G17, G18 and G19 explanation please

[cossiegaz]

Can somebody explain to me exactly what the purpose is of the G17, G18 and G19 codes please?
I am aware that they somehow relate to which of the machine axis are being used but i get confused by the fact that a G17 specifys X and Y axis yet the program being excecuted will use X, Y and Z axis so why is there not a code to specify all 3 axis?

[Geof]

You have it correct, G17 is XY plane, G18 is XZ plane and G19 is YZ, but it really only applies when you are doing circular interpolation; G03 or G02.

In G17 your circle goes around the Z axis, in G18 around the Y axis and G19 around the X axis.

[HuFlungDung]

I think I used a G18 or a G19 once in my programming life thus far, and even then, it was just a manual tryout

Would it not be the case that arc commands in the various planes all have different formats?
G17 G02 X,Y, I,J
G18 G02 X,Z, I,K
G19 G02 Y,Z, J,K

Hence my question: why wouldn't the control just know what plane to execute the arc in by its syntax? Of course, modal coordinates could never be assumed, I guess, but still....

[cossiegaz]

Originally Posted by Geof You have it correct, G17 is XY plane, G18 is XZ plane and G19 is YZ, but it really only applies when you are doing circular interpolation; G03 or G02. In G17 your circle goes around the Z axis, in G18 around the Y axis and G19 around the X axis.

So does this mean that G18 and G19 will only ever be used on a machine with more than 3 axis as thats the only sort of machine that will allow you to produce a circle around the X or Y axis whereas on a 3 axis vertical mill you will only ever be able to produce a circle around the Z axis so would only ever use G17?
And like HuFlungDung said - Why would the machine not just know what axis to use? Obviously it needs to be told otherwise we wouldnt use these codes, but i dont understand why.

[dcoupar]

Remember, these codes were invented when controls weren't as smart as they are now.

G17, G18 & G19 also select which two axes get cutter comp when you activate G41 or G42 (remember, unless you buy the option, you only get two at a time) and which axes do what when drilling with canned cycles.

[Superman]

dcoupar is on the money

Another way to look at the G17/G18/G19 issue is that:
there is 6 axes of motion
the first 3 are linear ( XYZ )
the remaining 3 are rotational ( ABC ), around XYZ

On a drill cycle when all XYZ are defined, which 2 are the positioning axes, and the remaining axis is the drilling line ( eg G18 XZ=positioning Y=drill line ) this is useful to know when programming for a right-angled head

Mills use the plane command as a point of view that the arc is described as " a true arc ".
An arc with it endpoints and centre points in the X,Y or Z plane would be seen as a line in either of the other planes.

Think about the motion of a skateboarder in a 1/2 pipe, if you wanted a cutter to form this inside radii like the skater, then G17 is wrong, as with using G17, it would only create a big C.
If viewed from the top, the skater is only moving in a line, but we all know he's moving in an arc when viewed from the side

[beege]

Originally Posted by HuFlungDung Would it not be the case that arc commands in the various planes all have different formats? G17 G02 X,Y, I,J G18 G02 X,Z, I,K G19 G02 Y,Z, J,K

This is correct. On machines that have helical interpolation, all of the words X,Y,Z, I,J,K could be used on one line. The plane selection G17 18 and 19 dictate which plane the arc is generated, and which axes create each arc.

And yes, G41 and G42 are cutter offsets applied in each plane.
And yes, (parameter enabled) canned cycles like drilling allow a peck by the third axis (G17-Z axis drilling, G18-Y axis drilling, etc).

As a visual aid, picture the contour you need to cut as you are standing in the plus-plus-plus quadrant of the contour you want to generate, looking back at the origin. On the XZ plane, a G02 will look counterclockwise from the front of the machine, because you are on the backside of that quadrant. Same goes for comp. The offset will need to be reversed because of that same viewpoint.

I once had a machine with spindles in three directions, one pointing from the Z+ (as any VMC), and some pointing from Y+, and some pointing from X+, so we got used to programming everything in all planes. Even tool lengths!

G19G43H01X1.
G18G43H11Y0.
G17G43H21Z1.

HTH

[HuFlungDung]

Ah, yes, thanks Beege, the requirements for helical interpolation would require the plane to be specified.

[Torsten]

Originally Posted by HuFlungDung I think I used a G18 or a G19 once in my programming life thus far, and even then, it was just a manual tryout Would it not be the case that arc commands in the various planes all have different formats? G17 G02 X,Y, I,J G18 G02 X,Z, I,K G19 G02 Y,Z, J,K Hence my question: why wouldn't the control just know what plane to execute the arc in by its syntax? Of course, modal coordinates could never be assumed, I guess, but still....

You could not rely on I and J or I and K or J and K been called out, because only one of each may be called out if the other happends to be zero.
The G17, G18 or G19 code lets the controller know wich plane to use for circular interpolation.

[cossiegaz]

Thanks for the replies, ive read them over and over again and am slowly getting my head round it a little more each time i read through.
Whilst the subject of helical interpolation has been raised can i also ask exactly what that means as it may make it clearer to me why the planes need to be specified, would it be referring to circular interpolation whilst also moving in the axis that the arc is being formed around? So as to be creating like a spiral effect?

[Geof]

Originally Posted by cossiegaz .......would it be referring to circular interpolation whilst also moving in the axis that the arc is being formed around? So as to be creating like a spiral effect?

Exactly!

Going around in a circle why moving along in a direction parallel to the axis of rotation; getting all screwed up in other words.

Very useful for interpolating holes; you ramp down into the hole the cutter is making, or for milling a boss by ramping down the OD. You can also mill threads by having the Z movement per circle equal to the turns per inch; for internal threads G03 starting at the bottom is used and for external G02 starting at the top.

[cossiegaz]

Right ive been thinking about this again and am still a little confused, i understand that G17 would be used when producing an arc around Z axis using X and Y plane, G18 for producing an arc around Y axis using X and Z plane and G19 for producing an arc around X axis using Y and Z plane. Now if i was producing an arc starting from for instance X0 Y0 and finishing at X10 Y10 (which would be at a 45 degree angle across both the X and Y axis) and produced the arc using the Z axis then the arc would be equally around the X and Y axis so what G code would i need to use in this case?
Hopefully i've written my question clearly enough to be understood, sorry if it doesnt make sense.