G02 & G03 in MDI

Hi guy's I'v been trying to use G03 in MDI to put a bellmouth at the start of a premachined bore.

My lathe is in radius mode.
The bore is 38.9mm. dia.. The radius of the bellmouth is 11.80mm.
The bellmouth Radius starts at X27.535 Z0. Which is where I position the cutter before commanding the G03.
The radius ends at X19.45 Z-11.20.
My centre offsets are I 3.715 J -11.20
My G03 is therefore X19.450 Z-11.200 I3.715 J-11.200 F60
But I get the error message Start=(X22.535 Y0.000), Center=(X31.25 Y-11.200) End=(X19.45 Y0.000), r1=11.8001 r2=16.269

Why is it showing Y instead of Z
Why is the end point Y0.000 instead of Y-11.200 or more appropriatly Z-11.200.
And I would have thought the centre offsets would have be in incremental i.e. X3.715 Y-11.200 not Absolute as shown or does EMC2 internally work in Absolute.
And whats wrong with my Gcode. or am I missing something here.

Thanks Rod

Rod,

Are you in the XZ plane with G18?

Also note that the G2/3 rotate about the imaginary Y axis plus end so if your setup is normal you have to lay on the floor and look up for G2/3 to seem normal.

Another thing is diameter mode... if your in diameter mode X is diameter but X offset (I) is in radius.

I was struggling the last few days on my lathe with this too.

John

Thanks for the reply John as I said my lathe is in radius mode. I also used the stepcon wizard to set it up so as I selected the lathe option there I thought I would'nt need a G18. But I'll give this a try today.
When this first happened I thought that maybe stepcon had failed to set it in lathe mode so I checked and its definitly in lathe mode there. I also looked at my ini. file and did notice that although XZ is there the number of Axis was still set at 3. So I tried to reduce this to 2 but when I restarted Axis it threw up an error about the number of axis so I put it back to 3.

Oh yes I did try this with a G02 as well the result was the same.
As I said I'll give the G18 a try today although I,m still unsure why I should need this as Axis should know that I'm in lathe mode and therefore surely always in G18.
Also I have run programs with G02 & 3 and have never used a G18 yet so is this something that is only needed in MDI.

Curious, Rod.

Rod,

While the user interface Axis "knows" it is in lathe mode EMC has no such thing as lathe mode and defaults to G17 XY plane when started. While you can put G18 in your ini file that won't stop another g code program from changing it so it is always best practice to put all your setup g codes in the preamble of your program. I include a standard line similar to G7 G18 G20... as the first line of all my g code files.

Even though you only have two axis on a lathe they are 0 and 2 so you need to load 3.

I'd bet your offsets are not correct as that it the hardest thing to get right.

Just drawing your arc in ACAD and I have the following coordinates.

Arc Start X27.535 Z0
Arc Center X31.250 Z-11.1999
Arc End X19.450 Z-11.200

Doing the math I get
X offset 3.715
Z offset -11.1999

So I end up with:
G8 G18 G21
G0 X27.535 Z0
G3 X19.45 Z-11.2 I3.715 K-11.200

This give me an arc of about 270 degrees... not sure your wanting that. Changing to G2 give me about 90 degrees.

Scrolling down to compare I this I see your using the XY offsets IJ instead of the XZ offsets of IK... so your math was sound.

www.linuxcnc.org/docview/html//gcode_main.html#sub:G2,-G3:-Arc

John

Thanks John I think I understand why it needs the G18 now. I also posted this on CNC zone and a reply from a guy on there pointing to the error of my ways with I J sorry K did G18 G03 X19.45 Z-11.2 I3.715 K-11.2 as he suggested and everything worked fine. I also did another Gcode entering a wrong dimension in my off sets just to test it, it through the error as expected but this time had the Z axis instead of the Y. Now I just have to log it in my brain for recall later. Not an easy task at my age.

Thanks for your help Rod

I hope to soon have a morphed version of my arc buddy for lathes. If you have a mill to you might want to take a look at it on the wiki.

John