Does anyone have a source, in Canada, for a precision balanced and low TIR ER16A 19 mm thread collet nut?
Has anyone been able to purchase such a collet nut from Sienci (itās not shown in their āshopā web page) and do they have any specs on their nuts (if they have them at all)
1 Like
Yeah youāre down there in watchmaker machinery, or machinery making machinery. Iām coming from the cabinet/millwork field to the custom jet interiors industry. Couple or ten thou is close enough. Here in hobby land, we sand it to fit, paint it to match. But I am interested to know if the torque is consistent, particularly between different diameter shanks.
I donāt know of a seller in Canada.
However, thereās no TIR spec for nuts. The only measurement spec for a nut is balance. The empirical version will typically be listed as under ISO 1940-1 spec and written as GX at/for X RPM. The lower the āGā at the same RPM or the higher the RPM for the same āGā value the better the balance. e.g. āG2.5 at 18,000 RPMā, isnāt as good as āG2.5 at 20,000 RPMā.
That being said the other thing that can effect the TIR is the angle ground into the nut. No spec I know of for that though.
Yeah, that high end guitars, PCB, cues, drones, etc.
My point above is less about the dimensional accuracy and more about what itās doing to slip/chipload and therefore feed, finish, and cutting forces. Wonāt belabor the point though.
You do a good job with that IMO. That and you always say your with PreciseBits so people know where your coming from. I for one have always found your posts to be very informative. Itās nice to see empirical data on how things affect a CNC machine because I drive by the seat of my pants!
2 Likes
Thanks, I appreciate it. My goal is always to provide data that can hopefully be used to get better results or understand the āwhyā of something. Even with the āby the seat of my pantsā style I think itās useful to know some of those whys to compensate with when things go sideways.
Let me know if thereās something I can help with.
2 Likes
@TDA Iāll add to @_Michael comment and say that I, too, always appreciate your thoughtful and educational posts.
2 Likes
Given the excellent comments re what can be realistically expected from āmachiningā wood, I would like to clarify my earlier inquiry about a precision collet nut ā¦ I intend to (eventually) machine aluminum and would rather pay a higher price once then to have to buy other stuff later on. This of course applies to both collets and collet nuts.
Edit to add: this entire thread has been very interesting !!!
2 Likes
I appreciate it.
I guess I will belabor the point a bit as the larger point Iām trying to make is being missed.
This is NOT about dimensional accuracy. Itās about like for like are you changing your runout and therefore your chipload.
If you are cranking down on these like in the example I gave you are picking up extra runout. That turns into variable feeds which will not only effect the cutting forces but your cut quality.
Another way to put this. However much runout you add gets added to your max chipload/feed and subtracted from your minimum. If you have the margin for it youāre fineā¦ You could have used that for your feed and gotten better tool life but it didnāt kill you. That might not be true for all cases. It might push you out of that range.
Letās do a super quick simple example. Letās say that I have a material that needs no less than 0.002" chipload, and I get a good cut at 0.004" chipload, and screw the material up at over 0.006" chipload. Letās say this is running a 2 flute at 20KRPM so we can do these in IPM instead of chipload. Those would be 80IPM minimum, 160IPM for a good cut, and 240IPM max.
So in the above example if I have no runout I can run those numbers 160IPM to 240IPM for a good cut. With 0.001" runout I have to run a minimum of 120IPM instead of 80IPM to account for the short cutting flute from runout, my good cut ārangeā is now only 200IPMā¦ no range at all as I have to account for the short flute getting 0.001" less chipload and the large cutting flute is getting 0.001" more. If I have any more runout than this I canāt keep both flutes of the cutter in the good cutting range at all.
This also changes things like how deep you can cut as the forces increase with cubic material removed per flute. So you might also have to lower your pass deep to account for more runout.
The issue on the other side is that if you are much too low in torque youāre potentially not getting enough clamping forces to hold the tool through the cut. To give a rough idea Pioneer states that on an 1/2" ER16 with a standard nut at MAX torque, it provides 50 ft/lbs of radial slip resistance (Link page 11). If you are halving the diameter of that shank you are not going to have even close to that much. Letās be forgiving and say half. Now if we apply letās say half the the nut torque, we will be forgiving again and say we have half of the remaining amount. So thatās 50 / 2 / 2 or 12.5ft/lbs. So if we put more than 12.5 lbs into the side of that tool in trying to cut, it will slip. Will you need more than that?
