M5 thread thru 2 inches deep HELPPPP!

[Ewindward]

Have a part here, calls for 9 M5 x 0.80 thru threaded holes and 4 M5 x 0.50 thru threaded holes. Part is 2 inches thick 6061 aluminum. I have looked high and low for a tap or threadmill to get this done and i've come up short. If anyone could point me in the right direction it would be greatly appreciated. This is a new customer and it would suck to tell him I cant get it done.

 

[Milland]

It's déjà vu all over again:

Tapping m6x1.0

You should be able to find standard M5 pulley or extension taps. The special pitch version will be trickier unless you can get a custom tap ground for your needs, and the time may not work out.

At worst, you can see if anyone like SCT is offering a single-row threadmill of sufficient length that you can spin grind the shank for additional clearance. It'll be a bit (a lot) floppy, but you're just cutting soft AL, take your time with multiple passes and you should be able to manage it.

 

[guest]

You'll probably have to find a nut tap. Normal pulley taps will not have long enough section of reduced shank.

The M5x.8 will be hard to source, the M5x.5 will be impossible. You'll have to have it made.

OSG, Balax, etc all will make custom taps. I have an M6x.35 in my desk I had to have made for a job a few years ago.

This is something like what you are looking for:

Machine Nut Taps, DIN 357, HSS-E, M 5 x 0.8 >> VOLKEL SHOP

edit: the M6 special I have was made by North American Tool. I'd give them a shout.

Home - North American Tool

If you have a tool post grinder or OD grinder you can also modify the shank on a standard extension tap.

You should do all this after you've kicked the engineer in the nuts though, on the off chance that the pain might get him to reconsider his stupid design...

 

[Ewindward]

Awesome, thanks guys. big help. Just before I had a chance to read this I stumbled across the nut taps. Customer is gonna love this quote with some custom tooling thrown in there. Do you happen to remember the lead time on that custom tap you got? Im going to give North American Tool a call in the morning.

 

[guest]

...Do you happen to remember the lead time on that custom tap you got? Im going to give North American Tool a call in the morning.

It's been a long time, but it seems like it was a couple weeks. Hope you don't have a bunch of those holes, glad it's your job not mine.

 

[Red James]

Both sizes/pitches are standard MSC taps, spiral pointed, and 70 mm OAL. Grind your own shank relief and tap without pecking.

 

[gustafson]

Quote it the way they want it and also the way it should be done, purchasing will appreciate your doing their engineering for them, or not.

There are approximately zero reasons for a 2 inch thread depth

Note the taps that can do the job are for reach, not actual depth

If they go for the mpre expensive route, you know they is idjits, act accordingly

 

[Shawnrs]

Have you thought about calling the customer and asking him/her does this tap need to be thru? It is possible they may only want the drill to do thru and they didn't specify an actually tap depth. At my place our young engineers have a tendency to making all taps thru when only the drill is needed thru.

 

[Ox]

or threadmill

Cough / choke!

Have a part here, calls for 9 M5 x 0.80 thru threaded holes and 4 M5 x 0.50 thru threaded holes. Part is 2 inches thick 6061 aluminum. I have looked high and low for a tap or threadmill to get this done and i've come up short. If anyone could point me in the right direction it would be greatly appreciated. This is a new customer and it would suck to tell him I cant get it done.

Sp Pt'd Pulley Tap?

May need to grind the shank down tho.

???

There are approximately zero reasons for a 2 inch thread depth

You don't know that.

Quote it the way they want it and also the way it should be done, purchasing will appreciate your doing their engineering for them, or not.

I would agree with that.



---------------------------

Think Snow Eh!
Ox

 

[gustafson]

You don't know that.








Ox

I am certain there are lots of reasons people think they need 2 inches of M5 thread depth, but I would ask you to provide any that make any sense, or are worth the tooling to do it.

 

[Ox]

Adjustment.

Not just fastening to.

Like maybe the hollow threaded bore of a straight shank collet holder/extension.

Odds are good that this app does NOT have any use for such, but from where you and me sit, we kan't be sure of that.


------------

Think Snow Eh!
Ox

 

[michiganbuck]

Oh the good old days when such a tap would be fudged up by a tool maker or a grinder hand with not even a thought it was out of ordinary...and not need buy a special tap that might cost $30
https://www.icscuttingtools.com/catalog/page_219.pdf

Quote Originally Posted by gustafson View Post
I am certain there are lots of reasons people think they need 2 inches of M5 thread depth, but I would ask you to provide any that make any sense, or are worth the tooling to do it.

Reason #1 the customer asked for it.

 

[gregormarwick]

I am certain there are lots of reasons people think they need 2 inches of M5 thread depth, but I would ask you to provide any that make any sense, or are worth the tooling to do it.

Almost certainly for an adjuster of some sort, especially given the non-standard fine pitch.

Engineers are not always idiots...

 

[Mechanola]

Fine pitch is also standardized. Do you mean regular?

A two-inch long M 5 thread is sign of stupidity. The mating surfaces are so big that the threads will need overly much attention in order to stay moveable, the right grease or oil or dry powder lubricant. I’d ask back whether a through bore will be acceptable with two threaded inserts.

