G32 Taper to straight threading

Hello, looking for insight on the following. When taper threading with G32, does the feed rate vary from the pitch of the thread? For example, I am programming a screw with a 1.5mm(.0591") pitch thread. The tip of these screws are pointed and the thread follows this pointed tip then continues straight on the OD. My code that is being posted gives a different feed rate for the tapered portion than it does for the straight. It doesn't vary much, maybe .0015" difference at most. I have run the threading cycle leaving the different feed rates in there and also changing them to be the same. I am having a hard time seeing any difference in the threads.

I have made plenty of bone screws with tapered to straight threads but this question has always come up.

I have run the threading cycle leaving the different feed rates in there and also changing them to be the same. I am having a hard time seeing any difference in the threads.

Click to expand...

Be more exaggerated in your F values and try aggin.



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

Think Snow Eh!
Ox

I'm sorry, I don't follow what you are saying. I'm simply just asking if the threading feed rate on a taper would vary from a straight thread to get the correct pitch on the taper.

Poofius said:

Hello, looking for insight on the following. When taper threading with G32, does the feed rate vary from the pitch of the thread? For example, I am programming a screw with a 1.5mm(.0591") pitch thread. The tip of these screws are pointed and the thread follows this pointed tip then continues straight on the OD. My code that is being posted gives a different feed rate for the tapered portion than it does for the straight. It doesn't vary much, maybe .0015" difference at most. I have run the threading cycle leaving the different feed rates in there and also changing them to be the same. I am having a hard time seeing any difference in the threads.

I have made plenty of bone screws with tapered to straight threads but this question has always come up.

Click to expand...

This is interesting and was kinda hoping a few more people would chime in on this. Maybe Ox could add some clarification to his last post, not sure I understand the point hes making.

I know very little about swiss lathes, know even less about bone screws. For what it is, a .0015 difference probably isn't going to matter much either way on its function.

I dont have your answer but would ask myself if I wasn't using computer generated code and was programming manually would you use different feed rates? I wouldn't.

Then again if your cam software is geared specifically towards orthopedics/bone screws then its possible there's some bone screw making technology going on here.

Yon need to add your location its the rules here. Welcome to the board.



Brent

I think Ox is saying change one of the feed rates (probably the tapered portion) to either an extremely fast lead (try something like .08 or so), or an extremly slow lead (.02/rev?). It should become apparent then. The difference of .0015 would probably be very hard to spot over such a short distance.

Ok I kind of see what he was getting at. I have to agree I would not use different feed rates if programming by hand. The software isn't specific to bone screws or any other part, just swiss. I have been searching for information on G32 but I come up empty everywhere I look. I am wondering if the feed on G32 affects only Z moves.

Also, doesn't help that threads like this cannot be run through a gage or mating part.

Edit: Maybe it would help if I post some code. Below is the posted code from my CAM. There is actually a bigger difference in feeds for this particular thread, the code I referenced in my OP was for a thread with less of a taper.

G0 Z-0.0548 T04
X0.2024
X0.0922
G32 Z0.0709 F0.0591
G32 X0.2338 Z0.2553 F0.0633
G0 X0.3439
X0.2024 Z-0.0542
X0.0829
G32 Z0.0709 F0.0591
G32 X0.2244 Z0.2553 F0.0633
G0 X0.3439
X0.2024 Z-0.0536
X0.0742
G32 Z0.0709 F0.0591
G32 X0.2158 Z0.2553 F0.0633
G0 X0.3439
X0.2024 Z-0.053
X0.0664
G32 Z0.0709 F0.0591
G32 X0.2079 Z0.2553 F0.0633
G0 X0.3439
X0.2024 Z-0.0525
X0.0592
G32 Z0.0709 F0.0591
G32 X0.2008 Z0.2553 F0.0633
G0 X0.3439
X0.2024 Z-0.052
X0.0521
G32 Z0.0709 F0.0591
G32 X0.1937 Z0.2553 F0.0633
G0 X0.3439
X0.2024 Z-0.0515
X0.045
G32 Z0.0709 F0.0591
G32 X0.1866 Z0.2553 F0.0633
G0 X0.3439
X0.2024 Z-0.051
X0.0379
G32 Z0.0709 F0.0591
G32 X0.1794 Z0.2553 F0.0633
G0 X0.3439
X0.2024 Z-0.0505
X0.0307
G32 Z0.0709 F0.0591
G32 X0.1723 Z0.2553 F0.0633
G0 X0.3439
X0.2024 Z-0.05
X0.0236
G32 Z0.0709 F0.0591
G32 X0.1652 Z0.2553 F0.0633
G0 X0.3439
X0.2024 Z-0.05
X0.0236
G32 Z0.0709 F0.0591
G32 X0.1652 Z0.2553 F0.0633
G0 X0.3439
G0 X0.2024 Z-0.05

Poofius said:

Hello, looking for insight on the following. When taper threading with G32, does the feed rate vary from the pitch of the thread? For example, I am programming a screw with a 1.5mm(.0591") pitch thread. The tip of these screws are pointed and the thread follows this pointed tip then continues straight on the OD. My code that is being posted gives a different feed rate for the tapered portion than it does for the straight. It doesn't vary much, maybe .0015" difference at most. I have run the threading cycle leaving the different feed rates in there and also changing them to be the same. I am having a hard time seeing any difference in the threads.

