Floating Tap stripping bottom half of the threads (?)

[Phase]

Hi,

I have not done much threading and I have not done it in quite a while, but this is weird...

I'm using a Fadal VMC15 with a Maritool ER25 floating tap holder and a OSG M5-0.8 spiral point tap. I drill a 0.166" hole in a 0.5" piece of 6061 and tap it. At that point the threads at the bottom half of the hole are gone. The threads at the top half are still there. It is a thru hole. I go 0.7" deep on a 0.5" stock so that the point of the tap clears the bottom of the stock.

The Q looks okay: 25.4 / 0.8 => 31.75 and 1 / 31.75 = 0.031496 => Q0.0315

Thoughts?

T10 M6
S200 M3
E1
G90 G0 X0.5 Y0.25
G43 Z0.6 H10
M8
Z0.2
G98 G84 X0.5 Y0.25 Z-0.7 R0+0.2 Q0.0315 F200.
G80
Z0.6

I do not have many of these to make, but it would be nice to know what is going on. Thanks!

 

[Leviathan]

Does your floating tap holder have an adjustable break point (the point at which it actually starts to float)? I suspect it is too high and the tap is recutting on the first part of the reversal until the tension it sufficient to get it tracking correctly again.

I know what you are thinking....the tap should break first. Weirder things have happened. It is aluminum. I had a particular brand of 1"-8nc tap that I couldn't use on the radial drill or in a manual lathe tailstock because it would happily cut on the reverse just as well as forward leaving anything from a really loose thread to a tough looking 1" hole...in steel.

In your case it's a much smaller tap...in softer metal.

Something to check anyway. Good luck.

Leviathan

Sent from my SM-G930W8 using Tapatalk

 

[Delw]

code looks wrong
heres a copy from a pdf I saved from fadalcnc.

I'm home now and cant give you proven code from my fadals

Rigid tapping uses a feedback signal from the spindle system and synchronizes the spindle
motion with the Z axis motion. This allows for consistent threads, precise control for blind holes,
and many other benefits.
Note: When rigid tapping, use the low range for spindle speeds of 750 RPM and below, and use
the high range for spindle speeds of 751 RPM and above.
Example: S750.1 (.1 for low range) S1500.2 (.2 is for high range)
The following example is for a 10 X 32 Tap at 1500 RPM:
Format 1:
Formula for Q value is 1.0 / TPI (1.0/32 = 0.0312)
N1 G0 G90 S1500.2 M5
N2 H1 Z.5
N3 X0 Y0 G84.1 Z-.5 F1500.2 Q0.0312
N4 X1. Y1.
N5 G80
Format 2:
Formula for F value is RPM / TPI (1500/32 = 46.87)
N1 G0 G90 S1500.2 M5
N2 H1 Z.5
N3 X0 Y0 G84.1 Z-.5 S1500.2 F46.87
N4 X1. Y1.
N5 G80

also when you say floating tap, your not meaning compression tapping are you, ie the tap holder isnt pring loaded like a tapmatic?
if it ise you have to feedrate in slower and feedout out faster in reverse like a lathe

 

[Phase]

Does your floating tap holder have an adjustable break point (the point at which it actually starts to float)? I suspect it is too high and the tap is recutting on the first part of the reversal until the tension it sufficient to get it tracking correctly again.

I know what you are thinking....the tap should break first. Weirder things have happened. It is aluminum. I had a particular brand of 1"-8nc tap that I couldn't use on the radial drill or in a manual lathe tailstock because it would happily cut on the reverse just as well as forward leaving anything from a really loose thread to a tough looking 1" hole...in steel.

Hi, this is the item CAT40 ER25 FLOATING TAP COLLET CHUCK TOOL HOLDER MariTool As far as I can tell there are no adjustments. It is possible that it is recutting, but what bugs me is that I only go down 0.7" so at reversal the tap is fully engaged. I can't quite figure out why it would not strip all of them, but only the bottom half. But if it is a spring tension issue maybe the ER16 version has setting meant for the small taps (I'm using the ER25). I'll call Maritool on Monday. Thanks!

code looks wrong
when you say floating tap, your not meaning compression tapping are you, ie the tap holder isnt pring loaded like a tapmatic? if it ise you have to feedrate in slower and feedout out faster in reverse like a lathe

Yes, it is not rigid tapping. It is a spring loaded holder with 5/16" give up and 5/16" give down. The tap engages and pulls itself down and then back up. The spring tension gives it enough room to not strip the threads (or may be not, LOL). My spindle is not synchronized. I'm using a canned cycle. There is only one RPM setting I used F200 for 200 RPM. Thanks!

 

[Ox]

'bout gotta be the tap jamming up with material.

Are you dooing this on one hole, or a whole series with same results each time?

If there is any tracking issues in any way - ALL the threads should be gone.

Try a different tap?
Preferably a different type/brand/coating...

What fer lube are you using?


------------------------

Think Snow Eh!
Ox

 

[sinha]

Peck tapping in non-rigid mode is rather unusual. Remove Q, and it should work perfectly.

 

[Spinit]

Hi,

I have not done much threading and I have not done it in quite a while, but this is weird...

I'm using a Fadal VMC15 with a Maritool ER25 floating tap holder and a OSG M5-0.8 spiral point tap. I drill a 0.166" hole in a 0.5" piece of 6061 and tap it. At that point the threads at the bottom half of the hole are gone. The threads at the top half are still there. It is a thru hole. I go 0.7" deep on a 0.5" stock so that the point of the tap clears the bottom of the stock.

The Q looks okay: 25.4 / 0.8 => 31.75 and 1 / 31.75 = 0.031496 => Q0.0315

Thoughts?