 

[gregormarwick]

Fine pitch is also standardized. Do you mean regular?

I understand the metric thread system, I altered my wording because many on here do not - anyone unfamiliar with it will not know at first glance that 0.5mm is a fine pitch for an M5.

A two-inch long M 5 thread is sign of stupidity. The mating surfaces are so big that the threads will need overly much attention in order to stay moveable, the right grease or oil or dry powder lubricant. I’d ask back whether a through bore will be acceptable with two threaded inserts.

Only if it's also a 2" long screw, which is pretty unlikely...

I'm going to stick with my previous assertion - there are possible legitimate reasons for such a feature, and we have no particular grounds to claim that it's just "stupidity".

 

[jz79]

if you need "adjustability" with a M5 screw for length of even 40mm (50 minus some save thread engagement length), that is a noodle of aprox 4.5mm sticking 40mm out of something to adjust the other thing? I'm quite sure there is another way of getting it done

one thing that might be the reason - is would be if the adjustment screw couldn't be inserted from the side it is protruding out, and it had to be screwed in from the back side, hence the need for continuous thread, but then again - why not drill it 5.1mm to half depth and then you only need 25mm or so deep thread from the other side

and if something else needs to screw in that hole from the back side, well, tap an M6 thread there, the M5 will still go through, if someone drew up that 50mm continuous thread in that part, I will bet than M6 at the other side instead of M5 will make zero difference

and:

You should do all this after you've kicked the engineer in the nuts though, on the off chance that the pain might get him to reconsider his stupid design...

this is so sexist... to suggest only a man could come up with such a design

 

[michiganbuck]

OT:[ but I would ask you to provide any that make any sense, or are worth the tooling to do it.

Perhaps some device that needs a long dog-point screw, or a standard length one to hold/locate at 2” away. The under-cut tap is a catalog item, and any machinist hand can fudge one up in a half hour or so.

The screw need not be as long as the threaded hole to make function such a design.

A dog point screw going through a casting or machined part to hold/locate/stop something.

With not the full length thread it might be difficult to start or remove the screw..

The option of a short thread would/might require a costume screw with a precision shaft diameter and then a bored or reamed hole past the threaded area. Agree the special tap may only be a 35.00 tool but I figure any trip to the store or an odd purchase order is a $100+ wast of time.

M5-0.80 x 25 mm Dog Point Socket Set Screw, Alloy Steel, Thermal Black Oxide (Pkg of 100)

M5 x 0.80 x 6 MM Coarse Thread ISO 4028 / DIN 915 Class 45H Socket Set Screw Dog Point Alloy Steel Black Oxide - ASMC Industrial

Te-Co Dog Point Knurled Head Screw, Round, 3/8-16 Size, 2.9375"L, Steel 43811 | Zoro.com

The toolmaker is just required to make the part..

*Agree .200 (about) x 2" long seems an odd tap/thread...perhaps the engineer is the owners son in law...or it a government rocket part where money is no object and every ounce of weight is considered.
* Thread class is important and so would go with a measured drill and the loosest class allowed.
* 9 holes and 4 holes... this part does not seem like a dog point application..

 

[jz79]

The toolmaker is just required to make the part..

that might have been the case when designers had the actual machining experience, and still some things would go back to be redesigned after prototypes are made, not the case these days, someone designs some weird thing because he has learned how to CAD, then a drawing is made and that gets sent around job shops for quotes, I often have to educate people asking/sending parts to be anodized about the problem of blind holes they make in parts, about 80% of time it turns out they could be made through, and avoid possible rinsing problems, cross contamination of tanks and cosmetic dye defects when the acid leaches out and eats the dye next to the hole, they just didn't know the problem existed...

and you wonder why you lose machining jobs to China? maybe that is a 5$ part made in thousands that now with that special feature get quoted by machinist shop for 35$, because the quote has to include the special tooling, high probability of broken taps, associated time trying to solve that issue and so on, just because the managers at either side don't want to do their job and manage things, they just push the PO order and evaluate the quote, then decide - with this lead time we can just order them from China at 20% cost...

I agree that if this was standard practice, everyone would argue how to make something and nothing would get done, but this doesn't seem to be the case here, if feature like this was standard, there would be tooling for it, I actually have around 100mm long M5 and M6 taps that might work here (that were not designed to do things like discussed here, just that the length might allow it to be done), but I would still ask the customer to see the assembly and then, if I indeed see some moronic reason for this 10xD continuous thread, I would raise an issue, with solutions mind you!

the problem with tapping such long threads is that spirals might not do it, the chip will probably break and cause problems when trying to reverse out, pecking such a long thread might cause it to be oversize at entry, through hole taps may work, but then the hole is very long, and chips might pack up and cause tool breakage again

 

[Goff]

You could turn the end of a standard length form tap and silver solder it into any size extension you like.

 

[gustafson]

Adjustment, no

You use a longer screw, the added tapped depth is irrelevant

making tools costs money, if you are doodling around your garage you can silver solder tools up, but when you charge a shop rate you are not doing your customer a favor by doing so.