I have made plenty of bone screws with tapered to straight threads but this question has always come up.

Click to expand...

With most controls, and using constant Lead G32, when the included angle between the Spindle Centre Line and the tapered surface is =< than 45deg, the Feed is applied to the Z axis. Accordingly, the pitch of the thread along the tapered face will vary when the taper is varied.

Regards,

Bill

angelw said:

With most controls, and using constant Lead G32, when the included angle between the Spindle Centre Line and the tapered surface is =< than 45deg, the Feed is applied to the Z axis. Accordingly, the pitch of the thread along the tapered face will vary when the taper is varied.

Regards,

Bill

Click to expand...

There you have it OP, sounds like the feeds should be different.


Brent

That's not how I read it.


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

Think Snow Eh!
Ox

How do you read it? His feeds should be the same along the strieght and the taper or can they be different? I may be confused..


Brent

the Feed is applied to the Z axis

Click to expand...

I believe that "Z axis only" is inferred there. No?

Making the actual feed on the hippopotamus slightly faster than programmed to accommodate the increase in X without changing pitch length.

No ???


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

Think Snow Eh!
Ox

You've got to be shittin me..hippopotamus lol..thats a hoot!! I damn near spit coffee all over the table.. Ok you might be right, Hell I dont know.. you should have been a comedian tho..


Brent

So, why would you want the screw pitch to follow the hippo and not be constant in Z? Seems like the pitch of the point and the pitch of the straight screw would fight each other if not constant in Z.

As I read what he posted (and would seem to make sense)

The Z pitch IS constant and as programmed "in Z".

The only reason that the "actual" is more is the added traverse of X.

If you buy a tapered 1/2-13 tap* (No clue what the app would be, and never [knowingly] ever seen one, but ....) you would expect the thread pitch to be 1/13 in Z the whole way eh? Even tho if you add the traverse of the grinders X travel - it actually "fed" faster than that along the hypo to keep the Z pitch accurate.


So the feedrate of the CAM is showing "actual" and apparently not what needs to be programmed.


FOS?


Maybe Bill will draw a map for us after get's his coffee and doughnuts?



* I guess a NPTF tap would be a better example @ 1* 47'.


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

Think Snow Eh!
Ox

I could be and probably am wrong but....I think what Ox was trying to say in his first post was exaggerate it as in the TPI to a much more course thread on a setup or scrap piece just to see what you are looking at, and what Bill was saying is the callout for TPI is in relation to the Z axis not necessarily the hippopotamus know what I mean? To be measured as a linear dimension, so how many TPI along the Z axis not along the hippopotamus.

So IMO to the OP no the feedrates should be the same.

Robert my ±2

Heck - I would have cut air for the trial.
No need to waste material.



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

Think Snow Eh!
Ox

Yeah maybe a map would help. Like I stated I my first post if I was programming manually I'd ues the same feeds on both the strieght and the taper if the call out on the print was the same on both surfaces.


Brent

My understanding is that any time the X is less than Z in a G32 move, the feed is applied to Z. The X just follows along.

So, if you program:

G0 X0.0 Z0.0
G32 X1.0 Z-2.0 F.1

It would feed at .1/rev in Z. The X feed would be whatever was required to keep up with Z.

ewlsey said:

My understanding is that any time the X is less than Z in a G32 move, the feed is applied to Z. The X just follows along.

So, if you program:

G0 X0.0 Z0.0
G32 X1.0 Z-2.0 F.1

It would feed at .1/rev in Z. The X feed would be whatever was required to keep up with Z.

Click to expand...

Yes that make perfect sense to me. The X would feed at whatever it ends up being to maintain the Z feed. I think..



Brent

yardbird said:

Yes that make perfect sense to me. The X would feed at whatever it ends up being to maintain the Z feed. I think..



Brent

Click to expand...

In a sense that is true but have you ever accidentally used G96 in a threading operation? If you know what I mean.....well then you know what I mean, the cutter needs to move along the Z axis at so many inches per rev regardless of the diameter. That is part of the reason CNC lathes use encoders. If you cut 10" diameter thread with 8 pitch and a 1" diameter with an 8 pitch you still end up with a .125" lead. I understand what you guys are getting at but I think you are overthinking it. Just because it is tapered and straightens out doesn't mean the feedrate will change or the RPM. That is part of the magic of an encoder.

My understanding is that any time the X is less than Z in a G32 move, the feed is applied to Z. The X just follows along.

Click to expand...

I am not really following this one, so are you saying that if the Z value is less than the X value the feedrate is applied to the X value? If that is what you're saying you are wrong my friend. What if your part were 10" diameter but needed to feed to Z- 5"