T10 M6
S200 M3
E1
G90 G0 X0.5 Y0.25
G43 Z0.6 H10
M8
Z0.2
G98 G84 X0.5 Y0.25 Z-0.7 R0+0.2 Q0.0315 F200.
G80
Z0.6

I do not have many of these to make, but it would be nice to know what is going on. Thanks!

Sounds like your hole is too shallow or your tap needs to go shallower. Maybe the tap is bottoming out and gouging up. Spring loaded tapping varies because it is not rigid taping.

 

[Delw]

Hi, this is the item CAT40 ER25 FLOATING TAP COLLET CHUCK TOOL HOLDER MariTool As far as I can tell there are no adjustments. It is possible that it is recutting, but what bugs me is that I only go down 0.7" so at reversal the tap is fully engaged. I can't quite figure out why it would not strip all of them, but only the bottom half. But if it is a spring tension issue maybe the ER16 version has setting meant for the small taps (I'm using the ER25). I'll call Maritool on Monday. Thanks!



Yes, it is not rigid tapping. It is a spring loaded holder with 5/16" give up and 5/16" give down. The tap engages and pulls itself down and then back up. The spring tension gives it enough room to not strip the threads (or may be not, LOL). My spindle is not synchronized. I'm using a canned cycle. There is only one RPM setting I used F200 for 200 RPM. Thanks!

Thats your problem your using a compression holder with a rigid tap sequence. I dont believe that will work.
just program it with a g1 feed down slower than your pitch and reverse spindle feed feed up a little faster than your pitch.


I believe you should have errored out if you DIDNT have rigid tap on your fadal.
try the code that I posted above and see if you get an error. ( back away from the part so you dont crash) if you dont get an error with the code above you could have rigid tap.

what year is the machine?

 

[Delw]

Peck tapping in non-rigid mode is rather unusual. Remove Q, and it should work perfectly.

on a fadal q is the lead not peck tapping

 

[KennyBoi]

Seems like material loading on tap maybe? I am assuming it is a two flute for aluminum and why not form tap, also 200 RPM seems very slow for tapping M5 thread in aluminum.

 

[adama]

If F is spose to be spindle speed divided by TPI your programme is wrong. Because i make it 6 not 200?

Whats your coolant concentration and is your tap a coated tap? Gold - TiN coatings will cold weld to aluminum amazingly well at these speeds!

 

[Delw]

my bad you can use g84 for compression tapping

heres the code from the manual

Compression (non
self-reversing) Tap
Holder Series
These tapping heads should use the G84 or G74 Tapping cycle. It is best to use
these in the high range (S word with a .2). The P word may be used to increase
the feed rate of the tap when it reverses, if the F word is used for the RPM and
the Q word is used for the lead. The G74 is used in Format 1 style ONLY.
EXAMPLE: Format 1:
N1 O1 (COMPRESSION TAP HOLDER SERIES
N2 G0 G8 G90 S1000.2 M3 E1 X0 Y0
N3 H1 M7 Z.4
N4 G84 G99 R0+.4 Z-.3 F1000. Q.05 X0 Y0
N5 X1.
N6 G80
N7 M5 M9
EXAMPLE: Format 2:
The following formula calculates the required feed rate:
Feed rate = ((1 / threads per inch) * RPM)
= ((1 / 20) * 1000)
= (.05 * 1000)
= 50.
N1 O1 (COMPRESSION TAP HOLDER SERIES
N2 G0 G8 G90 S1000.2 M3 E1 X0 Y0
N3 H1 M7 Z.4
N4 G84 G99 R0+.4 Z-.3 S1000.2 F50. X0 Y0 100% feed calculation here
N5 X1.
N6 G80
N7 M5 M9

 

[sinha]

on a fadal q is the lead not peck tapping

Thank you for information.

 

[sinha]

Is the tap clearing the job at the bottom completely? If so, that may be the problem. While returning, it may not be engaging the same threads initially.

 

[White Lightning]

Is the hole chamfered prior to tapping allowing the tap to start easily?

The tap may not want to start until spring pressure builds thus making a few revolutions before actually moving down into the hole. As the tap partially exits the bottom of the hole the high spring pressure may force the tap ahead and basically strip the bottom portion. On retraction it may be realigning with a good thread and retracting without damaging the top threads.

Just a thought. Good luck.

Sent from my SM-G960U using Tapatalk

 

[converterking]

If the spindle isn't stopping and reversing fast enough at the bottom of the hole you may need to add a dwell time. I have used a .5-.8 dwell time on one machine.

 

[sinha]

If the spindle isn't stopping and reversing fast enough at the bottom of the hole you may need to add a dwell time. I have used a .5-.8 dwell time on one machine.

This could be interesting.
So, your observation is that adding a small dwell actually speeds up the rpm reversal process.
I did not know this.

 

[Hazzert]

This could be interesting.
So, your observation is that adding a small dwell actually speeds up the rpm reversal process.
I did not know this.

The small dwell allows time for the spindle to finish winding down before changing direction and feeding out.

 

[Delw]

If the spindle isn't stopping and reversing fast enough at the bottom of the hole you may need to add a dwell time. I have used a .5-.8 dwell time on one machine.

The small dwell allows time for the spindle to finish winding down before changing direction and feeding out.

Would a (dwell)p200 added to a G84 cycle work?
I dont know I never tried it, now you got me curious

 

[Hazzert]

Would a (dwell)p200 added to a G84 cycle work?
I dont know I never tried it, now you got me curious

It should, depending on the control the P value may be in seconds or milliseconds.