[whagkangmakulet]

I need to make a 25 pcs of an aluminum bus bar with various holes, steps and an M4x.7 tap hole (8X) per bar. Can I drill,cut and prep a hole size for the M4x.7 for all 25 pcs. then setup the Procunier to tap all M4x.7 (200X) ?.... Thanks in advance!

[SCzEngrgGroup]

No reason why not....

Regards,
Ray L.

[whagkangmakulet]

No reason why not....

Regards,
Ray L.

Thanks! I'm a newbie, was told to drill and tap on the same setup. I should have spend the money on thread mills instead of procunier.

[SCzEngrgGroup]

Thanks! I'm a newbie, was told to drill and tap on the same setup. I should have spend the money on thread mills instead of procunier.

Thread mills make no sense for M4 threads - they'd take MUCH longer, and the threadmill that can do that size would be VERY delicate, easily broken, and expensive.

No problem using different setups for drilling and tapping, as long as you use the same coordinate reference for both. Tapping heads are relatively forgiving on alignment, so being off a few thou won't make a bit of difference.

Regards,
Ray L.

[whagkangmakulet]

Thread mills make no sense for M4 threads - they'd take MUCH longer, and the threadmill that can do that size would be VERY delicate, easily broken, and expensive.

No problem using different setups for drilling and tapping, as long as you use the same coordinate reference for both. Tapping heads are relatively forgiving on alignment, so being off a few thou won't make a bit of difference.

Regards,
Ray L.

Thanks Ray! I see this bus bar work will come around again in the next few months. Would you recommend for me to get Tormach tension compression tapping head to accommodate the ATC feature for M4 tapping if the quantity tap holes doubled..(400 tap holes)?

[SCzEngrgGroup]

If you plan to use an ATC, then tension/compression is the way to go, rather than a tapping head, as the tapping head cannot be used in an ATC.

BTW - On the Procunier, make sure you KNOW the true spindle speed, and set your feed rate based on that, NOT the speed you command in Mach3. Unlike other tapping heads, the Procunier does not tolerate the spindle down-feed exceeding the advance rate of the tap. If the head tries to lead the tap, the tap WILL be broken. Even knowing the actual spindle speed, I would suggest under-feeding by perhaps 5%, just to be safe. The Procunier will modulate its clutch as needed to feed properly.

Regards,
Ray L.

[rowbare]

For what you are doing, I would do it old school. Put the Procunier in a drill press and tap the 8 holes while the next part is running. It will take less time to do that than it would to re-clamp the parts in the mill. If you are doing single bars, it is probably faster to do it that way even if the number of holes doubles. You could probably do the holes in about the same time the two tool changes would take. Now if you were clamping 12 bars to a fixture plate, it would be a whole other story...

bob

[Steve Seebold]

[QUOTE=whagkangmakulet;1660310]I need to make a 25 pcs of an aluminum bus bar with various holes, steps and an M4x.7 tap hole (8X) per bar. Can I drill,cut and prep a hole size for the M4x.7 for all 25 pcs. then setup the Procunier to tap all M4x.7 (200X) ?.... Thanks in advance![/QUOTE

It would be so easy to GCODE the tapped holes in that part. Then you wouldn't need to spend the money on the Procunier tapping head. I have 2 Tap Matic heads that I haven't used since I learned how to GCODE my tapped holes.

[SCzEngrgGroup]

What does "GCODE tapped holes" mean?? Threadmill?? Use a tension/compression head? Other??

Regards,
Ray L.

[Steve Seebold]

What does "GCODE tapped holes" mean?? Threadmill?? Use a tension/compression head? Other??

Regards,
Ray L.

I use a tension/compression tapping head and write some GCODE for that. I have tapped 2-56 thru 1/4-20 threads that way.

[SCzEngrgGroup]

I use a tension/compression tapping head and write some GCODE for that. I have tapped 2-56 thru 1/4-20 threads that way.

And the code for using a tapping head is nearly identical, except don't reverse the spindle at the bottom, don't dwell while the spindle reverses, and retract at 2X instead of 1X feed. Both are "GCODE tapped holes" by your definition, and he already has the Procunier tapping head, and the tapping head is a lot faster.

Regards,
Ray L.

[JohnToner]

Ray,

Monday or Tuesday I'll be tapping 1/4 20 RH in 1/2" 6061 with #7 through holes and a spiral tap Will this code work?

G1 Z0.1000
M3 S400 F20
G1 Z-0600
M4 S800 F40
G1 Z0.1000

Thanks,
John
Or, did I just break a cheap tap inside an expensive part?

[kstrauss]

Consider using a thread forming tap in a T/C tapping head or they should work fine in your Procunier (I don't have one to try...). If you drill the right size holes thread forming taps work wonderfully and there is no swarf to jam things.

[JohnToner]

Thread forming taps are on my list of the next things I need to learn. For certain they should yield a much cleaner, professional looking thread. Did my code look like it would work with the Procunier?

[SCzEngrgGroup]

Ray,

Monday or Tuesday I'll be tapping 1/4 20 RH in 1/2" 6061 with #7 through holes and a spiral tap Will this code work?

G1 Z0.1000
M3 S400 F20
G1 Z-0600
M4 S800 F40
G1 Z0.1000

Thanks,
John
Or, did I just break a cheap tap inside an expensive part?

Where are you going to find a 1/4-20 tap 600 inches long? :-)

Actually, you DON'T reverse the spindle and DON'T change the RPM with a taping head, so remove the M4 line entirely. ALL you need to do is retract at 2X the downfeed rate, and the tapping head will reverse the rotation automatically. You should also pull out further, since the tapping head will trail the spindle coming out. You need to retract far enough to make sure the tap has completely disengaged before moving the to next hole.

G0 Z0.1000
M3 S400 F20
G1 Z-0.600
G1 Z0.2500

Regards,
Ray L.

[popspipes]

Or, did I just break a cheap tap inside an expensive part?

John,
I used the Alum and water mixture in a crockpot to take out a couple of #6 taps from aluminum, worked really well but it isnt fast. I have used a carbide drill on a couple as well but they were larger taps.

[SCzEngrgGroup]

John,

BTW - MAKE SURE you know what the actual spindle RPM is! The Procunier does NOT tolerate over-feed. If you're feeding at the correct rate for 400 RPM but the spindle is running slower, you WILL break the tap, and/or strip the hole.

Regards,
Ray L.

[JohnToner]

Thanks Ray,

I'll retract a bit further and also search for that missing decimal point. It must be around here someplace ;-)

[JohnToner]

So, can I kick the RPM to 450 or more? I have one of those hand held tachs but it's Chinese so there is a "slight" chance it isn't accurate.

[SCzEngrgGroup]

So, can I kick the RPM to 450 or more? I have one of those hand held tachs but it's Chinese so there is a "slight" chance it isn't accurate.

You can, in theory, run up to about 1000 RPM, but I prefer to go slower. I do my tapping at 300 RPM. But, the claim to fame on the Procunier is how gently it engages, so higher speeds are fine. I would still suggest you start slow, until you're sure everything is tuned properly.

Even a cheap Chines hand-tach should be pretty accurate. Make sure you allow enough time for the spindle speed to settle down. At lower speeds, they can often take several seconds to get up to speed and stable. You can put a G4 right after the M3 to make sure it's settled before tapping the first hole.

Regards,
Ray L.