Posted previously and had some good suggestions. New job, same issue. LM 2.5, SLB. Rough cut for 2.5D model no problem. Raster finishing cut (about 12 hours total) with Sienci 1/4", 1/16", Ball nose. Previously suggested slippage due to pressure on upcut bit (makes sense. I noticed deepening ramp when cutting more material, especially vertical). Also suggested changing collet. First was Makita, next 2 Sienci Precision Collets. Have tried my āstandardā tightening and āextra-forceā. Have verified that cutter has slipped looking at side ārampā of job plus when return to Home position. Am resetting Z, cutting for about 20 minutes, then repeating. Have verified F&S with Sienci. Suggestions? Possibly replace cutter?
I probably donāt have anything you havenāt tried but what the heck!
Iām sure youāve cleaned the collet but I think I found some stuff inside the shaft before so itās worth sticking a pipe brush in there to check.
Iāve heard of oil from the factory on the bit but that most likely only applies if the bit is new. I often clean the collet and nut just by unscrewing it all and tapping it out but maybe it needs a more thorough cleaning. Iām not sure of the best way to do that though. I just searched and I think Iāll watch this video, maybe Iāll learn something.
The other problem I had once was putting the bit too far into the collet, so far that it bottomed out, or maybe it topped out depending on how you look at it. As the collet nut is tightened it pushes the collet into the shaft. If the bit hits inside the shaft it can prevent it from moving up and squeezing the bit enough. That happened with a long bit and tall stock. I was trying to eek out some more Z travel and it didnāt work out for me.
EDIT: Just remembered that I had some chatter going on with that long bit but I donāt know which came first the bit slip or the chatter. Seems like a chicken and egg problem to me, each probably making the other worse. I know you verified F&S but if all else fails maybe slow down a bit? Iām not great at feeds and speeds though, I just do what sounds okay to me.
Depth of cut could be an issue as well. Iāve heard things like you can cut as deep as the bit is wide but Iāve never even come close to that. For me Iām more like a 1/3rd the width for the depth. Shallow cuts let me keep the feed rate up which is better for the bit than going slow and deep. My Mk1 is not as stiff as your Mk 2.5 though so maybe you can do a bit more than me. I think some of these ārules of thumbā Iāve heard as well as most chipload charts are for big boy machines and not applicable to my LM Mk1.
2 Likes
Thank you. Have tapped, cleaned the collet/nut, multiple times, and used shop vac on shaft. Checked with mirror - clean.
Have tried minor differences on cutter shaft insertion (never full bottom). Have done some gentle sanding of shaft with 120 G paper.
Using 5% stepover for the cutter setting. Nice and smooth cut, butā¦
Had same problem several months ago on a different job, which I cut at 2/3 the rated feed of the cutter, so speed does not seem to be an issue. If I lower the feed, the cut time will go from 12 hours to ???
Have router set at 25K rpm, as per Sienci, and have tried going a bit higher rpm to reduce pressure on the cutter flutes.
Using W Oak, so should not be an issue with hardness, such as with ebony.
My guess at this time is that it is either the Makita router or the cutter is just too aggressive on the flutes.
I figured you had probably tried my suggestions but itās not a problem. I can type okay! On another note how did I know when I watched a video that I found when searching how to get oil of from a collet that he was going to use oil to clean the collet 
Again Iāve heard people complain about the oil but that doesnāt mean itās a problem per say. When we are having trouble and grasping at straws we tend to blame whatever we find, no? I was kinda thinking as I wrote about the oil in my first response āWhat about those machines that mill metal with what I assume is oil flying around the whole cutting chamber?ā.
Unfortunately Iām out of ideas to help but I wish you all the best with your project, sir.
1 Like
More infoā¦
Have contacted Sienci - requested measurements of my 3 collets and shaft of cutter - all at 0. 249. Sienci has asked for a video of my ātightening techniqueā. OK - do not claim perfection, but I have been doing this for 6 decades or soā¦ always willing to learn.
My Brother (Mech Eng), bless his soul, suggested two further options: bluing the cutter shaft, and applying some lock-thread compound. Will wait for Sienci response and will KYP.
Concerned about expensive wood spoilage in all this experimentation, butā¦ Need a totally dependable depth cut for my projects!
Quick update.
