Printable View
Could do with some advice on single point threading in a CNC mill.
.
Is there a good place to buy tools in the Uk?
.
I have a range of sizes of thread I'll need to cut. One for example is approx 80mm diameter internal thread, others down to 30-40mm. Will I need different sized tools to get the right thread form in the base of the cut etc?
It used to me hugely expensive to buy gear cutters until some bod started selling full sets of Chinese tooling on Bay of Fleas.
The thread cutters look so flimsy I would be wary of practicing with an expensive one unless I had a lot of iron and huge floods of coolant to back it up :black_eyed:
But are the Chinese parts bringing the price down yet? I don't know :beer:
A few, but they won't be cheap. How much are you willing to spend?
To get a thread with a correct thread form, you'll need a different tool for each pitch, however unless you really need to meet the official spec, then you can get away with only one or two tools.
You will also need some way to gauge your finished thread to ensure it complies with the recognized standard.
Regards
Mike
The ones I've seen in the US seem to be around £100. Pretty pricey but if I only need one then I guess I can live with it. If I need several its another matter clearly and I'll need to rethink.
I'd prefer an indexable one so I could replace tips rather than the whole thing!
For that size range you can use an ISCAR MGCH 06 or MGCH 08 with a thread cutting insert, the inserts are available in the two most common thread angles.
Tony at Jurassic Tools has a few in stock at an excellent price - http://www.jurassictools.com/store/s...re&phrase=mgch
My only connection with Jurassic tools is as a very satisfied customer,
- Nick
If you're happy spending that kind of money, another suggestion to go along with Nick's, is the simmill PX range. I've got one for grooving, but they do various different inserts, including threading.
Cutwel supply them - http://www.cutwel.co.uk/milling-tool...milling-tools/
Although I notice they're not showing as having the holders in stock.
Thanks Nick, one of those would be perfect. Just need to find a source for the inserts. So far can only see Iscar selling them direct at £170 for 10! Will email Tony and ask if he has/can get singles.
PM me if you struggle to find a supplier, I may be able to help.Quote:
Originally Posted by Lloyd Barnes
Will do, thank-you. Tony has already responded to say he can't get them. I'll have a look at the Simmills as well this week. Thanks for the leads, much appreciated. :thumsup:Quote:
Originally Posted by magicniner
Robin,Quote:
Originally Posted by Robin Hewitt
It's not in the least bit scary, I've never broken a cutter and I've cut internal threads down to M3.
Provided you run at the recommended rpm you are fine, air + mist lube is sufficient to clear chips and lube the tool and the lovely part is that if you need to or if you are prototyping you can take multiple passes until you get where you need to be ;-)
Regards,
Nick
When I first saw this thread, I wasn't sure whether it was referring to tools for screwcutting (in effect, using the CNC mill as a kind of vertical axis screwcutting lathe) which would need a spindle encoder to synchronise the spindle rotation with XYZ movement but would be appropriate for a single-point tool, or for thread milling where the cutter revolves at higher speed and only needs XYZ synchronisation, which should be achievable on any reasonable CNC mill. In the course of doing a little bit of research to try to understand the differences myself I stumbled across this, which is a very nicely written document from Sandvik that talks about these different operations and has a lot of useful information (well, if you start out ignorant, anyway...).
Still not sure whether a single-point tool could be used for thread milling (although I don't see why not) even if it wouldn't have the "full hole-depth thread in one rotation" capability of the "proper" cutters as used for production.
Hi Neale, plenty of vids online about using single point tools for thread milling but I'm also learning. I'm trying to explore cost effective tooling for it for my hobby use and also get my head around how many tools you would need and what the limitations are. I've been surprised at the pricing of them given they are nothing more complex than any other indexable cutter but I guess there are a lot less sold.
I've cut threads on my old manual lathe but its a slow process and if I can switch to a CnC mill then so much the better. Got to be one or the other with 75mm diameter threads, I'm not buying a tap that big!
They're used all the time. No different from any other milling cutter, as it's rare more than one cutting edge is in contact anyway. The main drawback (or could be classed as advantage depending on how you want to look at it), is a lower feed rate as you only have one tooth doing the work. If you have the horsepower available along with the rigidity to handle it, a multi-thread/tooth thread mill is far quicker, as you can do the whole thread height in a single circular pass.Quote:
Originally Posted by Neale
Off course, tapping is usually quickest, but then you're into needing enough torque to handle the tap, having the capability to handle the required synchronisation, and a tap being available in the correct size.
That way you will also need the budget to buy a cutter for each pitch you wish to cut.Quote:
Originally Posted by m_c
I have cutters capable of full thread depth in a single pass for frequent jobs but a single point cutter can give you a lot of flexibility for one-off jobs and you don't end up with a drawer full of "once-used" threadmills.
Something to put on the shopping list - slightly further down than the CNC vertical mill conversion...
