Absolute and Incremental Toegether

[johnd]

I am cutting a constant pitch screw with varying root diameter with constant pitch on my mill using the 4th axis .
The screw has a major root diameter (.325") for 6 turns and then transitions to a minor diameter (.265 ") for 8 turns.
From there the screw is cut an additional 6 turn at the minor diameter.
Right now I am cutting in one direction from left to right .
After completing the pass I am raising the spindle up to a clearance height and then moving X and A back to there initial
starting position to the left..
A lot of time is wasted returning A axis back to 0,0 to start the next pass.
Right now every line is written in absolute mode.
Can I combine G90 and G91 on the same command line such that X and Z moves would be in absolute and
A moves would be in incremental ?

Similar Threads:

• Newbie- 0m-a G90 absolute G91 incremental no difference?
• Need Help!- From incremental to Absolute,
• Problem- Incremental Vs Absolute mode
• Absolute or Incremental
• Absolute and Incremental

[sinha_nsit]

I do not think so.
G90 and G91 belong to the same G-code group, and only one code from a group remains active at any time.
You may, however, experiment and let us know the result: G90 G00 X_ Z_ G91 A_

[mactec54]

I am cutting a constant pitch screw with varying root diameter with constant pitch on my mill using the 4th axis .
The screw has a major root diameter (.325") for 6 turns and then transitions to a minor diameter (.265 ") for 8 turns.
From there the screw is cut an additional 6 turn at the minor diameter.
Right now I am cutting in one direction from left to right .
After completing the pass I am raising the spindle up to a clearance height and then moving X and A back to there initial
starting position to the left..
A lot of time is wasted returning A axis back to 0,0 to start the next pass.
Right now every line is written in absolute mode.
Can I combine G90 and G91 on the same command line such that X and Z moves would be in absolute and
A moves would be in incremental ?

No you can't have the 2 active at the same time but you could use them on any individual lines one will cancel the other

[deadlykitten]

hy johnd

A lot of time is wasted returning A axis back to 0,0 to start the next pass

is the rapid of the 4th axis really-really slow ? what is it's rapid speed ?

repositioning movement is done in feed or in rapid ?

during threading, is the 4th axis used in positioning mode ( degrees / minute ), or like a spindle ( rpms / minute ) ?

if your code works in positioning mode ( degrees / minute ), then have you tried to "start" and "end" at same spindle phase ? so to eliminate the need to reposition the 4th axis between passes ?

Can I combine G90 and G91 on the same command line such that X and Z moves would be in absolute and A moves would be in incremental ?

it is possible to achive this somehow ( by using a soubroutine, etc ), but i don't believe that you really need this trick

i hope that all those questions listed above will light a spark / kindly

[angelw]

I do not think so.
G90 and G91 belong to the same G-code group, and only one code from a group remains active at any time.
You may, however, experiment and let us know the result: G90 G00 X_ Z_ G91 A_

No you can't have the 2 active at the same time but you could use them on any individual lines one will cancel the other

Hello sinha and mactec54,
In the way you can combine Absolute and Incremental with a lathe control, (G00 X100.0 W-30.0) so are you able to do the same with a mill control using G90 and G91 in the same Command Block. The following example is quite legal and results in a combined Absolute move to X100.0 and an Incremental move of Y-10.0.

G00 G90 X100.0 G91 Y-10.0

One caution that should be observed is that on completion of the above example Block, the control will be in G91 (Incremental) Mode.


Regards,

Bill

[deadlykitten]

hello angel

G00 G90 X100 G91 Y-10

same (iso) code may perform differently, depending on control brand

each code line ( block , etc ) has different words inside it, and some controls may be sensitive to words order; in such a case, that code will work

a conflict may appear on controls that are not sensitive to words order, because there are at least 2 words that belong to the same family

G00 X100 W-30

such a code may be executed identicaly on both types of controlers, because G90 is "modal", while W is "one shot"

kindly

[angelw]

hello angel



same (iso) code may perform differently, depending on control brand

each code line ( block , etc ) has different words inside it, and some controls may be sensitive to words order; in such a case, that code will work

a conflict may appear on controls that are not sensitive to words order, because there are at least 2 words that belong to the same family



such a code may be executed identicaly on both types of controlers, because G90 is "modal", while W is "one shot"

kindly

I see you're still demonstrating your lack of knowledge.



G90/G91 are from the same G Code Group



Yet they can be combined in the same Block. The above are extracts from a Fanuc Manual, but Haas, Mazak, Yasnac and many other controls are the same. It is, however, not allowed to program G90/G91 in the same Block with an Okuma control.

[deadlykitten]

Yet they can be combined in the same Block. Haas, Mazak, Yasnac and most controls are the same

because the controller is sensitive to words order

It is, however, not allowed to program G90/G91 in the same Block with an Okuma control

because the controller is not sensitive to words order, at least for g-codes


please, will you share the full list of those G groups ? kindly