My tightening technique: I tighten the collet manually, with the router shaft stop, then, use two wrenches, squeeze, and then give a good tug at the end. Takes a good heave to undo it after. Sienci not supportive of the tug at the end and suggested longer wrenches. I am concerned re overtightening. Spoke with two separate techās at Makita, who support my technique and are completely against longer wrenches. Have requested a discussion with Sienci engineer. Will KYP.
Update. After interchanges with Sienci, and an experienced machinist, seems clear that downforce of cutter exceeds holding power of collet(s) when cutter engages with vertical (1/2") on the pattern.. I have some projects planned at 1" depth. Sienci has kindly offered to replace the router, butā¦not yet. Mak collet designed for ātrim routingā, not for CNC, according to Makita, and makes sense, butā¦ many CNC suppliers use them, so, why am I having this issue? Next steps: try same project again, with reduced F&S - means my time babysitting will go up, butā¦ Perhaps upgrade to spindle? with ER collet? Suggestions welcome.
Hi retiree,
Well, at least there is a solution to try. I must say, the thought of engaging half an inch and even a whole one at once, gives me movies at the backside of my eye lids that involve fire, explosions and me running in slo mo while the neighbourhood cop shooting rounds into my shed, just to make sure whatever beast is in there roaring does not come out.
I would not dare take such agressive passes. I know, I know, Iām a wee over cautious, but there are times when my machine engages some AzobĆ© and starts to fibrate while pushing a cmp round a curve, I donāt like to be in the same room as my mill. And those are only 3 or 4mm deep passes max.
Iāve seen bits slip out due to fibration, and those arc passes accross the grain of these hard wooden boards are the exact spots I imagine that to happen. Engaging half an inch of that wood, with a longmill and a lonely blue hand router.
Something would snap and it would not be the wood. And if not the machine, it would be me.
I like your extreme approuch though and I would love to have some footage of your machine doing these passes. The sound, the feeling, the shaking of the walls.
@Retiree A question: When you are taking 1/2" passes, what is your ramp length? Tks.
Usual preface, Iām with PreciseBits. So while I try to only post general information take everything I say with the understanding that I have a bias.
Hopefully this doesnāt get me in troubleā¦
The main issue with all of the Makita trim routers and their clones is the collet design itself. The ONLY area that can do anything to grip the tool is the tapered section:
Taken from Sienciās store page, so hopefully not an issue. If you look at this print you only have 4mm that is producing force to hold the tool. If the taper angles arenāt a perfect match, thereās surface issue in the 4mm section in either the collet or the router, etc. Itās not going to be able to make much use of even that. On top of this, most of all the Makita collets available are only slit from one direction. This means that they are very likely to pinch at the slit end and not get full compression or contact.
That being said it sounds like you have a poor armature or wear in the taper section of your router (as you have the same issue with multiple collets). To get the most out of it, use something like a penetrating oil to clean the outside of the collet and the inside of the router taper. Wipe them clean but leave a layer of the oil. Then as much as I HATE saying this, use acetone followed by as high percentage of alcohol you can find to clean the inside bore of the collet. That will let you transfer more force by getting better compression and less friction loss to the outside of the collet and increase friction inside against the tool.
Reducing the feed wonāt help much. At 5% stepover you are deep into chip thinning. So your chipload even at the max 4000mm/m and 25KRPM would be 0.003"/0.076mm (Feed / RPM / Flutes). However, with the 5% stepover that shrinks to 0.0013"/0.033mm. Thatās into grinding territory and below what most starting points in most woods, even for most micro tools. If anything, reducing the feed will produce extra heat that will probably make the situation worse.
Reducing the pass depth or skipping the 1/4" tool could help as those will reduce the cubic material removed per flute per rev more than your chipload is going to.
One last thing. Donāt take sandpaper to the shank of a tool for this (or in general). It MIGHT help a couple of times. But the grooves you put in the shank of the tool will eat the collet making the situation worse over time.
Hope thatās useful. Let me know if thereās something I can help with.
2 Likes
Thank you all for you comments and suggestions. I have much to think about, when I get the time. Basic info:
Cutting area about 8"W x 6"H
Raster Rough cut bottom to top: 1/4" cutter, 2 passes, to 0.4598 depth, Chip load 0.0014. Lots of expensive sawdust. No issues.
