Next issues... (Lead 1010 with RoutER11) After installing a modified High Z mod I was squaring my RoutER11 and noticed my spindle is out by almost 0.08mm (Sorry, my dial indicator is in mm). Before the modification I was getting more and more chatter so I replaced all the worn Wheels with new and added the second C beam to the X axes like the Lead 1515. While this greatly increased stability I still have some chatter and I believe it is because the RoutER11 seems to have a runout of 0.08mm (about three-thousandths. ) In the past I have ran my RoutER11 into the waste board a couple of times and snapped bits, could this knock the spindle out? I have been using it almost daily, usually only a hour or 2, but some days 6 to 8 hours straight. I don't think that would be over use by any means. Should I get a new RoutER11 or is there other options?
Looks closer to 0.15mm to me, but the easiest way to check the router is to just take off the nut and throw the indicator on the ER taper itself. Looks like all you're measuring here is the runout of a particular tool (or ER collet)
A lot of that I think is just bouncing around. When I carefully rotate the shaft by hand I get about a 0.08mm deflection. I have tried several different bits and changed collets and collet chucks. They all give me that 0.07 - 0.08mm runout on the bit. Some of them are high quality bits. But after you mentioned it I checked the inside taper, it shows about 0.03mm deflection, so just over one thousandths. I don't know the tolerance of the RoutER11 but I'm guessing it's not much better than this. Pic attached showing what I am chasing. Material HDPE, 0.22" thick, 2mm cutter, 8mm LOC, RoutER11 set on speed 2 (about 14K RPM), 1700mm/sec 2.794 DOC, Going to start playing with Feeds and speed and see what happens. Thanks
Yeah, could be bouncing. Around a thou sounds plausible. If it's not axially parallel with the spindle axis (ie. it's swirling instead of cranking) it could be a much larger error at the tool tip. Sometimes you can improve runout at the tool tip by clocking the collet and or tool shank. HDPE can be tricky to machine. It has high thermal expansion and can be grabby, so it likes high chiploads and low speeds, with coolant if possible. Basically the opposite of what hobbyist routers are set up to do. 2mm at nearly 4x depth, is probably neither rigid enough (especially with that 8mm LOC) nor has enough chip evacuation to deal with a stringy, gummy plastic without trying to bind up at the kind of chipload it really needs to produce a good surface finish. I'd try a test piece at various feeds and speeds (lower speeds, higher feeds, primarily) with a well-known excellent cutter with an odd number (for vibration stability) of very sharp edges, plenty of chip evacuation and a ton of rigidity to be able to run slowly, like a YG1 3-flute hi-polish Alu-Power. Something along those lines in 1/4" diameter. If that produces a significantly different finish, you have a tooling issue. If it doesn't, you have a spindle issue (or a machine rigidity issue). But you can probably get a pretty solid set of data points for about $20. If it works, and you actually need the smaller cutters (beyond trying to save material, which I've learned the hard way is a fool's errand), you could step down to the same type of tool in 1/8", though at that point the need for chip evacuation might override vibrational stability and you drop to two-flute. In general, I wouldn't be assuming it's a spindle problem when you're testing 2mm tooling, anyway. But spindle runout does cause a lot more issues with small tooling- far more flexing and uneven wear.
Use a bigger bit if you can, if not slow down 25% and use a finish pass full depth about 0.1mm. I find HDPE a joy to cut maybe I was just lucky. 2mm bit, is it single flute? Good luck Gary
Thanks for the suggestions, after running a few test on feeds and speed I was able to get a much smoother cut. The bit is a single flut and one of the primary reason I am using a 2mm is to avoid a bit change. The entire plate takes about 10 min to cut and I am cutting about 100 plates each week. The last thing I want to do is change the bit for each plate. Anyways, I found a lot of the chatter is only in the Y direction, I think this is from the push/pull on the router mount, which seems to be a week part of this set up. I already have a bracket in the works to stiffen the router mount. I also noticed something a bit more concerning. I found that my test pieces (in addition to more chatter) are trapezoidal in the Y direction only, see attached pic - exaggerating for clarity. The X direction is nice and square. At first I thought maybe it was some weird part geometry so I rotated the part 90 degree and cut it again, the trapezoidal cuts remained in the Y direction. Even though the drawing is exaggerated, the part is only 1/4" thick and it's noticeable. I'm at a loss on this one. EDIT: Update, I increased the chip load a bit more and it is much better but not completely gone - I'll see what happens when I get a support bracket on the router. (I think the bit is "pulling in" causing the router to skew) Also, cutting in the conventional direction is 10x worse.
Adding this helped, see pic. Utilizes two of the open holes in the gantry plat and the side holes in the router mount. That reduced the push/pull in the Y direction.
