Spiralock Taps

[JB7280]

I have a part, 17-4PH H1150 that calls for 8-32 Spiralock taps.  Some through, some blind.  The print specifically calls out NASM 85353/1 so the Emuge Self-Lock taps won't work here.  Everything I have read points to the Stanley brand taps being junk.  That being said, would you guys suggest form or cut taps?  I have used Emuge, 8-32 self-lock form taps in the same material and was relatively successful.  Not sure if I'd have the same luck with the Stanley taps.

[#Rekd™]

I had a job to do that required those and agree their taps suck....They eventually sold me a decent one...

[Matthew Hajicek - Singularity]

I threadmill all my 17-4.  Just need the gauge to size it in.

[JB7280]

9 minutes ago, Matthew Hajicek - Conventus said:

I threadmill all my 17-4.  Just need the gauge to size it in.

I considered threadmilling it, but this part has 40 holes in it.  My experience is minimal compared to you guys, but it seems like threadmilling would be very time consuming for that many holes.

[Colin Gilchrist]

What's not to love about a material that work-hardens when you so much as glance in its direction...?

1 minute ago, JB7280 said:

I considered threadmilling it, but this part has 40 holes in it.  My experience is minimal compared to you guys, but it seems like threadmilling would be very time consuming for that many holes.

Only with single-point Threadmilling Tools.

If you get a multi-tooth threadmill, it is a couple of passes per hole, with a single "vertical helical move", plus the lead in-out.

[Matthew Hajicek - Singularity]

2 minutes ago, JB7280 said:

I considered threadmilling it, but this part has 40 holes in it.  My experience is minimal compared to you guys, but it seems like threadmilling would be very time consuming for that many holes.

Threadmilling does take longer than a nice, dialed-in tapping routine, but it's much faster and easier to get going in difficult materials.  Consider how much time you'd lose if you bust off a tap in the 39th hole.  If you're running hundreds of the parts, it's probably worth getting a tool rep in to guide you in setting up a tap; if it's just one, just threadmill it and call it done.  Worst case scenario you bust a threadmill, you just pull it out and replace it and keep going.  Only way to lose the part is to overcut.

[JB7280]

1 hour ago, Matthew Hajicek - Conventus said:

Threadmilling does take longer than a nice, dialed-in tapping routine, but it's much faster and easier to get going in difficult materials.  Consider how much time you'd lose if you bust off a tap in the 39th hole.  If you're running hundreds of the parts, it's probably worth getting a tool rep in to guide you in setting up a tap; if it's just one, just threadmill it and call it done.  Worst case scenario you bust a threadmill, you just pull it out and replace it and keep going.  Only way to lose the part is to overcut.

This is a large quantity of parts.  Unfortunately I think I'll have to stick with the taps for now.  Emuge only makes self-lock threadmills in metric sizes, and we won't be able to get the Stanley thread mills quickly enough.  Not to mention I can't even find a listing on Stanley's website for the threadmills to see what is available!!

 

1 hour ago, Colin Gilchrist said:

What's not to love about a material that work-hardens when you so much as glance in its direction...?

Only with single-point Threadmilling Tools.

If you get a multi-tooth threadmill, it is a couple of passes per hole, with a single "vertical helical move", plus the lead in-out.

Thanks for the suggestion.  I'm going to try to start the job with taps, just to get going, then I'll get with some reps and see if we can get multitooth thread mills.

[Colin Gilchrist]

31 minutes ago, JB7280 said:

This is a large quantity of parts.  Unfortunately I think I'll have to stick with the taps for now.  Emuge only makes self-lock threadmills in metric sizes, and we won't be able to get the Stanley thread mills quickly enough.  Not to mention I can't even find a listing on Stanley's website for the threadmills to see what is available!!

 

Thanks for the suggestion.  I'm going to try to start the job with taps, just to get going, then I'll get with some reps and see if we can get multitooth thread mills.