Raster Finishing cut, bottom to top: the Sienci cutter I have indicated. Program says 0.4998" depth, at a chipload of 0.0016 (far less than Sienci rating). It starts at that depth on the bottom flat section, and then starts to get deeper as it encounters the vertical of the model. Parts of the vertical are abrupt, as one would expect, and I do hear more loading, but not much, IMO. I also note that at the top, once it has finished the verticals, the flat cut stays at a steady depth, but it is far deeper than 0.4998", of course. I did see it deepening, but decided to let it run to the end. No earthquakes in W Ottawaā¦lol
I am convinced that the issue is the weak holding power of the Makita collet, as indicated by TDA. Will try to understand the information provided and will KYP. Have another project in mind, much larger, at almost a 1" depth model, and do not want to attempt until after I get this resolved. Thank you all again.
1 Like
Hi John. Your explanations make sense to me, and thank you for practical suggestions (no, I will NOT get you into trouble, LOL). I will try the chemical route next time, but as you indicate, if same issue with 3 collets, seems they are not the issue. Interesting that one person āsolvedā the issue by using crazy-glue.
Question re F&S - if chipload is calculated based on full length of flutes (is this correct?), then it seems my approach is producing flour instead of chips? Have been ādetuningā F&S to help address the issue, but it seems this is not right approach?
Thank you.
Not Problem.
More worried about Sienci not liking my opinion of the router. But I appreciate it.
So without going too far into a rabbit holeā¦ The main issues with any method that does this is that itās adding something to the interface between the collet and the router. Pretty much without exception that will increase runout. Runout is how much the bit spins off the center axis of the router. The runout will not only make your cuts inaccurate. But, it will also change your chipload in uncontrollable ways.
No, chipload is the width of the chip made per flute per rotation. Or another way to think of it is itās the amount the tool is moving āforwardā per flute per rotation. What I was talking about above is that that width gets narrower if you are not cutting at least 50% if the tool diamter. A picture is probably easier to explain this with:
This is as if we could look down āthroughā the tool as itās cutting. The red would be how far the tool would move āforwardā for a single flute and therefor what will become the chip. The smaller you get from 50% the smaller that chip width (chipload) actually is.
Chipload itself is probably the most important factor in milling. Thereās minimums in each material and tool geometry to actually ācutā. Going less than that will grind material out of the way which generates more heat and forces. Chipload is also one of the main factors that determine the cutting forces applied to the tool and machine.
It can beā¦ But you already have such a small chipload here that itās already not ideal. The main things that will determine cutting forces other than tool geometry are the chipload, stepover (or tool diameter if slotting), and pass depth. Together those remove a certain amount of material and everything has to resist those forces. So an inaccurate but easy way of thinking of it is that if you go half as deep but twice as fast (chipload/feed), the forces are approximately the same. Itās not completely true as things like the tool helix (flute twist) change it, or at least the force direction.
The other non-obvious thing you have to consider in this is the flute engagement time. A very simple way of thinking of this is "how long is it between the time the first edge of the tool hit the wood to when that flute stops cutting. In tools with a helix that number goes up with pass depth (like for like). In this case that could be important as itās how ālongā each āpullā of the tool is.
Let me know if thereā something I can help with or you want expanded on.
3 Likes
I was thinking about this not too long ago. Thanks for confirming my suspicion that it is an inferior design compared to an ER collet. Funny thing is my little 3018 Chinese machine used ER collets albeit on a really small under powered spindle. Thatās the only thing that was better with that machine. I understand why Makitaās are use so often for hobby mills. Nice spindles add a lot to the price tag.
On my LongMill MK1 this is the approach that Iāve taken. I think compromises have to be made when dealing with hobby level machines. Going shallow but faster seemed like the only way I could even approach the recommended chiploads.
Thanks for your informative posts!
1 Like
Thanks for diagram and explanation of chipload. I checked via my VectricPro S/W, and regardless of tool geometry, the chipload was identical if F&S and no. of flutes the same. Good, however, seems more a theoretical parameter as opposed to a practical one? If one does a deeper cut, the width of the chip would be the same (assume same F&S), but the chip would be longer, indicating more force. Parallel for me is a cut on a table saw - same F&S, but different depth of cut requires very different force to maintain F&S. If want to maintain equal force for different depth cuts, must adjust the Feed (do not have a variable speed motor). Back to CNC - tool suppliers indicate F&S, DOC, S/O, etc., and I have been using these parameters (actually, have been reducing F by 20-30% - me being cautious as a newbie - perhaps wrong approach?). There are also vertical and horizontal force differences based on geometry/type of tool and amount of material engagement/pass (varying in my case). Consensus is that my Makita router spindle/collet is the problem - I have contacted Sienci. One suggestion is to make several passes for the finishing cut. Have not found how to do this in Vectric, but can always set the Z-Home physically to achieve this. Probably some experimentation coming upā¦ Fascinating stuff.
