PCNC 770 Tapping capability

[Fortune7]

One of the first jobs on my new 770 is to make some Tee-nuts for the table, with metric M12 threads to suit my other mill's clamping set. I've got as far as the threading; it's a strip of mild steel about 150mm long which when cut will make 5 or 6 tee-nuts.

My lack of experience was (again) evident when the M12x1.75 spiral-point machine-tap entered the hole about 3 threads and the spindle stopped through lack of torque. It was mounted in Tormach's ER20 tension-compression tapping head. I'm pretty sure I had the settings right in F360 (500 rpm, correct axial feed of 1.75mm/rev, etc). I suppose I should have foreseen this having tapped quite a few M12 holes by hand.....Of course I can, and probably will, just hand-tap the holes but the exercise raises a few questions which I'm hoping the assembled brains-trust can help-with!

1. I just bought 2 each of metric taps 3-12mm, in both spiral point and spiral flute flavours. Clearly, I wasted money on the M12s but which others should I try returning for a refund? Who here has successfully tapped 3/8" UNC or M10 in steel with the Tormach 1hp spindle? If not, does 5/16" UNC or M8 work? What rpm was used?

2. If tapping above (say) M8 is a struggle, here in UK I'm looking for a thread-milling solution which isn't size-specific; an M12 carbide threadmill is around £120 ($156) - forget it. No doubt I can try to fashion a single-point tool out of (say) a 5/16" round HSS tool blank but it would be quite a project for me without a tool grinder. Any ideas? Ideally, I'd want one tool to do both M10 and M12 internal threads.

3. At 500 rpm, what hp is my 770's spindle delivering? I'm sure it's not 1hp! If anyone has done a hp (or better, torque) curve for this mill I'd be interested to see. I did call Tormach Tech. support before trying this madness and they were sceptical, saying they normally don't use taps bigger than 1/4", and at 900 rpm on the hi-belt setting! To be honest, 500 rpm seems quick enough for me at my stage of experience but perhaps that's the only way the machine will give enough torque for the job. Thoughts, please?

Ultimately, I'm pleased not-to have busted a tool or crashed the work but annoyed (and not a little embarassed) to have wasted £££ on some of the bigger taps I can't use. Hey-Ho, experience isn't gained cheaply, unless it's learned from others!

Cheers, Andy

Similar Threads:

• Tormach PCNC 1100 capability/precision
• CAD Capability
• Y-axis capability
• Best way to get Al engraving capability to VMC?
• Capability

[C*H*U*D]

Are you running your belt in Hi or Low? I can't tap 1/4-20 at 500 on the Hi setting.

[Fortune7]

Thanks, C*H*U*D, I'm using the low belt setting.

Cheers, Andy

[Bob La Londe]

Something to think about. While those taps may not spin through on your Tormach they are not wasted. I often use machine taps for hand tapping with a tap guide. They cut very fast for their intended applications and without having to back out several times on thru holes with spiral points, and often only having to back out once on blind holes with spiral flute taps in order to bottom out. I actually don't do much tapping on my mills although I do sometimes use a thread mill for odd stuff. I do most of my tapping as a secondary operation with a drill press and a tapping head. In fact I do so many 10-32 and 1/4-20 holes I have two bench top drill presses setup with tapping heads that have those taps more or less permanently mounted.

[Fortune7]

Something to think about. While those taps may not spin through on your Tormach they are not wasted. I often use machine taps for hand tapping with a tap guide. They cut very fast for their intended applications and without having to back out several times on thru holes with spiral points, and often only having to back out once on blind holes with spiral flute taps in order to bottom out. I actually don't do much tapping on my mills although I do sometimes use a thread mill for odd stuff. I do most of my tapping as a secondary operation with a drill press and a tapping head. In fact I do so many 10-32 and 1/4-20 holes I have two bench top drill presses setup with tapping heads that have those taps more or less permanently mounted.

Thanks, Bob - good info. I guess I can use the taps as you suggest in my other mill, chinese but 'bridgeport' size and power, with the geared spindle I bet it would have the beans to drive the tap thro', and as you say, with machine taps (SP/SF) there's less concern about chip relief.

Cheers, Andy

[SCzEngrgGroup]

I would not expect power tapping 12mm threads in steel to be within the range of any 1HP machine with some serious reduction on the spindle. At a minimum, you'd have to go down to at least 50% thread, likely even less, and probably take multiple passes, to get to full depth (and that's not really practical without a synchronized spindle).

I would do as Bob suggested and use the machine as a tap guide, but turn the tap by hand. Otherwise, I think you'll end up spending a lot of money on broken taps.

Regards,
Ray L.

[GBru]

Hi Andy

Like you, I too failed miserably at tapping an M10 thread into 25mm thick Mild Steel yesterday. As Ray has already suggested I drilled a 9mm hole which = 50% thread but the 770 still stalled out on me in Low range. Feeling deflated I decided that the only way forward is thread milling so bought myself a M10 Helical Thread Mill from shop-apt.co.uk, not cheap at £108.00.

Next task is to figure out how to apply this in Fusion360, but will create a new thread for this so as to not jack this one.