The reasoning is I have 4 nuts to make. 75mm diameter thread, can you imagine the cost of a 75mm diameter tap!! I would use it twice and in fact need 2 (2 nuts LH thread, 2 RH).
Single point threading seems a very sensible option as I'll be able to use it again for other large but different threads. I'd only need to buy a LH and a RH insert. That's assumes I can find one of course!
Do you need two different inserts? Surely the only difference between cutting LH and RH threads is the movement in the Z axis?
That's correct, thread milling tools cut left or right handed threads.Quote:
Originally Posted by Neale
That was my logic too but the inserts still seem to be available in left or right handed versions which makes no sense to me.
I need to spend some time browsing the links provided earlier in this thread at the weekend.
You mean for the tools that can be used both for turning & milling like the one I linked to?Quote:
Originally Posted by Lloyd Barnes
It's because you do need left and right hand inserts for some turning operations, I always thread away from a shoulder and from the bottom of a hole outwards and it's handy to have both LH & RH threading inserts.
The LH/RH in that respect is to do with the physical position of the cutting edge, not the type of thread.
There are holders/inserts available for turning that require angled shims, to ensure the insert is cutting at the correct angle for the required diameter, and ensure the correct thread form is produced. Larger diameters for a given pitch, have a less angled thread, so to ensure a 100% correct thread form, the cutter has to be angled to compensate for the thread angle, however if you need that level of accuracy in your threads, you probably won't even be considering thread milling.
If you need a full thread right to the bottom of a flat bottomed blind hole you probably won't even be considering anything other than thread milling.Quote:
Originally Posted by m_c
If you need a thread with specific start/finish points for alignment of two mating parts you probably won't even be considering anything other than thread milling.
If you want one tool in your drawer that will get you a working part covering a huge range of threads you probably won't even be considering anything other than thread milling.
Job specific threadmills can produce perfectly accurate thread forms and full forms too, not partial, what you have to understand is that the form of the tooth on the tool differs not just for different thread angles but also for different diameters of tool, outside threads versus inside threads and different ranges of Major Diameter, knowing these the manufacturer designs a cutter profile which when swept through the work and following a helical path generates the correct thread form.
Single point inserted thread milling tools are a great thing to have around, they are specifically produced because they allow a wider range of threads to be cut, albeit with reduced accuracy, but in this situation it is clearly incumbent on the programmer/operator to ensure the resulting thread is close enough to spec to be acceptable.
If you need a higher level of accuracy in your threads you probably won't even be considering not buying the correct threadmill for the job. ;-)
- Nick
Is that to go with the 90 degree hole the designer wants drilled at the bottom of the blind hole?Quote:
Originally Posted by magicniner
Rigid tapping? Plus any good lathe will able to control the exact thread start point.Quote:
If you need a thread with specific start/finish points for alignment of two mating parts you probably won't even be considering anything other than thread milling.
To give you a comparison to think about, why do gear hobs have to be offset at an angle from what they're cutting so accurately?Quote:
If you want one tool in your drawer that will get you a working part covering a huge range of threads you probably won't even be considering anything other than thread milling
Job specific threadmills can produce perfectly accurate thread forms and full forms too, not partial, what you have to understand is that the form of the tooth on the tool differs not just for different thread angles but also for different diameters of tool, outside threads versus inside threads and different ranges of Major Diameter, knowing these the manufacturer designs a cutter profile which when swept through the work and following a helical path generates the correct thread form.
Single point inserted thread milling tools are a great thing to have around, they are specifically produced because they allow a wider range of threads to be cut, albeit with reduced accuracy, but in this situation it is clearly incumbent on the programmer/operator to ensure the resulting thread is close enough to spec to be acceptable.
If you need a higher level of accuracy in your threads you probably won't even be considering not buying the correct threadmill for the job. ;-)
You could cut a gear keeping everything perfectly inline, and you'd still get a gear with the correct number of teeth, but would the tooth form be correct?
For over 99.9% of uses, a thread mill will produce a perfectly acceptable thread. I was just highlighting where it might not be acceptable, but the fact is, very few people would be able to test the difference. For those of us posting on here, we're far more likely to have problems with a milled thread not being perfectly round, let alone having problems with the correct thread form.
If your mill doesn't cut circles that are round one assumes you'd realise thread milling isn't for you but if you haven't done any thread milling and so haven't read around the subject to a reasonable extent then this-
http://www.productionmachining.com/a...g-makes-sense-
Might help with understanding Thread Milling and it's capabilities :D
Note. Better Finish, Lower Power Requirement and Fuller Thread Profile than tapping ;-)
- Nick
It's an Apples to Oranges comparison because angling the hob relative to the work lets you use one hob for a variety of gear sizes and pitch angles, even racks, it's not relevant to thread milling because Thread Mills are made Inside/Outside specific and for a set pitch and range of Major Diameters, these are all but 3 of mine (the other 3 live in holders by the mill), each is for a specific job -Quote:
Originally Posted by m_c
Attachment 21249
- Nick