right, more accurate. It’s not the main reason why people upgrade to them but it is one reason.
Unfortunately the Makita does not have any alternatives for a better collet. Theirs and aftermarket ones I have seen are all of the split design.
I am curious as to what the measured diameter of your Whiteside bit is. Was it really 0.250? I understand you measured the widths of tool cut channels but back to the actual bit, what is its actual diameter?
I measured that long ago, and discarded it in favor of an actual cut (thinking that was far more accurate than trying to get the bit’s diameter measurement correct).
Using calipers and some blocks (to get rid of any tilt) I come up with .2455 inches/6.2357mm at the widest part of the flutes.
Looks like the .2460" was pretty accurate.
Interesting discussion on stock collet runout here. There, the author says he’s measured both a factory-new and several hundred hours-old Makita RT0107C collet’s runout…“Runout on both was around 0.0015″ (measured from the shank above the nut).”