Try Carmex.

http://www.carmexusa.com/products/TM00/TM00 S000.aspx

They even have a very handy "NC Code Generator", where you plug in your parameters, and it spits out a Subprogram for cutting the threads. I believe they are "left-handed" tools, meant to cut with M04, so you can cut "top-down", instead of "bottom-up".

 

[#Rekd™]

53 minutes ago, JB7280 said:

Thanks for the suggestion.  I'm going to try to start the job with taps, just to get going, then I'll get with some reps and see if we can get multitooth thread mills.

I found their Ni P PVD taps worked the best, the first taps they sent I was lucky to get 10 holes out of a tap.

 

[JB7280]

17 hours ago, Colin Gilchrist said:

Try Carmex.

http://www.carmexusa.com/products/TM00/TM00 S000.aspx

They even have a very handy "NC Code Generator", where you plug in your parameters, and it spits out a Subprogram for cutting the threads. I believe they are "left-handed" tools, meant to cut with M04, so you can cut "top-down", instead of "bottom-up".

 

They don't have anything with the spiralock thread profile though, do they?  I didn't see one on their site.

17 hours ago, #Rekd™ said:

I found their Ni P PVD taps worked the best, the first taps they sent I was lucky to get 10 holes out of a tap.

 

Those are from Stanley or Emuge?

[#Rekd™]

3 hours ago, JB7280 said:

Those are from Stanley or Emuge?

Directly from Spiralock at the time. 

[JB7280]

Thanks, I'll look into that.  That must be the ones they call "High Performance"

[Newbeeee™]

Spriralock form is not uniform flank angle though? It has the 30degree kick making one side of the V different to the other?

So isn't it proprietary so only the Spiralock manufacturer taps/gauges etc are available from them?

 

[JB7280]

6 hours ago, Newbeeee™ said:

Spriralock form is not uniform flank angle though? It has the 30degree kick making one side of the V different to the other?

So isn't it proprietary so only the Spiralock manufacturer taps/gauges etc are available from them?

 

Yes, however emuge has their own, which achieves the same function, with just a slightly different thread profile.  We have used them in the past on different jobs calling for spiralocks.  Some prints use terminology where we can squeak it by.  Other times we were just in a bind and had to.  I just don't want to be the one to use them, and have a large order get kicked back on my decision.

[Newbeeee™]

16 hours ago, JB7280 said:

Yes, however emuge has their own, which achieves the same function, with just a slightly different thread profile.  

Not being an azz...but as you state it's a different thread profile.

As the spiralock are designed to do just that - lock, the thread angle is paramount for their locking data.

If you're the design authority or using this for in-house fixturing etc, no biggie. If it's for a customer product...IMHO you have to be a brave person to deviate like this...

[JB7280]

On 3/29/2021 at 4:53 AM, Newbeeee™ said:

Not being an azz...but as you state it's a different thread profile.

As the spiralock are designed to do just that - lock, the thread angle is paramount for their locking data.

If you're the design authority or using this for in-house fixturing etc, no biggie. If it's for a customer product...IMHO you have to be a brave person to deviate like this...

Agreed.  Owner likes to take risks though.  60% of the time it works every time.  

 

[FROZEN]

I think you should consider the cost of a part to cycle time. If you're ok with losing a part because of a broken tap than tap a way. Taps do and will break. I prefer thread milling to tapping for the only other reason. If the thread mill breaks, you replace the tool, blow out damaged hole and rerun thread mill. The part should be savable. If you are going to tap??? I would use a form tap and drill ream to remove any work hardening. So, pilot drill leaving about .015 to .030 per side. 

[Rstewart]

I. Hate. Reamers. 

[Colin Gilchrist]

59 minutes ago, Rstewart said:

I. Hate. Reamers. 

Why? Who are you using? 

I've had great success with Hannibal carbide reamers.

[crazy^millman]

13 hours ago, Rstewart said:

I. Hate. Reamers. 

You must have never done tool and die work, injection molds or precision tooling. All we ever seemed to use was reamers.

Or Better yet you have why you don't like them.

[JB7280]

On 3/30/2021 at 8:22 PM, Colin Gilchrist said:

Why? Who are you using? 