NONE of this is about dimensional accuracy or even the amount of margin you have to have for things like moisture content in wood changing your cutting forces. It that not controlling these leads to variables that can screw up your cut or tooling.
Iām not sure anyone can help you much if you are specifically looking for good quality nuts from a decent manufacture with a hex head an 19x1 thread. I donāt know of any regardless of location. If you are not trying to use something like the RapidChange, than just get a good mini nut and castle wrench. You will have MANY choices.
Keep in mind that if you are planning to machine metal you need to have VERY rigid hold down in addition to minimal runout (most metal shops are 0.0002" max, a bit more forgiving in aluminum). At least to actually ācutā it. If you are willing to sacrifice cut quality, and throw tool life out the window, you can āgrindā a part out. Itās more or less using the tool as glorified sand paper.
Hopefully this help make some more sense out of what I meantā¦ I hope at leastā¦
2 Likes
Again, very interesting ! Who knew (I certainly didnāt). A lot of information to digest!
@TDA I apologize, John, for taking this way, way off topic. Iāve edited my really irrelevant post and deleted entirely my moderately irrelevant post.
Carry on. 
??? Probably more my fault than anyone else. Iām pretty sure I ended up dragging us from type of nut ā RapidChange issues ā why those issues matter. They were all connected in the thread, as I believe your post was as well.
As long as @JPlocher is okay with it Iām good. Seem that it was worthwhile info to some in the threadā¦ Unless Iāve assumed too much and you were apologizing to the other Johnā¦
@TDA No, I was apoligizing to you. Although, now that you mention it, Iāll make it a sort of global apology to everyone who has posted.
@gwilki, I saw nothing that was irrelevant and I wish people would stop editing/deleting things at a drop of the hat. I now feel that I am missing something 
@Jens I will respectfully disagree. The topic was started by @JPlocher with the subject line dealing with collet nuts.
@TDA provided a lot of good information on that subject with very technical input.
I went off on a tangent that had nothing at all to do with collet nuts, their specs and how they should be handled.
Others joined in, but always asking questions or adding information about collets and collet nuts.
So, with respect, I did not delete my input āat the drop of a hatā. My input was not on topic. You am not missing anything by its absence. 
I just learned that one can see the original post. I had a look at your original post and while you are correct that things went off topic a bit, I still think that your thoughts were valuable to me and likely to others.
Anyway, live goes on ā¦
Leaving this here to amplify the good points @TDA (the other other John?) madeā¦
I finally had enough and I had to check runout on my Altmill spindle. Barring any measuring errors (I donāt do this every day), I had 0.0003" runout on a 1/8 collet that was installed from a previous job. Cleaning up all mating collet surfaces and that was reduced to ānon measurableā (on an indicator that reads 0.0001/division). A 1/4 Sienci collet showed runout at 0.0003 and an aftermarket 1/2 collet showed 0.001 runout.
I went searching for a quality collet and landed on the KBC Tools site (Canadian). For $42 CAD you get a quality 1/8" ER16 collet rated at 0.0002" TIR.
The moral of the story - the Sienci collets are indeed nice, aftermarket can be crap, quality collets are dear, working with wood probably makes a quality collet a luxury that is hard to justify but milling Aluminum would probably be better done with a quality collet.
(I realized I sent this only to one person and not the forumā¦)
Peace, all.
I appreciate all the posts here, on and off topic! I learned a lot, and hope to continue learning more from all of you. Thank you, other John; I recognize the passion and love of topic you put in your writing, and the rest of you for the thoughtful responses. Please keep the discussion going, it will be fine, no matter where we end up.
The other other John
Good to see some numbers. Were these at the face, the 4x DIN standard, or some other position? Make sure you record these too. Youāll be able to see when you need new ones from this as collets and nuts are consumables. Although, worst case I guess itās recorded hereā¦
Just depends on how much margin you have to eat to hit tolerance and finish. In my opinion itās not worth the variability and lost performance vs tooling and material.
Appreciate it.
Iām keeping my eye out as much as possible. Feel free to @ or PM me if I miss something or thereās another thread I could help with (poison with text walls).