Tapping methods without rigid tapping

[Maverick302]

Hello Brian,
Extension, Compression tapping tools are available that have a Freewheeling zone. Typically and in its simplest form, its an axial slot in the bore that the tapping tool runs in, with a drive pin engaged in the slot. The Freewheel feature is an Annular groove that the axial slot crosses. To operate:
1. the Z axis is stopped short of the full depth to be tapped and a dwell programmed. During this dwell the tap continues to feed towards the bottom of the hole until the drive pin finds the annular groove. In this position, the spindle can rotate but the tap won't be rotating and therefore, no further feed of the tap occurs.

2. the spindle rotation direction is reversed and the Z axis starts to feed back towards the Z Start Point for the tapping operation. As the Z axis moves, the drive pin engages in the axial slot on the opposite side of the annular groove and starts to feed out of the tapped hole.

With this type of Tapping Tool, very accurate tapping depths can be achieved and tapping close to the bottom of a blind hole is consistently achievable.

Regards,

Bill

This actually sounds like the perfect solution. Do you happen to have a brand or link you could share?

 

[5 axis Fidia guy]

What???

Never power tapped hard 56 R.C. S-7 I see.

 

[Mud]

This actually sounds like the perfect solution. Do you happen to have a brand or link you could share?

My favorite are Universal/TSD/Devlieg or whatever they are called now.

 

[Mud]

Isn't it possible for some error in spindle rotation to over-rotate the tap and bottom out?

You have to know your machine. Whatever your machine does will be consistent from hole to hole. At least if it's working right I suppose. It will overtravel the same every time at the top and at the bottom so you experiment a little and make notes. Program a hole with a very short tap depth and watch it and measure it and adjust the program and also tool length if needed to get the results you need. I usually add .200 to the height of the programmed hole or else raise the tool by about .200 for a tap in a T/C holder to safely clear the top of the part before it moves to the next hole. Other machines and controls and spindle drives might give different results. You can also add a slight dwell at the top of the hole to give the tap an extra turn to wind completely out of the hole before rapiding away to the next one but I find it simpler to just raise the beginning of the hole in the CAM file.

It's considered common to reduce the feed by 5 to 10% so that the T/C holder extends while feeding the tap, I find that's not necessary, because usually the holder extends at the bottom of the hole while the spindle is slowing to a stop and feed has halted, if the holder is already extended too far when that happens you can top out the holder and pull the part out of the vise. Again, you have to know your individual machine. And know how it varies from speed to speed. Same with tapping heads, a little more clearance at the top can reduce stress on the operator, and you need to determine how much overtravel happens at the bottom before the tapping head declutches.

About tapping heads - the NC heads reverse at the same speed as they go forward. That's so you can program it with the same feed in both directions, I usually use a feed in/feed out boring cycle. Standard tapping heads usually reverse faster than forward to get the tap out faster when used manually in a drill press so they would need programming gymnastics to use in a CNC.

 

[Mr. Atoz]

I have struggled using a form tap in a tension/compression holder when cutting steel. There must be a secret I don't know. Cut taps - no problem.

 

[Maverick302]

You have to know your machine. Whatever your machine does will be consistent from hole to hole. At least if it's working right I suppose. It will overtravel the same at the top and bottom so you experiment a little and make notes. Program a hole with a very short tap depth and watch it and measure it and adjust the program and also tool length if needed to get the results you need. I usually add .200 to the height of the programmed hole or else raise the tool by about .200 for a tap in a T/C holder to safely clear the top of the part before it moves to the next hole. Other machines and controls and spindle drives might give different results.

It's considered common to reduce the feed by 5 to 10% so that the T/C holder extends while feeding the tap, I find that's not necessary, because usually the holder extends at the bottom of the hole while the spindle is slowing to a stop and feed has halted, if the holder is already extended too far when that happens you can top out the holder and pull the part out of the vise. Again, you have to know your individual machine. And know how it varies from speed to speed. Same with tapping heads, a little more clearance at the top can reduce stress on the operator, and you need to determine how much overtravel happens at the bottom before the tapping head declutches.

About tapping heads - the NC heads reverse at the same speed as they go forward. That's so you can program it with the same feed in both directions, I usually use a feed in/feed out cycle. Standard tapping heads usually reverse faster than forward to get the tap out faster when used manually in a drill press so they would need programming gymnastics to use in a CNC.

Thanks, that makes sense.

 

[Vancbiker]

I have struggled using a form tap in a tension/compression holder when cutting steel. There must be a secret I don't know. Cut taps - no problem.

Switch to a tension only tap holder when using form taps. The lack of compression forces the form tap to start consistently.

