G91 G code question

[beekeep]

I did a cad drawing in rhino and saved it as a dxf file. I imported the drawing into lazycam. Lazycam posts the g code in incremental mode. It looks like it uses a G91.1 code to go to the incremental mode. If I edit the g code and remove the .1 I get a strange tool path curve. My question is "What does the .1 do?"

Thanks
Greg Ferris

[HuFlungDung]

Wouldn't the interpretation of G91.1 be up to your controller? What kind of machine are you running? What post processor are you using? Do they match?

[beekeep]

I am using mach 3 mill.

[neilw20]

Section 10.7.26

[HuFlungDung]

So does that exerpt from the manual mean that Mach won't do absolute positioning with incremental arc centers, which is the way most cncs are designed to work? Or does plain old G90 do that?

[ger21]

You need to have a G90 for absolute movements along with the G91.1 for incremental IJ arcs.

When you change G91.1 to G91 your changing two different things.

G90= Absolute positioning
G91 = Incremental positioning.
G90.1 = Absolute IJ
G91.1 = Incremental IJ

[beekeep]

the program that I saw G91.1 in didn't have any arcs in it. All cuts were straight lines so there is no need for such a code. In a previous progam, again all with straight lines, when I ran it on mach 3 it curved all the joining lines. I'll have to go back and give that G code a closer look. I'm thinking that I have a fillet button turned on in lazycam.

[ger21]

Originally Posted by beekeep the program that I saw G91.1 in didn't have any arcs in it. All cuts were straight lines so there is no need for such a code.

It doesn't hurt anything for it to be there. ANd when you do have arcs, it assures that Mach will cut them correctly.

Originally Posted by beekeep In a previous progam, again all with straight lines, when I ran it on mach 3 it curved all the joining lines. I'll have to go back and give that G code a closer look. I'm thinking that I have a fillet button turned on in lazycam.

Most likely you're seeing rounded corners caused by CV mode.

[sinha_nsit]

Unless you are in "exact stop" mode, the execution of the next block starts, the moment the tool comes within "in-position" distance of the programmed end point in the current block. This causes rounding of corners. If this is not acceptable, reduce the in-position value through a parameter, or run the program in exact stop mode.

Most CAM softwares approximate arcs by small straight line segments.