Newbie- EIA Theata offset possible?

[Chris_A]

Hi all, first post here.

I did my first EIA program today and called it up as a sub in Mazatrol but unfortunately the offset units I have in there do not also change the sub program.

SO my question is, do I need to know a G-code that will off set the sub IN the EIA? or am I going about this all wrong?

LOL, please be a little patient, I am COMPLETELY new to this area of CNCs

TIA!
Chris

[psychomill]

If you're looking for the EIA version of Theta.... Yes, it's called G68. Look up coordinate rotation in the programming book. Basically, before you run your cuts, you'll need to tell it something like:

G68 X0 Y0 R(angle)

Then a G69 to cancel before jumping back into Mazatrol program.

Do you need to jump into a EIA sub if you're starting from Mazatrol?

[Chris_A]

Exellent! thanks! I'll take a look at the book when I get into work tomorrow. Trying to find a good explenation in there is... "difficult" some times .

Ok so G68 and G69, now when I cancel at the end of the EIA it's as so:
G69
M99
Not the other way around correct?

Also would it be possible to have more than one G68's in one EIA program? would I have to go G69 and then G68 again after?

The reason behind this is I have a part that the roughing passes through Mazatrol were pretty inefficent for machining time. Doing it through EIA has cut the time by 2/3rds. What I'd like to do though is run all of the offsets in one EIA for the roughing, then transfer back to the Mazatrol for the finishing (mostly because it's already been tested and works... so yeah, it's there ).

Thanks!
Chris

[psychomill]

If the roughing is all in the same time frame, you don't have to keep toggling the G68/G69 between passes. The only time would be is if you're say changing work offsets. Then you need to cancel, pick up new work offset then initialize a new G68 command.
You can G68 inside of a G68 but not if you're changing work offsets. Keep in mind too, when you G68 inside of a G68, the second command is actually rotating on top of what you've already rotated in the first command. If you need to only change the main rotation angle, cancel the first one then rotate to a new position (just to keep things simple)...

G69 M99

That would be correct...

[Chris_A]

That's perfect, thanks!

Finished the program today and did a dry run, worked like a dream. I did have a little "head scratch" with the G68 coordinates lol, eventually I figured out the period after each axis .

All in all the EIA saved almost 2 hours off the tool path using Mazatrol.

Thanks again!
Chris

[psychomill]

Keep in mind, you can G68 rotate your program from "any" coordinate point. The XY is relative to your work offset point (being your part origin). If you wanted to rotate from a different point on the part, simply put in the rotation point such as:

G68 X2.5 Y-3.662 R-42.6

... and Yes, the rotation value can be a negative as well to 'go the other way' so to speak. So instead of saying R270. , you could say R-90. . Depends on how you want the programming viewed by an operator or set up machinist is how I generally determine this. Or if I'm repeating a pattern in a particular direction, I may use a negative so that the operator/Set up machinist has an idea which direction the pattern is going to move (order of operations). None the less, it's gets to the same place....