demonx Posted December 9, 2014 Report Share Posted December 9, 2014 I've bought the end mills and have a bit of an idea, but before I go breaking any in trials I thought I'd ask how others are going about using these half millimeter bits successfully? How deep pass? 0.25mm? What's an average without breaking? How slow feed speed? Drill or ramp? I can see both methods would put different strain on such a fine bit, the ramp would flex it, but then the drill would apply pressure when the x or y movement begins Curious to hear your experiences. Thanks. Quote Link to comment Share on other sites More sharing options...
DC Ross Posted December 14, 2014 Report Share Posted December 14, 2014 First thing, be aware with that narrow of a bit, you'll get into trouble trying to seat any normal-sized frets. I learned that even for frets with a .021" tang, a .023" bit is iffy unless you're using softer woods. I ended up with a neck that had so much back-bow that it looked like the St. Louis Arch. Depending on the type of wood, I ramp at about 15-30 in/min, taking .025" per pass. As with everything, start conservatively and you should be fine. Quote Link to comment Share on other sites More sharing options...
demonx Posted December 14, 2014 Author Report Share Posted December 14, 2014 First thing, be aware with that narrow of a bit, you'll get into trouble trying to seat any normal-sized frets. I learned that even for frets with a .021" tang, a .023" bit is iffy unless you're using softer woods. The endmills I've purchased are .56mm, which is virtually the same size as the stew Mac saw blade I've been using for the last couple years (.58mm) and the same size as the stewmac fretsaw that is now as blunt as a butter knife. The fretwire I use has a tang width of .508mm and I've never had an issue with frets being too tight. Im also going to make the assumption that slotting with the endmill with several passes won't br exactly .56mm and it'll be very close to the .58mm anyway. Quote Link to comment Share on other sites More sharing options...
demonx Posted December 14, 2014 Author Report Share Posted December 14, 2014 Depending on the type of wood, I ramp at about 15-30 in/min, taking .025" per pass. As with everything, start conservatively and you should be fine.Out of curiosity, have you broken many bits? Your ramp speed is a touch faster than I was planning, you're around 380mm and I was thinking of going around 300mm to play it safe, but your depth of cut surprises me I've been led to believe that it's best to try cut no deeper than half the router bits width,you're cutting at its full width, which in guessing would put a lot of stress on such a small bit. Like I said in the op, I haven't used these small bits yet, Im just painting a picture in my head before I do. I know that Ive broke enough of the tiny stewmac bits in my dremel to have given up using them, so I want to play it safe on the cnc! Quote Link to comment Share on other sites More sharing options...
DC Ross Posted December 14, 2014 Report Share Posted December 14, 2014 I used to use the StewMac thin kerf table saw blade, which was advertised as .023" (.58mm). That worked fine, which is why I started with the .023" endmill. They definitely didn't give similarly wide slots. The wobble of the blade and the tighter tolerances of the endmill combined to make much smaller slots on the CNC. I've taken .030" passes with a .023" endmill in ebony (remember, this is a ramping op, so that max depth of cut (DOC) is only at the very end of the path), but that's as far as I'm willing to push it. It's really not as bad as it sounds, it comes out to 0.00075" per tooth (normally I shoot for .001"/tooth on bigger bits). I broke two bits while I was figuring out what speed/feed rates worked best. They're cheap, so I wasn't too upset; besides, education is worth the price Quote Link to comment Share on other sites More sharing options...
demonx Posted December 14, 2014 Author Report Share Posted December 14, 2014 Interesting, I thought the spinning bit would have the opposite effect. What is the tang width on the wire you're using as that could make all the difference? Quote Link to comment Share on other sites More sharing options...
DC Ross Posted December 14, 2014 Report Share Posted December 14, 2014 I've been using the stainless wire from Allied lately, so .019" or .021" (the barbs measure .031" and .037" respectively). If you're trying to shove a .021" tang with a .037" barb into a .022" slot in ebony, you're gonna have a bad time Some advice I wish I were given when starting out w/ the CNC: Tight tolerances are good, but a "perfect fit" needs a bit of room. Quote Link to comment Share on other sites More sharing options...
demonx Posted December 15, 2014 Author Report Share Posted December 15, 2014 I'm glad I asked, as the tangs you're using are wider than mine, not heaps wider, but enough to make just make that bit of difference. I'll still run some test cuts to be safe though. I've stumbled across something else that is a bigger priority to work out at the moment so the fret slots will be on hold for a week. Turns out the jigs I made to do the neck wont work how I planned, so I have to rethink and make them again. I allowed for the scarf joint angle etc, but I didn't allow for the crease to be in a different place when I flip the neck, in that error, it also creates other issues with varying depth of neck blank with different heel angles etc, so I need to come up with a new plan to flip the neck on the bench. Quote Link to comment Share on other sites More sharing options...
