Hi. I need a little help with milling/machining threads.

[LightArmsJXF]

Hi all. It's been a long minute since I was on here, so long in fact that my old account name doesn't even show on the Member List any more, but recent life events got me to thinking about completing my old marker projects. As such I've just ordered a Carvera Air to get bits done. I know that it can't handle some things that I'd ultimately need another piece of machinery for but I'm hoping it'll get me started on CNC. I'll be using Fusion 360 for designing stuff as it's what I've been using for a while for 3D Printing.

Onto my problem. To begin with I was looking to make an autococker feedneck (1/2"-20 UNF thread) and an autococker barrel adapter (15/16"-20, Oversize GH-7). What I can't find is definitive information on how to actually achieve these threads using a CNC mill. I can't find a milling bit that's specifically for "15/16"-20, Oversize GH-7" and trying to find how to model either thread on Fusion 360 seems to completely baffle me (e.g. applying a 0.5"-20 thread to my model of a feedneck just makes the ID of the tube 1/2"). Not to mention that 15/16-20 doesn't even come up as an option as far as I can see. I've watched plenty of vids that showed me how milling threads looks, what kind of bits do what kind of cuts, etc., but I can't find the specific info nor the specific bits. Maybe there's a technique using a different sized milling bit to achieve the correct thread? I simply don't know what I'm missing here as I'm literally that new to CNC work. Can anyone help?

Further info:
I can buy an adapter to allow the use of 8mm shanks at the largest (standard included adapter allows 1/8" shanks) and other, smaller, adapters are available.
I'll be working primarily in 6061t6 and/or 6082t6 Aluminium.
Milling bits I'll be receiving with my machine are M3, M4 and M5 so if there's a way that I can use these to cut the above mentioned threads I'd really like to know.
Lastly, I'm UK based so getting UNF/UNC bits isn't as easy as someone US based. Although we use a combination of both Imperial and Metric over here, Metric is primarily what we use for machine things. (nuts, bolts, milling bits, etc.)

Thanks in advance.

[StaticShocked]

I would personally go with a single cutting-edge style thread mill like a Scientific Cutting Tools - Single Profile Thread Mill: 5/16-16 to 5/16-48, 16 to 48 TPI, Internal & External, 4 Flutes, Solid Carbide | MSC Direct. The single cutting edge will keep tool loads down and hopefully cut without chattering much. There are other design thread mills that can cut holes faster but require a rigid machine and larger shank sizes on the tools. Since you can only collet 8MM or smaller, the link is a 1/4" shank diameter and works on 16 to 48 pitch threads as small as 5/16". It should allow you to do any thread with that pitch larger than a 5/16 major diameter. As for using fusion 360 CAM for a thread mill, I will have to have someone else help with that. My CAM experience is with Inventor CAM which is similar family, but not the same so i would probably be lost.

However, if you want to manually program the thread mill in G-code, i can help with that and its not too bad to do. Just a 3-axis interpolation that keeps spiraling from the bottom out of the hole and you just program each pass to remove the material in stages until the pitch diameter of the thread is achieved (which you could measure with a good sample part and you wouldn't need an actual gauge unless you want to ensure you achieve the GH-7 thread specification). The GH-7 appears to be basic thread pitch diameter plus .0030" to plus .0035".

[flyweightnate]

Been there, done (some of) that - on a Nomad 3, so a similar size machine, in Fusion 360 no less.

Definitely, single-thread mill. Fusion 360 recognizes it natively if you import/create a proper tool. Just tell it what your major offset is from nominal modeled hole size, basically. Do several passes, maybe 0.003" stepover, as these little machines are underpowered. "Luocut" has usable threadmills on Amazon but are often out of stock; https://www.carbidetoolsource.com/si...m-thread-mills is a great US source but some of the shanks are a bit long for the work envelope available. Avoid coatings that have aluminum in them - stick to DLC, bright, or TiN (NOT AlTiN).

You'll need to get the adapter, as a threadmill typically has a shank diameter the same as the major of the milling point; most of mine are 6mm or 5/16" shank.

The sizing on the single-form mills is interesting - it tells you the smallest minor diameter it fits in (e.g. 5/16"); get the biggest you can use so it's more rigid. Then it tells you the range of pitches (e.g. 20-56 tpi). Use it on a 16tpi thread, it can't reach the bottom (unless you cut your crests off); use it on a 64tpi thread, the root will be too flat (since it's not "sharp" enough). But the software handles the pitch of the cut, whether it does 20tpi or 32tpi.

This is more flexible than the ones you'll see that have 3 (or more) forms - which can only be used at that pitch, so all three threads line up every time. Sure, it'll cut 3x faster. But you need a lot more tools.

As far as using your metric bits... 20tpi is 1.27mm pitch; I doubt that's in your inventory. Just get a new threadmill. Although the M5 is pretty close to 10-32... for a short hole you can possibly just adjust your diameter to get something that is wrong, but works.

[LightArmsJXF]

Thanks for the help/info!

