I bought the Hog from IDC a couple of months ago and finally tried it today. I was using .5” DOC at 18krpm and 80ipm to clear out a pocket for a box. It was a test piece before attempting the real one.
The bit made short work of the clearing, but there was way more squealing than I usually hear. Am I being too conservative or too aggressive with my C3D router.
In his videos Garrett takes even bigger bites with this thing.
Has anyone else here tried it? My intent was to then come back with a different bit to cleanup the floor and walls. Although I have to say it left a pretty decent surface on the floor of the pocket.
On the practice piece it worked great. On the real piece the bit was slipping out of the collet so that the cut looked more like a 3D rouging pass instead of a pocket.
Well, that finished but then I had bit slipping issues with another portion of the project while using a .25” extended reach upcut and a .125” DOC. I will rework to have a pocket instead of a slot in that case although it doubles the time.
I am going to toss all my collets and order new ones although some of these are not old at all. I don’t know the ER-11 collets and the spindle reduce this tendency.
It seems I run hot and cold on this. I went through a phase 6 months ago and since then with my cleaning procedure everything was great until today. I can baby things but it’s frustrating to continually have to worry about this.
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.
Hey Cullen, I won’t belabor the points made in the other thread. But with collets that aren’t gripping like that I think it’s adding too many variables to really narrow down much. For those that want it I’m referencing this thread (Link). I will add though that when you have either sprung collet or a out of spec router bore the runout becomes very variable from change to change or even during the cut from cutting forces.
I would check the nut for damage. However, from memory, it doesn’t have a second taper on the nut side. So outside of something really significant inside the nut, or the thread being screwed up I don’t think it would change much.
Hopefully this doesn’t get me in trouble. The collet system for the Makita leaves a lot to be desired. The only section of that collet that does anything for clamping or aligning is the tapered section. It’s extremely short for the angle. It’s one of the reasons that we never developed collets for it. It was too inconsistent to get the numbers we were looking for even with perfect collets and bores. We learned this one that hard way with Bosch Colts…
I don’t know of a spec for the Makita in terms of torque. If I was to take a crack at it I would try around an ER11 with a standard nut (18ft-lb/24Nm for 3-7mm). Taper angle is different though and no second taper nut side. That would lead to less accuracy and clamping force. However, the max is for preventing damage and distortion. So that’s probably close.
The screaming bit could be related to the bit slipping. However, in my opinion without specialized tool geometry 18K is too fast for a 1/4" bit. That’s around 1200SFM I usually try to stick to 800-1000SFM in most domestic hardwoods without aggressive tool geometries. That aside, you’re only cutting around a 0.0015" chipload. That’s below what I’d consider a minimum for 1/4" tooling in that size range. However, with runout some of those flutes are cutting even less material. That too can lead to a squealing/screaming tool.
Hope that’s useful. Let me know if there’s something I can help with.
More or less. It’s a standard chip-breaker/corncob/threaded bit (not to be confused with a chip-breaker router from the PCB world). Although, there’s a few ways to make them. I’m assuming in this case that they are just offsetting the crosscuts to reduce engagement time of the flutes and therefore deflection. There is a way to make them that uses different offsets so each flute is only picking up percentage of a normal fluted endmill. However, that is typically used for composites and harder material not a roughing tool.
The bar is higher for ER. There are still poor spindles out there but in general unless you are really unlucky you going to be a lot better off. Regardless of that you have much more margin in the clamping force with ER. You can get in just as much trouble buying cheap collets though. But there are a lot of decent ones all the way to individually measured high precision ones from multiple sources.
I’ve tried the IDC bits as well. I’ve ended up finding a much less expensive solution on Amazon.
.5" depth/cut at 80ipm with our trim routers is demanding, especially on hardwoods. I rough out projects several times/week with the same bits and have found .3" depth/cut at 100ipm to be loud enough. The bit makes a heck of a racket. No comment on the speeds and depth this youtuber films.
I tossed out a collet the other day because my bits were creeping out at these speeds/feeds. The makita arbor, collet, nut and bit can really heat up changing the torque and grip you set before running these cuts. It would be nice it these trim routers had ER style collets, perhaps they would do away with creep. I don’t think the designers had our CNC demands in mind and you can only tighen so much without risking damage to threads and cheap wrenches.
