G91 in canned cycles

[Ashish B]

Hi All

Suppose we have a program -
G91 G81 G98 X4 Y5 Z-0.6 R1.8 L3

Than does G91 gets cancelled after completion of the Canned cycle ?


& G90 is followed thereafter

Thanks,
Ash

[Torsten]

G90 and G91 are modal, they stay in effect until changed by the other.
So is G81, you want to call G80 cycle cancel when done.

[Ashish B]

But IS generally G91 is used in conjunction with any canned cycle....?

What is the industry Standard ?


Ash

[tobyaxis]

But IS generally G91 is used in conjunction with any canned cycle....?

What is the industry Standard ?


Ash

No, G91 is Incremental Coordinates and G90 is Absolute Coordinates Programing

[Ashish B]

Ya, I know that G90 & G91 represents Absolute & Incremental Programming.

But while writing canned cycle, what is the pattern followed. Is G91 used while writing a canned cycle.

A example of canned cycle will be a favour....

Ash

[tobyaxis]

Ya, I know that G90 & G91 represents Absolute & Incremental Programming.

But while writing canned cycle, what is the pattern followed. Is G91 used while writing a canned cycle.

A example of canned cycle will be a favour....

Ash

Using G91 in a Canned Cycle is up to the programmer. Personally I do not use G91 in a Drilling or Boring Cycle because I see no point.

I have however used G91 for Sub-Programs. An example would be if the Stock/Material is too thick and will require many roughing passes because the shell mill only has a max DOC of .15 and I have to remove 1 inch of stock.

The first rule of CNC Programming is that the only limit is the programmer and their imagination.

[Andre' B]

Ya, I know that G90 & G91 represents Absolute & Incremental Programming.

But while writing canned cycle, what is the pattern followed. Is G91 used while writing a canned cycle.

A example of canned cycle will be a favour....

Ash

If you are writing you own canned cycles one of the first things you would do is store the current state of G90/91 then switch it to what you want to use, do the cycle then put the G90/91 back to what it was before giving control back to the g-code program.

[Ashish B]

Well i don't fall into experitise category to write a self canned cycle with help of macro programming.....


I understand that there is no sense to use G91 in canned cycles & G90 is the best & industry standard for any canned cycle.


Thanks a Lot, FRIENDS

Ash

[Torsten]

Well i don't fall into experitise category to write a self canned cycle with help of macro programming.....


I understand that there is no sense to use G91 in canned cycles & G90 is the best & industry standard for any canned cycle.


Thanks a Lot, FRIENDS

Ash

Well I have not used this a lot but there are reasons one may use G91 in a Drill cycle.
Example:
G91 G81 X1. Y0. Z-1. R.1 F3. L6

Would Drill six holes along the X Axis, spaced 1. inch apart.
I don't know if your control supports this repetition command.
Even if, CAM processors usually are not setup for this and would use the longer sequence of posting the 6 locations in G90 mode.

[Ashish B]

Hmmm....

Getting your point....Lenghty but a must preferred enggineering practice.

Ash

[Superman]

The G90/G91 codes switches the machine "state", same as the inch/metric or G94/G95 codes

It can be used on 1 block ( line of code ), and is executed before any movement occurs, like the feedrate (F) address is executed before moving.
or
on a line by itself

Your manuals should also tell you the protocols of execution, when that address is actually performed, no matter where you have placed it on the line of code.
ie G1 M9 G91 X5. Y0. Z0. F.01 G95 G40 ( this is a little mixed up, but the control will place and execute it in a set order of priority, ie G91 G1 G95 G40 F will happen before movement, M9 after target is reached )

as stated earlier- it is modal---( active until another code from the same "group" is run )
all codes have some sort of "group" policy ( refer to your machine manual )
ie G0/G1/G2/G3...make-up 1 group
G94/G95............are another
G17/G18/G19......are yet another

Generally, only 1 code from each group can be stated on the same line, but this means it must also fulfil it's own critria. ie G1 G4 X1.Y0. is not permitted as G4 is a time/dwell and X is the address the time value is read from...not an actual co-ordinate you also want to feed to.

IMO it would be advisable to place the change of machine state on it's own line, instead of "losing it" in amonst other code, and being missed by an operator.

Also
Some machine controls do not allow more than 1 G-code per line, this means that your example of G91 G81 G98 would create alarms.

[Ashish B]

But on my machine, if you command -


G90 X40.0 G91 Y12.0 ...it will move 40 in absolute mode & 12 in incremental mode

Also, if you command


G20 X1.0 G21 Y100.00....will move 1 inch in X axis & 100 mm in Y axis


WITHOUT ANY INTERRUPTIONS.

Strange...