G33 Threading help


Adrian Payne
 

Hello All
Sorry to ask a probably stupid question but I cannot find a post with the answer.
When I try to run the simple threading code below, as found elsewhere on this group, I get an error. Lead parameter i required. What have I done wrong?
G0 X.56 Z.25
G33 X.49 Z-.75 K.05
X.48
X.472
...etc
I can run G76 without a problem.
Many thanks.
Adrian.


Dave Kowalczyk
 

Good morning Adrian!

  Glad to help.  For G33, each axis called out (e.g., XYZ) requires a lead parameter (IJK) to specify how far per revolution to move.  So the program is asking for an "I" to go along with the "X."

  Presumably you're cutting tapered threads for piping or similar, so your code will be akin to:

G0 X.56 Z.25
G33 X.49 Z-.75 K.05 I0.0035
etc...

  Hope this helps!

-Dave Kowalczyk
Author, TurboCNC


Adrian Payne
 

Hello Dave
Many thanks for getting back to me. This was to be a parallel thread, I was hoping to use G33 instead of G76 so I could set up spring passes with the same X setting.
Can I simply use I0.0 for parallel thread.
Adrian



Sent from my Samsung Galaxy smartphone.

-------- Original message --------
From: Dave Kowalczyk <dkowalcz@...>
Date: 09/07/2020 12:23 (GMT+00:00)
To: turbocnc@groups.io
Subject: Re: [turbocnc] G33 Threading help

Good morning Adrian!

  Glad to help.  For G33, each axis called out (e.g., XYZ) requires a lead parameter (IJK) to specify how far per revolution to move.  So the program is asking for an "I" to go along with the "X."

  Presumably you're cutting tapered threads for piping or similar, so your code will be akin to:

G0 X.56 Z.25
G33 X.49 Z-.75 K.05 I0.0035
etc...

  Hope this helps!

-Dave Kowalczyk
Author, TurboCNC


Dave Kowalczyk
 

Adrian:

  For parallel threads, just spec Z and K only.  G33 will go to the Z coordinate, timed to the spindle to give K/rev from the start point.  It stops there, so you need to program the return passes yourself, for example:

G0 X.56 Z.25
G0 X.49
G33 Z-.75 K.05
G0 X.56
G0 Z.25
G0 X.48
G33 Z-.75 K.05
etc...

  Using an I of 0.0 is somewhat degenerate, when I tried it on my machine here it moves X and Z together to match (much the same as if the I was calculated to give an exactly even increment per rev) - but I'm not immediately sure that result can be guaranteed to occur if it's not fully specified.  Multi-axis G33 is typically for tapered threads, wire winding and gear hobbing (a form of so-called "digital cam").  Single axis G33 is also useful for "trick" threading like cutting on alternating flanks or multi-start threads by varying the start point.

  You might consider a "follow up" G33 pass after G76 has done its work for your spring passes/cleanup to avoid writing a lot of g-code. 

  Or pick a smaller initial first pass infeed "D" for G76, it'll cut approximately equal areas per pass so the final passes end up being fairly small increments in X (i.e., "close enough" to a proper spring pass).

  Have fun!

-Dave Kowalczyk
Author, TurboCNC


Adrian Payne
 

Hello Dave
Many thanks for taking the time to reply to me and thanks for the information. Adding a couple of G33 spring passes to a G76 threading line is probably the most efficiently code.
Many thanks again.
Adrian



Sent from my Samsung Galaxy smartphone.

-------- Original message --------
From: Dave Kowalczyk <dkowalcz@...>
Date: 10/07/2020 02:22 (GMT+00:00)
To: turbocnc@groups.io
Subject: Re: [turbocnc] G33 Threading help

Adrian:

  For parallel threads, just spec Z and K only.  G33 will go to the Z coordinate, timed to the spindle to give K/rev from the start point.  It stops there, so you need to program the return passes yourself, for example:

G0 X.56 Z.25
G0 X.49
G33 Z-.75 K.05
G0 X.56
G0 Z.25
G0 X.48
G33 Z-.75 K.05
etc...

  Using an I of 0.0 is somewhat degenerate, when I tried it on my machine here it moves X and Z together to match (much the same as if the I was calculated to give an exactly even increment per rev) - but I'm not immediately sure that result can be guaranteed to occur if it's not fully specified.  Multi-axis G33 is typically for tapered threads, wire winding and gear hobbing (a form of so-called "digital cam").  Single axis G33 is also useful for "trick" threading like cutting on alternating flanks or multi-start threads by varying the start point.

  You might consider a "follow up" G33 pass after G76 has done its work for your spring passes/cleanup to avoid writing a lot of g-code. 

  Or pick a smaller initial first pass infeed "D" for G76, it'll cut approximately equal areas per pass so the final passes end up being fairly small increments in X (i.e., "close enough" to a proper spring pass).

  Have fun!

-Dave Kowalczyk
Author, TurboCNC