What's new
What's new
By:
Advanced search…

Npt tapping lathe speed and feed help

T

twr

Hot Rolled
Joined
Mar 18, 2014
Location
Kitchener Ont. Canada
Hi I am trying key word trying, to tap 3/4 npt with a tension/comp holder on my lathe and as it's going in it's pulling the tension part out so i know my feed is to slow. What rpm and ipr feed should I be using in aluminum?
 
G97 Sxxxx M3 is a spindle RPM and direction.

With a spring holder I just

G97 S100 M3
G99
G0 X0 Z.5
G1 Z-1. F.071428
M5
G1 Z.5 M4

I've never tapped with G32 so not exactly sure about that?

Brent
 
yardbird said:
G97 Sxxxx M3 is a spindle RPM and direction.

With a spring holder I just

G97 S100 M3
G99
G0 X0 Z.5
G1 Z-1. F.071428
M5
G1 Z.5 M4

I've never tapped with G32 so not exactly sure about that?

Brent
Click to expand...
Hello Brent,
Using G32 over G1 is preferred, as G32 locks out the Feed Override function of the control. If the Feed Override setting is moved from 100%, on purpose or inadvertently, in a turning operation using G01, it normally doesn't have disastrous consequences. If the same were to happen in a tapping operation, the result is nearly always a wrecked thread and or a broken tap (depending on the amount of free travel in the axial floating tool holder). Using G32 will ensure that the programmed Feed Rate is used irrespective of the Feed Override setting.

Regards,

Bill
 
Post the exact code you are trying for the complete tapping operation for us to have a look.

Is you coolant restricted from entering the spring holder. My coolant pressure will give my spring holders a woody?

Brent
 
angelw said:
Hello Brent,
Using G32 over G1 is preferred, as G32 locks out the Feed Override function of the control. If the Feed Override setting is moved from 100%, on purpose or inadvertently, in a turning operation using G01, it normally doesn't have disastrous consequences. If the same were to happen in a tapping operation, the result is nearly always a wrecked thread and or a broken tap (depending on the amount of free travel in the axial floating tool holder). Using G32 will ensure that the programmed Feed Rate is used irrespective of the Feed Override setting.

Regards,

Bill
Click to expand...

Hi Bill

Actually I hadn't considered the feed override. Absolutely cause major problems.

Can you post an example of a tapping cycle using G32? Not long ago I saw an example that had a M5 in G32 line of code. I was confused on that.

Brent
 
twr said:
Well just tried it again with G99 same shit, it pulling comp holder out as it goes in. Rpm is 50 and ipr .0714 this can't be correct?
Click to expand...

Hi Tracey,
You need to determine if the feed of the machine matches the programmed feed. Still using G99, either via MDI, or in a short test program, have the Z axis feed over a distance and measure the time taken. Convert your 0.0714/rev into IPM feed rate and see if the calculated time for the programmed length equals the actual time taken. You can time it using a Stop Watch, or using the control's Timer System Variable in a Macro statement. If using a Stop Watch, make the Feed Length reasonably long so as to get better accuracy.

Regards,

Bill
 
yardbird said:
Hi Bill

Actually I hadn't considered the feed override. Absolutely cause major problems.

Can you post an example of a tapping cycle using G32? Not long ago I saw an example that had a M5 in G32 line of code. I was confused on that.

Brent
Click to expand...

Hello Brent,

G97 S600 M03
G0 X0.0 Z0.1 M08
G32 Z-1.0 F.071428
M04
G32 Z.1F0.071428
G0 Z1.0 M09

Due to the compression of the axial floating holder that can occur before the tap engages with the material and starts feeding, often a slightly slower feed rate than the actual lead of the tap is programmed so that the slight compression of the tool holder at the start and the axis deceleration at the end of the Z travel is compensated for. Similarly, due to axis acceleration when the spindle and axis travel reverse, the feed out is often programmed at a slightly faster rate than actual lead of the tap.

Regards,

Bill
 
angelw said:
Hello Brent,

G97 S600 M03
G0 X0.0 Z0.1 M08
G32 Z-1.0 F.071428
M04
G32 Z.1F0.071428
G0 Z1.0 M09

Due to the compression of the axial floating holder that can occur before the tap engages with the material and starts feeding, often a slightly slower feed rate than the actual lead of the tap is programmed so that the slight compression of the tool holder at the start and the axis deceleration at the end of the Z travel is compensated for. Similarly, due to axis acceleration when the spindle and axis travel reverse, the feed out is often programmed at a slightly faster rate than actual lead of the tap.

Regards,

Bill
Click to expand...

Thanks Bill

I'm not being nit picky here Bill because it's already been mentioned I'm seriously asking. Do G31 G32, G33, G76 cycles all feed in ipr unless of course G21 is active and then it'd metric. If G98 is active do those cycles also disregard G98 ipm and feed G99 ipr automatically?

I see where lots of guys rigid tap ipm feed rates on the mills but never have I once noticed a guy running a threading cycle ipm on a lathe. This may be just because of how you could change the rpm without have to mess with the feed idk. I really hadn't given this any thought before now.

Does Fanuc lathe controls have override enabled/disabled M codes? I don't have any manuals on hand at the moment.

Brent
 
twr said:
Brent it seems to spin fine but I will try G41 can't hurt.
Click to expand...

M41... I think because the machine is in second gear you can't achieve 35 rpm. You've commanded G97 S35 M3 and a G32 Z- E.0714 and the control may think the spindle is turning at 35rpm but the minimum rpm in M42 second gear may be faster then that giving you the appearance it is feeding faster then it's supposed to but what's happening is the tap is being sucked into the part because the of a faster rpm?

Does that make sense? Maybe not the case but that's my train of thought. Lol...

Brent
 
Just out of curiosity, have you programming it to feed faster than it should, to comp for it tensioning your holder?

It might tell you if its just not feeding at the right amount, or maybe its ignoring your programmed feed.

Do you have a tachometer to check chuck RPM?
 
Well don't know what the fuck but it's good now!!! I used G41 but I played with the adjustment on the tap holder and all is good in aluminum, stainless is for Sunday and see how it works out!! Fingers crossed!!
 
ManualEd said:
Just out of curiosity, have you programming it to feed faster than it should, to comp for it tensioning your holder?

It might tell you if its just not feeding at the right amount, or maybe its ignoring your programmed feed.

Do you have a tachometer to check chuck RPM?
Click to expand...

Ed i was feeding in and out at the same .0714 ipr and yes the tach says it's the correct speed in low gear. I am not sure but i think it also has something to do with dry run being switched ON. After playing with the adj.on tap holder and G41 and dry run off it was fine. Stainless will be a pita i beat and that's what these are going to be machine out of.
 
You must log in or register to reply here.

Similar threads

E
What is projection on a tension and compression tap holder?
Replies
5
Views
264
EyeEmTrash
E
A
NPT Thread Possibly Damaged
Replies
9
Views
539
Bill D
B
J
NPT threads generating shavings and flakes during use
2 3
Replies
41
Views
2K
William Lynn
W
E
Help with a Lathe tapping cycle
Replies
7
Views
440
DouglasJRizzo
DouglasJRizzo
M
Haas lathe stops feeding when changing speed. Is there a parameter to change this?
Replies
10
Views
563
Ox
Ox








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top