FWIW, I will be ordering some single point thread mills probably beginning of November from Tormach. Let me know if you need anything, probably work well for both of us as we can share shipping costs.

G.

[MFchief]

G.

Check out NYC CNC, if you haven't seen it before. John has a youtube channel and a large percentage of his videos relate to Tormach machines. He recently did one on how to thread mill in Fusion 360 on a Tormach mill.



Terry

[GBru]

Thanks Terry! Yup seen that vid from John, although I have noticed that Fusion now has a Thread Mill feature which I think I have figured out after reading some HSM threads.

G


Sent from my iPhone using Tapatalk

[Fortune7]

Hi Andy

Like you, I too failed miserably at tapping an M10 thread into 25mm thick Mild Steel yesterday. As Ray has already suggested I drilled a 9mm hole which = 50% thread but the 770 still stalled out on me in Low range. Feeling deflated I decided that the only way forward is thread milling so bought myself a M10 Helical Thread Mill from shop-apt.co.uk, not cheap at £108.00.

Next task is to figure out how to apply this in Fusion360, but will create a new thread for this so as to not jack this one.

FWIW, I will be ordering some single point thread mills probably beginning of November from Tormach. Let me know if you need anything, probably work well for both of us as we can share shipping costs.

G.

Thanks, Grant - good to know. I'd be interested in your experience with the M10 threadmill (F360, speeds/feeds, etc.) For now, I'll use my taps in my other mill on low-speed where I think there'll be enough torque to do M12. The weak point (apart from the tap breaking!) will probably be the ER32 collet slipping but we'll see.

I'd still be grateful for general feedback or advice from others re: tapping with the 770 - max. diameter and rpm. if poss please.

Thanks also for offer of a shared-shipping purchase from Tormach in November - I think I might get a couple of those thread mills too - can't find anything equivalent here in UK for the same price, even though the £/$ still isn't good!

Cheers, Andy

[Bob La Londe]

Thanks, Grant - good to know. I'd be interested in your experience with the M10 threadmill (F360, speeds/feeds, etc.) For now, I'll use my taps in my other mill on low-speed where I think there'll be enough torque to do M12. The weak point (apart from the tap breaking!) will probably be the ER32 collet slipping but we'll see.

I'd still be grateful for general feedback or advice from others re: tapping with the 770 - max. diameter and rpm. if poss please.

Thanks also for offer of a shared-shipping purchase from Tormach in November - I think I might get a couple of those thread mills too - can't find anything equivalent here in UK for the same price, even though the £/$ still isn't good!

Cheers, Andy

Nice thing about single point thread mills is you can thread any pitch. Even tapered threads if you can program it. They are limited to the backlash of your machine for concentricity, you can destroy them quick if you push them too hard, and they are expensive.

[RussMachine]

Through trial-and-error on my 770, I've learned that the largest tap I can push through 1018 Steel is 5/16" ( 8 MM )
There simply isn't enough torque at low RPM's with the small 1 horsepower motor.
I also have to run the tap at high RPM's to get the job done.
At least 1000 RPM to prevent stalling.
Anything over 5/16" (8 MM ) should be done with a threadmill.
This is the threadmill I use:
5 16" 18 48 TPI Single Pitch Thread Mill Brand New TiAlN Coated | eBay

[Fortune7]

Through trial-and-error on my 770, I've learned that the largest tap I can push through 1018 Steel is 5/16" ( 8 MM )
There simply isn't enough torque at low RPM's with the small 1 horsepower motor.
I also have to run the tap at high RPM's to get the job done.
At least 1000 RPM to prevent stalling.
Anything over 5/16" (8 MM ) should be done with a threadmill.
This is the threadmill I use:
5 16" 18 48 TPI Single Pitch Thread Mill Brand New TiAlN Coated | eBay

That's great feedback - thanks!

Andy

[RussMachine]

Glad I could help Andy.
Thread milling can easily be programmed by hand.
No need for CAD/CAM software
Start at the bottom of your hole, circle mill Anti-Clockwise G03. (Climb-Cut)
Circle mill and RAMP into your cut 1/4 Pitch in Z to get started.
Then, for every full circle come up one 'Pitch' distance in Z.
Repeat G03 with Z moves until you clear the hole.

[SCzEngrgGroup]

Glad I could help Andy.
Thread milling can easily be programmed by hand.
No need for CAD/CAM software
Start at the bottom of your hole, circle mill Anti-Clockwise G03. (Climb-Cut)
Circle mill and RAMP into your cut 1/4 Pitch in Z to get started.
Then, for every full circle come up one 'Pitch' distance in Z.
Repeat G03 with Z moves until you clear the hole.

Start at the bottom, and work up if cutting right-hand female threads, or left-hand male threads.
Start at the top, and work down if cutting left-hand female threads, or right-hand male threads.

Regards,
Ray L.

[RussMachine]

Start at the bottom, and work up if cutting right-hand female threads, or left-hand male threads.
Start at the top, and work down if cutting left-hand female threads, or right-hand male threads.

OOPS!
I forgot to mention that tidbit.
Thanks Ray.
I was visualizing internal right hand threads, which accounts for about 90% of my thread milling operations.