I've had great success with Hannibal carbide reamers.

Reamers always felt like black magic for me.  Mfr speeds/feeds never seem to be right. Our tolerances are often -0/+.0002" which is often less than the tolerance of the reamer.  I believe it was cncappsjames that told me he generally starts a reamer at 1200/10 and I've had pretty good luck with that.  I generally use garr carbide reamers, or harvey for small sizes. 

[Colin Gilchrist]

32 minutes ago, JB7280 said:

Reamers always felt like black magic for me.  Mfr speeds/feeds never seem to be right. Our tolerances are often -0/+.0002" which is often less than the tolerance of the reamer.  I believe it was cncappsjames that told me he generally starts a reamer at 1200/10 and I've had pretty good luck with that.  I generally use garr carbide reamers, or harvey for small sizes. 

Yes, generally you want high feed-per-tooth values for a reamer, combined with low SFM. For super tight tolerances like you mentioned, I would order double the number of tools, and hand-guage the sizes to find tools which are on the low end of the tolerance band. You might consider PCD or Diamond tipped, since it will be an expensive tool, with plus or minus about 50 millionths. 

Also, a great technique I've seen is to use a combination Boring Endmill with Start Chamfer, which is sized to give a perfectly 'on-center' start hole for the reamer.

On a Yasda, I would just circle interpolate the hole with the right tool, since typical roundness measures about 1.8 Microns. You just need to cut a semi-finish pass, and adjust the tool wear compensation with the Probe. But not everyone has access to such great equipment. I was machining a set of spherical surfaces for a lever, and the tolerance was -0.0001 +0.0000 on the 0.3125 sphere diameter. Once I got the cutting process dialed in, we were holding about -20 to +20 millionths, from nominal (0.31245 Nominal), part-to-part. 

[Rstewart]

On 3/31/2021 at 6:59 AM, crazy^millman said:

You must have never done tool and die work, injection molds or precision tooling. All we ever seemed to use was reamers.

Or Better yet you have why you don't like them.

I work in a mostly one-off, or less than say 10 parts per run facility.  If the holes aren't extreme L x D I usually interpolate where I can.  I'm also talking about standard made in USA  HSS chucking reamers.  I cannot get one to cut On size (± .0005" ) without dicking with it forever.

If I need to make a lotta holes that are required to be Round and tighter tolerance, I will invest in a nice carbide application specific reamer...

[JB7280]

15 hours ago, Colin Gilchrist said:

Yes, generally you want high feed-per-tooth values for a reamer, combined with low SFM. For super tight tolerances like you mentioned, I would order double the number of tools, and hand-guage the sizes to find tools which are on the low end of the tolerance band. You might consider PCD or Diamond tipped, since it will be an expensive tool, with plus or minus about 50 millionths. 

Also, a great technique I've seen is to use a combination Boring Endmill with Start Chamfer, which is sized to give a perfectly 'on-center' start hole for the reamer.

On a Yasda, I would just circle interpolate the hole with the right tool, since typical roundness measures about 1.8 Microns. You just need to cut a semi-finish pass, and adjust the tool wear compensation with the Probe. But not everyone has access to such great equipment. I was machining a set of spherical surfaces for a lever, and the tolerance was -0.0001 +0.0000 on the 0.3125 sphere diameter. Once I got the cutting process dialed in, we were holding about -20 to +20 millionths, from nominal (0.31245 Nominal), part-to-part. 

We have a Yasda px30i and that's a damn impressive machine.  I haven't been able to do any jobs on it yet though.

[Colin Gilchrist]

32 minutes ago, JB7280 said:

We have a Yasda px30i and that's a damn impressive machine.  I haven't been able to do any jobs on it yet though.

Awesome, the PX30i is a great machine. Where area are you located in?

At Methods, we've had a PX30i at our Precision Center in Acton, MA for a while, but recently started installing a 2nd demo machine in Sudbury. So now I'll have access to 2 different machines for customer demos and test cutting purposes.