Peck tapping with floating holder?

Quickie. As above.

Can I CNC peck tap (G84 Q_) with a floating holder, or would the result be weird/unreliable/etc? Would I need to change any parameter?

Tichy said:

Quickie. As above.

Can I CNC peck tap (G84 Q_) with a floating holder, or would the result be weird/unreliable/etc? Would I need to change any parameter?

Click to expand...

Hello Tichy,
There are two types of Peck Tap Cycles available, one where the tap retracts a small amount at the end of each Peck and the other where the Tap withdraws to the R Plane at the end of each Peck. The type of cycle is selected via parameter bit 5200.5 in controls from FS16 onward.

Peck Tapping with a floating holder is OK using the cycle where the tap doesn't retract to the R Plane between each Peck, that is, it stays engaged with the work-piece until the tapping operation is complete.

The issue you may have when using the cycle where the tap withdraws to the R Plane, is that when the tap initially started, there may have been some compression of the axial floating system before the tap actually engaged with the material. In this situation, when the tap tries to re-engage with the now partially cut thread, their may be a slight mismatch of index between the tap and the thread in the hole. This is more likely to occur if the spring resistance of the floating holder is weak; generally the resistance is quite reasonable and you shouldn't have any trouble in this regard.

Regards,

Bill

Tichy said:

Quickie. As above.

Can I CNC peck tap (G84 Q_) with a floating holder, or would the result be weird/unreliable/etc? Would I need to change any parameter?

Click to expand...

Damnit Tichy, just Tap the hole. Get a really good Tap and make sure the Minor Diameter is right, and just Tap it. It's what they are made for. Modern Taps don't need Floating holders. Old equipment does.

And unless you are having trouble getting finished with a hole, don't peck. Wait until you have a problem then work out the problem, you've got the cart in front of the horse.

R

Thanks Bill. My parameters are 1mm retract for the fast peck cycle. That's why I asked, maybe I needed more.

what is "peck tapping"?

dian said:

what is "peck tapping"?

Click to expand...

Pecking with a tap, like peck drilling.

I have never used it, not sure what the point is. I have tapped some nasty shit before, and usually if it is a major problem we moved to thread milling, Not sure of what it's 'real' application is.

I have done it, but I would not use a "rigid tap" cycle.

Mike1974 said:

Pecking with a tap, like peck drilling.

I have never used it, not sure what the point is. I have tapped some nasty shit before, and usually if it is a major problem we moved to thread milling, Not sure of what it's 'real' application is.

Click to expand...

You'd move to thread mill an M5?

The real application for me is that since I moved to peck tapping I haven't broken a tap and that was three months ago or so. It used to happen pretty regularly in the past. Sure, I'm sure it'll happen again, it just hasn't, not over more than a thousand holes.

I don't work with that shitty material normally. 1312, 2333, 4404. Sometimes SMO. Now that last one is a real b*tch. But I often have to tap deep holes with a small diameter. As an example, tapping a 40mm M5 hole.

Tichy said:

You'd move to thread mill an M5?

The real application for me is that since I moved to peck tapping I haven't broken a tap and that was three months ago or so. It used to happen pretty regularly in the past. Sure, I'm sure it'll happen again, it just hasn't.

I don't work with that shitty material normally. 1312, 2333, 4404. Sometimes SMO. Now that last one is a real b*tch. But I often have to tap very deep holes with a small diameter.

Click to expand...

M5 isn't that small in my world, but depending on depth....

I regularly mill features with .031 and smaller tools. Ran a production job one time thread milling 10-32 because they needed threads to within 1 turn of bottom for some reason, but they were only about 3/8" deep IIRC.

Mike1974 said:

M5 isn't that small in my world, but depending on depth....

I regularly mill features with .031 and smaller tools. Ran a production job one time thread milling 10-32 because they needed threads to within 1 turn of bottom for some reason, but they were only about 3/8" deep IIRC.

Click to expand...

I think the smallest I ever tapped is M2.5. M4 is pretty regular. We don't have tools for thread milling small holes. We're pretty much stone age. I operate a stone age machine.

I would never bother to peck tap anything where the hole is less than 3D deep UNLESS the material is a total nightmare.

I think another reason I haven't broken any taps at all lately is I switched to a combination of air gun plus internal cooling. It's annoying when you open the door tho. Aerosols everything.

5 axis Fidia guy said:

I have done it, but I would not use a "rigid tap" cycle.

Click to expand...

Hello Fidia guy,
When you say "I have done it", are you referring to Peck Tapping? If so, what cycle did you use if not Rigid Tapping and what Control? If a Fanuc Control, Peck Tapping is only available with Rigid Tapping. To Peck Tap with the standard G84 cycle, you would have to repeat the tapping of the same hole at ever increasing Z depth until full depth is reached. Although the tap would likely follow the previous thread, its not guaranteed.

Using Rigid Tapping would ensure the spindle and hence the tap, would stay in synch with the partly completed thread; surely there is no argument for not using Rigid Tapping when Peck Tapping.

Regards,

Bill