DC Ross Posted December 17, 2014 Report Share Posted December 17, 2014 As with everything, ymmv. This is just my experience, and what I've found to work for me. I'm curious how you're doing scarf joints on the cnc. Are you actually cutting the scarf on the machine, or is the scarfed headstock glued up beforehand? Quote Link to comment Share on other sites More sharing options...
demonx Posted December 18, 2014 Author Report Share Posted December 18, 2014 I'm curious how you're doing scarf joints on the cnc. Are you actually cutting the scarf on the machine, or is the scarfed headstock glued up beforehand? Making the blank beforehand as per usual to put under the CNC. Quote Link to comment Share on other sites More sharing options...
Prostheta Posted December 21, 2014 Report Share Posted December 21, 2014 If you're not planning on making blind fret slots, cut them on the CNC and then open them out with a saw. Sounds like it is defeating the object, but nonetheless maintains the accuracy of CNC. Quote Link to comment Share on other sites More sharing options...
demonx Posted December 21, 2014 Author Report Share Posted December 21, 2014 If you're not planning on making blind fret slots, cut them on the CNC and then open them out with a saw. Sounds like it is defeating the object, but nonetheless maintains the accuracy of CNC. Being that I can fret an entire board accurately with my slotting jig in around a minute, the only reason I'd be even looking at doing it on the CNC is for blind slots as you call them, where the slot doesn't break out the side of the board and the ends aren't visable, or down the track for fanned frets. Quote Link to comment Share on other sites More sharing options...
Prostheta Posted December 22, 2014 Report Share Posted December 22, 2014 That's what I figured. Other than basic "suck and it and see" the slots probably shouldn't be milled as slots. DC Ross is on the money I think. Good to hear you sharing progress and experience within the learning curve. Quote Link to comment Share on other sites More sharing options...
verhoevenc Posted July 25, 2016 Report Share Posted July 25, 2016 Uhhhh.... @DC Ross, where are you getting "cheap" fret slot cutters? I'm learning and just snapped one and kissed $20 (precisebits) goodbye! I'm not seeing them any cheaper on places like HarveyTool.com either. This may be the most frustrating CNC learning step yet... Chris Quote Link to comment Share on other sites More sharing options...
DC Ross Posted July 26, 2016 Report Share Posted July 26, 2016 Ha, yeah, the PreciseBits are the cheap ones. Well, cheaper than the $80 1/2" spiral bits that I use for most ops that I need to replace every 6 months I haven't broken a slotting bit in quite a while, using those numbers I quoted above. What are your feed, speed, and depth of cut? Quote Link to comment Share on other sites More sharing options...
verhoevenc Posted July 26, 2016 Report Share Posted July 26, 2016 I was going at .3333in/sec and .030" DOC. I think the issue was trying to get MeshCAM to actually do this radiused slot operation... which I'm having a heck of a time trying to make it do... seems to be the only limitation I've found with this 3D CAM package so far. There's no "follow this line in 3D" function. So I've have to model the slots in full 3D... and it still just isn't grasping the concept... Granted, I also haven't played with ramping at all... should probably learn a bit about that. Chris Quote Link to comment Share on other sites More sharing options...
curtisa Posted July 26, 2016 Report Share Posted July 26, 2016 You might find it easier to manually edit the NC file to make each slot follow a radius. Should be fairly easy to identify each linear slot and convert it to an arc around the Y axis. 0.33" per sec is 20" per min. Maybe that's asking a bit much for some bits? I've done 3 boards with a 0.023" twin flute Kyocera bit (eBay in packs of 10, not expensive), 12"/min, ramping to 0.012" at each end of the slot without any issues. Could probably go harder with experimentation, but haven't tried it yet. I would think that making a direct plunge into material to a depth of 0.03" and suddenly wrenching the bit sideways to begin the slotting operation would be asking for trouble with small bits, even at low feedrates. The gentler approach of ramping into the cut is ideal for this kind of work. Quote Link to comment Share on other sites More sharing options...