 

[Brian]

Hello Brian,
Extension, Compression tapping tools are available that have a Freewheeling zone. Typically and in its simplest form, its an axial slot in the bore that the tapping tool runs in, with a drive pin engaged in the slot. The Freewheel feature is an Annular groove that the axial slot crosses. To operate:
1. the Z axis is stopped short of the full depth to be tapped and a dwell programmed. During this dwell the tap continues to feed towards the bottom of the hole until the drive pin finds the annular groove. In this position, the spindle can rotate but the tap won't be rotating and therefore, no further feed of the tap occurs.

2. the spindle rotation direction is reversed and the Z axis starts to feed back towards the Z Start Point for the tapping operation. As the Z axis moves, the drive pin engages in the axial slot on the opposite side of the annular groove and starts to feed out of the tapped hole.

With this type of Tapping Tool, very accurate tapping depths can be achieved and tapping close to the bottom of a blind hole is consistently achievable.

Regards,

Bill

Not sure I've seen many of those for the milling machines. Common on lathes though, Hardinge made the TT 5/8 style units and I've used larger unit on the Warner Swazey turret lathes we had. Been using the T&C units for years though, they hold depths within probably less than .010" tolerance for me all the time.

 

[angelw]

This actually sounds like the perfect solution. Do you happen to have a brand or link you could share?

Hello Maverick,
Its been years since I've had to source any, as most of the machines, lathes and MC, I deal with have rigid tapping, but I'll look back through records to get the make and where I got them.

For Machining Centres, I've used both dedicated BT tapping tools and parallel shank tools with a Whistle Stop held in a side lock milling tool holder.

Regards,

Bill

 

[dieselpilot]

Not sure I've seen many of those for the milling machines. Common on lathes though, Hardinge made the TT 5/8 style units and I've used larger unit on the Warner Swazey turret lathes we had. Been using the T&C units for years though, they hold depths within probably less than .010" tolerance for me all the time.

These are releasing tap holders. The discontinued NC series by Tapmatic are of this type and were also sold by Kennametal. I'm sure there were other makes, but patents on these are older than I am. You can find them on Ebay. http://www.tools-n-gizmos.com/specs/Tapmatic_NC-x_QC.html

Were they actually that common? It only seems necessary with a machine that didn't stop fast or consistently and depth had to be accurate. You'd have to have a lot of holes before finishing by hand was more expensive than the tool.

 

[CarbideBob]

Never power tapped hard 56 R.C. S-7 I see.

Giggle and be shy a bit. You are the man.
I know nothing and admit to lack of knowing about cutting tools and chip formation.
You have it nailed, I do not and when I die the Lord is going to get a lot of questions about metal cutting.

 

[FredC]

Another source for releasing tap holders Soma Tool:

R&L Releasing Tap Holder | Somma Tool Company

View our line of R&L Releasing Tap Holder.

www.sommatool.com

I have an older version not in their catalog anymore. It works well on turret lathes and I have used it occasionally on an Omniturn. These do release very cleanly and do not hammer on a turret lathe. The few times I ran them on the Omniturn each time I wrote the programs I got a release at depth and reversed before the tap made a full revolution. Never broke a tap on set up or running.
I assume the one in the link will work as well on CNC lathes, no clue if it could work in a mill. You could call and ask they will give you a straight answer.

 

[5 axis Fidia guy]

Giggle and be shy a bit. You are the man.
I know nothing and admit to lack of knowing about cutting tools and chip formation.
You have it nailed, I do not and when I die the Lord is going to get a lot of questions about metal cutting.

Exactly what I thought.

 

[MwTech Inc]

I use a RDT50, tapmatic. As Mud said use a boring cycle, I back off the feed rate just a tad then pickup the retract rate a bit too.
Don't be scared of a used one, super easy to fix. Parts are not bad from Tapmatic
Just pop it apart and replace anything worn.
Get used to it by running some thru holes and you will learn the lead the head has.....then it's a no brainer to use.

 

[CarbideBob]

Exactly what I thought.

Not sure how to take that comment.

 

[Vancbiker]

Not sure how to take that comment.

I'm thinking 5 axis guy doesn't understand sarcasm.

 

[mhajicek]

• Thread milling - How small of a thread size is realistic? Does cost of tooling really add up relying on this method? Any other caveats?

I've threadmilled a few hundred 000-120 holes in grade 5 Ti. At that size the tool wears and deflects pretty quickly, and I had to keep dialing it in, and replacing the tool fairly often. I switched to a form tap; much better tool life and process reliability.

 

[M. Moore]

About tapping heads - the NC heads reverse at the same speed as they go forward. That's so you can program it with the same feed in both directions, I usually use a feed in/feed out boring cycle. Standard tapping heads usually reverse faster than forward to get the tap out faster when used manually in a drill press so they would need programming gymnastics to use in a CNC.

I use a standard head for tapping, a Procunier. It reverses faster but it is no problem when running the same feed rate in and out. The clutch just slips a little and out comes the tap. The depth accuracy is quite amazing. I have been tapping 4mm x .7 threads in stainless. Did over 500 holes with one tap which just started to complain at the end of the run.
Also they are blind holes.