Form Tapping

[hersh]

Hi all,
I'm using an PCNC1100 with their ER20 floating tap head and YG brand M3 threadforming tap.


I'm trying to form tap some M3x0.5 holes in AL6061 about 0.30" deep, hole depth is 0.40". The problem is, about the top half of the threads are being pulled out, so I can wiggle the screw into the hole past several threads before it stops and I have to start turning it.

I have had success using thread cutting taps of this size and others with not issues.

I checked on a manual mill, using the same 7/64" (0.109") drill and same M3 tap, power tapping with a Bridgeport quill. Threads are fine. Inspected the tap, threads are not damaged or galled up.

So it must be something with my program or a setting.

I've tried both my original program generated in Fusion360 and then I made a test program using Pathpilot covnersational, same results, most of the threads are pulled out of the hole.

Is this a dwell time issue?
Am I not setting the tool length correct? (I jog down to a piece of shim stock and zero minus the thickness of the shim when I feel friction, since the tap head is spring loaded, its not a hard stop like a drill bit would be).


Any help would be appreciated.

Similar Threads:

• tapping : cut / form / mill + punch ?
• Need Help!- Form Tapping
• Roll form tapping questions
• Large Form Tapping In 400 BHN
• Newbie- Form Tapping

[Warren_3Deee]

I threadform a lot of small sizes (M3-M6), but by hand, and they do seem to take quite a bit more pressure than cutting taps. I'm wondering if the amount of torque with the tapping head isn't quite enough and so the Z movement is a little too fast for the rotation?

[jwatte]

What lube are you using? Tap Magic?

Also, I believe there should be zero dwell if you can help it, but that would affect all the threads, not just the top.

[hersh]

I watched the threads, I don't think its slipping, and I was able to tap using a drill chuck on a bridgeport. (These taps are brand new and have been in less than 10 holes of aluminum.)
On the Tormach its held in a ER20 collet.

I e-mailed Tormach, they responded within an hour.

They suggested either my clearance was too high (Retract is set at 0.20" above part, and clearance is 0.40" above part) or dwell was wrong.

It could be the retract, if there is enough movement in the floating head, that it gets to the retract height and the rapid to the clearance height, it could be pulling the threads out with it.
But then I checked my Dwell, its set at 0.2s ... So yea, that's probably it. Tormach suggested 0.5sec to give the head more time to catch up, which sounds right to me.

So I'll try it again tonight. 3 tenths of second between scrap and $$. Fun stuff.

[hersh]

What lube are you using? Tap Magic?

Also, I believe there should be zero dwell if you can help it, but that would affect all the threads, not just the top.

Yes, I'm using the blue Mist Coolant Tormach sells, which had been fine for cutting threads and general milling, but after the first ones pulled out, put some Relton A-9 Aluminum Cutting Fluid on the holes.


Why dwell at 0?
I feel like I've read that for pathpilot before, but that was before I had a Tormach.

[Steve Seebold]

If you’re using the E/C tapping head from Tormach, I have developed a process that works really well.

I run my tap at 500 RPM and a feed rate of 10% less than your calculated feed rate going in and 10% faster coming out.

When I thread holes 6-32 and smaller I use 5% compensation.

And I use flood coolant.

[popspipes]

sounds to me as if the spring pressure isnt enough to cause the tap to start biting into the hole but spinning until the pressure is great enough to start the tap.

The dwell in Sprutcam is to let the spindle stop before reversing reversing the Z at the bottom or end of the tap CW cycle, before starting the CCW cycle, I use .5 seconds for 320 rpm, the higher the rpm the more dwell is needed.

[rowbare]

Are you chamfering the hole before tapping?

bob

[Davez64]

sounds to me as if the spring pressure isnt enough to cause the tap to start biting into the hole but spinning until the pressure is great enough to start the tap.

The dwell in Sprutcam is to let the spindle stop before reversing reversing the Z at the bottom or end of the tap CW cycle, before starting the CCW cycle, I use .5 seconds for 320 rpm, the higher the rpm the more dwell is needed.

X2


Sent from my iPhone using Tapatalk Pro

[hersh]

Are you chamfering the hole before tapping?

bob

Yes, a 0.120" chamfer for the 0.109 hole.

I was able to get it to work last night. I set the dwell to 1.2seconds and I backed off the depth by 0.050".
After this, all the threads felt good, tapped 140 holes this way with no problem.

Still not sure what the problem is. But I noticed that the tap almost backs itself completely out of the hole before the head starts moving up to retract.

[Davez64]

Yes, a 0.120" chamfer for the 0.109 hole.

I was able to get it to work last night. I set the dwell to 1.2seconds and I backed off the depth by 0.050".
After this, all the threads felt good, tapped 140 holes this way with no problem.

Still not sure what the problem is. But I noticed that the tap almost backs itself completely out of the hole before the head starts moving up to retract.

I had that problem on a Hurco VMC with ridged tapping! Never found out the problem?


Sent from my iPhone using Tapatalk Pro

[SCzEngrgGroup]

You can easily judge whether your g-code is correct by watching the tapping head as it taps a hole. In an ideal world, the head will compress SLIGHTLY, as the tap enters the hole, then remain a fixed length as it runs to full depth. It will then extend SLIGHTLY more when the spindle stops, then retract SLIGHTLY as the spindle reverses, and the head starts moving up. It should then remain fixed length until the tap is competely clear of the hole. If you see significant extension or compression of the tapping head, then your settings are off. If the tapping head ever reaches either limit of its travel, it's game-over, and a broken tap, or stripped threads, will result. On mine, I see very little extension or compression throughout the whole cycle - perhaps on the order of 1/8" absolute worst case.

Regards,
Ray L.

[R.DesJardin]

I set dwell at 1.0 sec at the bottom and up feed 10% slower when reversing back up. Both my 1100's work with this. Also make sure you are feeding to clear the part up far enough that the tap has exited before the rapid up move up.

[MichaelHenry]

Also make sure you are feeding to clear the part up far enough that the tap has exited before the rapid up move up.

That's one of those lessons that one learns quickly.