DC Ross Posted July 26, 2016 Report Share Posted July 26, 2016 Sorry I can't help with your MeshCAM issues, but I'd be surprised if there's no "Groove" or "Slot" operation that allows you to choose a 3D path for it to follow... I've modified my approach somewhat since that post from Dec. 2014. I now use a 2-flute .027" diameter (.025" for non-ebony) carbide bit, at 20,000 rpm, going 30IPM, and cutting .01" deep passes, and it poses no problems at all. Quote Link to comment Share on other sites More sharing options...
CMStewart Posted October 16, 2022 Report Share Posted October 16, 2022 On 7/26/2016 at 3:21 PM, DC Ross said: Sorry I can't help with your MeshCAM issues, but I'd be surprised if there's no "Groove" or "Slot" operation that allows you to choose a 3D path for it to follow... I've modified my approach somewhat since that post from Dec. 2014. I now use a 2-flute .027" diameter (.025" for non-ebony) carbide bit, at 20,000 rpm, going 30IPM, and cutting .01" deep passes, and it poses no problems at all. Hey DC. I am looking to use the Jescar 47095 fretwire (0.021" tang with 0.035" barbs), and was wondering which bits you would recommend for that size? I see you use 0.027", but I wasn't clear what size fretwire you use. And what manufacturer do you recommend for the bits? I appreciate the help a ton! - Colby Quote Link to comment Share on other sites More sharing options...
Prostheta Posted October 16, 2022 Report Share Posted October 16, 2022 Zombie thread! I would say that it depends on your CNC. If your spindle has significant runout or there is flex in the cutter, that 0,027" cutter might end up cutting a much wider slot than you want. A hair over the tang width is fine, so 0,027" would be correct in theory. In reality, I would consider having one or two finer cutters in case your spindle does want to cut wider than the endmill actually is. You'll probably find that if this is the case, you'll have a larger incidence of breakage from asymmetrical load. Do tests and establish what you're able to achieve, and that should help you develop a working strategy. Quote Link to comment Share on other sites More sharing options...
CMStewart Posted October 16, 2022 Report Share Posted October 16, 2022 11 hours ago, Prostheta said: Zombie thread! I would say that it depends on your CNC. If your spindle has significant runout or there is flex in the cutter, that 0,027" cutter might end up cutting a much wider slot than you want. A hair over the tang width is fine, so 0,027" would be correct in theory. In reality, I would consider having one or two finer cutters in case your spindle does want to cut wider than the endmill actually is. You'll probably find that if this is the case, you'll have a larger incidence of breakage from asymmetrical load. Do tests and establish what you're able to achieve, and that should help you develop a working strategy. That sounds like some very reasonable tips. I really appreciate it!! Quote Link to comment Share on other sites More sharing options...
Prostheta Posted October 16, 2022 Report Share Posted October 16, 2022 No worries. Start a thread documenting your process, @ me in and start a discussion. It both helps others understand the process and also provides an opportunity for others to weigh in and help you through to the result you need. Quote Link to comment Share on other sites More sharing options...
CMStewart Posted October 16, 2022 Report Share Posted October 16, 2022 3 hours ago, Prostheta said: No worries. Start a thread documenting your process, @ me in and start a discussion. It both helps others understand the process and also provides an opportunity for others to weigh in and help you through to the result you need. Will do. I just have one last quick question. Harvey tool has a lot of options for long flute micro end mills, but they all seem to be 3-flute. Is there a downside to 3 flutes vs 2 flutes? Quote Link to comment Share on other sites More sharing options...
Prostheta Posted October 26, 2022 Report Share Posted October 26, 2022 Sorry for the slow response. Only just saw this in my notifications. It's a question of the material you're cutting and the size of the end mill. Single flute endmills evacuate the most material since the flute gullet will be larger, however there is plenty of chance of asymmetrical tool pressure within a cut, plus the cutting is less efficient in terms of cuts by distance. Three flute endmills will be the most even in tool pressure (to a point) but cannot evacuate larger chips as efficiently, leading to slower feed or spindle speed being required, plus a greater degree of recutting waste and heat in the cut. Sizewise, smaller endmills are less precisely made, especially less than 0,5mm diameter. For the price that most endmills cost, it's worth getting in a few examples of each option so that you can develop a feel for the differences. Your CNC's capabilities, the material properties and milling approach may favour one over another. I don't believe that a single answer would be appropriate one way or another, mostly because it doesn't help develop a strong basis of knowledge. FWIW, my last fingerboard inlaying and slotting job used 0,5mm single flute mills which I drove way too conservatively. Quote Link to comment Share on other sites More sharing options...
Recommended Posts
Join the conversation
You can post now and register later. If you have an account, sign in now to post with your account.