I've started looking for suitable bits now while I'm waiting on the Carvera Air to arrive. If I'm gonna do this I'm at least gonna aim to do it right straight out of the box. So far I'm having difficulty finding TiN coated as opposed to AlTiN/TiAlN. Would "Bright" be "No coating"? I'm finding "No Coating" and something called TC50 coating for Aluminium. I'm also seeing GuTong Cupreous Coating and Black coating (with no further explanation) and Nano-Coating for Steel on my search through AliExpress. eBay UK is coming up with a load of AlTiN variants from all over the world. I'm still doing a non-usual suspects sites search to see if I can find a UK supplier that I can order directly from.

[flyweightnate]

Bright/ uncoated would work well.
AlTiN might load up, but if you're taking light cuts, it'll work. Just beware that if it gets hot, you're in trouble.

[LightArmsJXF]

Okie dokie. Light cuts and I'll try to hook up my compressor for "air assist" to help blow chips out of the way. I'm sure it won't do much but maybe that'll help cool things a little too. 👍

[LightArmsJXF]

It's been a while but I've got another CNC query.

I'm still in the "Design" phase of things and I'm wondering how much clearance I can go down to when designing parts to fit into one another. I want there to be "Zero Gap" between parts once screwed into place but I don't want parts to have to be "squeezed into position" in order to get them to fit, if you know what I mean? I've been seeing vids where you can't even see the join/split lines until it's disassembled but no information about tolerances are attached to the descriptions or even in the comments. I know I'm just a beginner in CNC with a Carvera Air so I'm not expecting to be able to achieve that level of seamlessness (which I'm assuming is like SSS Rank milling ability) but the closer I can get to it the happier I'll be, y'know? Is 0.1mm/0.0035in going to be gappy or would it not give enough clearance? How close is going to be enough?

edit:
I've only done 2 little test projects so far, a jig to hold a Spyder upper receiver and a plate to hold a small vice, and they've turned out ok. Using Fusion 360 to set up the G-Code for the Carvera Air seems to have been a mistake as the cuts between sides is inconsistent, creating weird milling artifacts and increasing job time with all the extra movements. Getting consistent Z-axis heights also seems to be problematic when using Fusion 360. Generally the Air would do all the homing (as per instructions to align materials) then the Fusion 360 G-Code would set the top of the material as Z=0 and start milling at twice the height. Once I'd switched to Makera CAM to set up things all the aforementioned issues seemed to disappear. Unfortunately I'd only did that after I'd gotten halfway though the 2nd of my little test projects and I'm not going to buy more material to correct either as they can still be used as intended even though they're a tiny bit wrong.

[flyweightnate]

Look at ISO Limits and Fits tables. Typically, an H-class fit (H7/h6) gives a slide together fit with very little wiggle room; moving the shaft part to a k6 or higher would turn it into a light press fit.

The problem is, lots of these fits will be .0004" tolerance (give or take) at the size we're working with, and these inexpensive machines can't cut that. So plan on 0.001" clearance at the minimum, and if something has to be tighter, cut undersized holes and ream to size then use precision pins for assembly.

If you know your tolerance is .0035" (a thick sheet of paper), just design around it.


Regarding Fusion - when you do your setups in the CAM tab, it asks where you want your zero to be. Paying attention will make the G-code start in the right spot.

[LightArmsJXF]

Thanks for the Fusion zero bit. Any idea what's causing the extra movements that cause milling artefacts?

[flyweightnate]

Look at lead-in and lead-out, and check what your stock settings are - constraining box, constraining cylinder, or previous setup/ previous solid. If you tell it you're milling a rectangle, it'll cut air if it thinks that air is part of your bar stock.

[LightArmsJXF]

Cool. Thanks for all the info. I'll look into everything as well as double check what the manufacturer says the machine is capable of. I looked it up when I'd received the machine but can't remember jack now. lol

[Chemical-x.....ahain]

ive been looking at the carvera systems and nearly bought one. id really like to know how it works out for you and what your plans are with it.

[flyweightnate]

For a reference, the Nomad 3 has been bulletproof from a programming and motion perspective, but 150 W spindle power is extremely limiting. (0.010" depth of cut at 40ipm with a 0.060" stepover is running it pretty hard. Finish pass needs to be closer to 0.002" DOC.)

The Shapeoko HDM has caught my eye, as it has 10x the power and is specifically designed for light machining in aluminum and brass. No tool changer, though.

Power matters.

[LightArmsJXF]

ive been looking at the carvera systems and nearly bought one. id really like to know how it works out for you and what your plans are with it.

To me it seems really good but I haven't really cut much material so far (I've only done 2 test bits to make sure it works) so I'm not sure if I've got a good enough perspective on it to be able to recommend it. Also, I don't have any prior experience with milling (CNC or not) so I really couldn't say if the Carvera Air is better than any other machine. Aside from the obvious difficulties in learning something new, it does seem fairly easy to use but, that being said, I'm side-stepping from 3D printing and not starting from absolute zero so I'm not sure if that could be a factor/consideration.

As for my plan? What plan? I guess my plan is, ultimately, to use it to finish off all of my marker builds (36 at last count) that I'd accumulated between when I started in Paintball 2004 to about 2012(ish) when I last packed everything away. It's mainly Spyders, Tippmanns and Cockers. Aside from that I've also got a lot of RC models that need custom parts.