@Retiree If by āfinishingā you mean that 3D finishing toolpath, there is no way in Vectric to do that in more than one pass. You can, however, do multiple roughing toolpaths with ever smaller mills.
Thanks for confirming the Vectric capabilities/limitations. Makes sense that one can reduce force on finishing cut by roughing with smaller diameter cutter. Much to considerā¦
Update. Tried a different cutter on the uncompleted (and ruined) current job: IDC Tapered ball nose, 10 Ā°, 0.045"r. Ran it for 1/2 hr, at their rated F&S, andā¦the bit slowly slipped, though not as fast as the Sienci. Confirms the Makita router shaft seems to be the issue.
Sorry, Mondayās donāt typically give me much spare time.
This is a pet peeve of mine so take this for what it is. A lot of āRecommended Chiploadsā are complete BS. Some of them are the absolute limit of what a new tool can do on an industrial machine, with perfect material, in a perfect environment. Some are extremely conservative to try to account for every negative variable that will leave a lot on the table for cycle, finish, and tool life. Some will have a range, use a formula, be pulled out of thin air, etc.
The best thing to do is understand some basics of machining and the tools you are using. Then test on YOUR machine, in YOUR material, in YOUR environment.
There are some baseline things or rules of thumb that can be applied. But thereās no way that even if someone tested a specific tool on the same model of CNC and router that you could walk away with anything but a starting point or base range. The differences in things like runout, wood variability, hold down methods, and even humidity will alter that range . Then add tool geometry or tolerances differences and those error bars can get massive.
In general though most of the numbers you will see are either formula based (e.g. X% of diameter for chipload at X surface speed), or pulled from a fairly high end test machine. The first could go either way depending on what they are shooting for (marketing/safety). The second pretty much puts you in a position where if you donāt have a machine of similar capability, itās going to be overly aggressive.
In this specific case what we are dealing with is cutting forces. Both from the perspective of slip resistance and deflection (bending). Both of those are tied functionally cubic material removed per flute per rotation (per flute MRR). So the more material being removed the higher the forces. Those may not be in the same directions depending on tool geometry, but the forces have to go somewhere. "Cheating "the cutting forces the easiest way is to take shallower passes. Find a good cut at a really low pass depth, then scale the pass depth to the forces and tolerances you can handle. Should probably add some margin for dulling and variability. But you will end up with a much more stable and useful number. One potential exception to this is that itās a lot easier on the tool not to slot. So thereās some advantage to testing something like small pockets with a 50% stepover, depending on your situation.
Yeah, all the Vectric software shows is the very basic chipload number (Feed / RPM / flutes). It wonāt show you the corrected amount if youāre below 50% stepover.
More or less and probably an easy way to think about it. It may be the the PEAK force is the same. But itās maintained for longer. You can also get into a situation where you are engaging multiple flutes at a time. Thatās probably outside the scope of this discussion though.
See above reply to Michael. Short version, easiest way to ācheatā is pass depth. The problem is if you get too low on the chipload (feed), you are not actually cutting but grinding. Or how I like to put it āturning the end-mill into glorified sandpaperā.
Iām not really sure thereās a lot they can do there. All of these type of routers have been the best of bad options. CNC is also āoff labelā use for them (barring the Kobalt ER11 router that had a very short life). Arguably the DeWalt 611 was better overall, especially from a collet stand point. However, it doesnāt have the RPM range and there was a LARGE issue with supply for a while that made a lot switch to the Makita.
Let me know if thereās something I can help with.
2 Likes
Thank you for detailed, logical explanations. So, I could/should do the finishing cut (as per the above pic), in letās say 2 passes. The first one would be cutting air for most of the time and cutting the upper half of the butterfly model. Would reduce the forces on the cutter, IMO. The second pass would be the real finishing cut at programmed depth. On the flat base (walnut), the cut is .04" (love the turning mill into glorified sandpaper", then abrupt force when encounter edge of model, but forces lower since upper half of model already cut. Seems logical, however, how to determine 2 passes, 3,ā¦? Am learning a lot.