Hi Woody

Yes apologies, Mach does use G95 for feed per rev, I think the list I have was for Fanuc, everyone seems to do things slightly differently.

I have amended one of my programs to G95 and run it.  The problem then becomes that Mach does not display the feed rate during the cycle, only at the point that the feed is set and at the end of the run, so it is impossible to quantify.
The trace in the G3 arc does seem to be faster than the G2, but without a feed readout that becomes subjective.

Maybe this is why no-one has raised it before, they all use G95 and you cannot tell if the feed rate increases because nothing gets displayed.

Yes I am using the latest lock down version of Mach and Dave is using 1.84, but we are both seeing the same thing.

The weird thing is that G2 does not show the same speeding up.

I have no access to any of their code, so have no idea how they implemented these G codes, but you have to imagine that the basic program model would be the same but with direction reversed and centre point of the arc moved from outside the billet to inside it

Strange

cheers

Melee

(PS Hood, just got your post - XML attached. Obviously Daves' is completely different and he gets same speeding up phenomenon.)

Ok I am seeing this with your code, not sure if its actually related to  G3 as such, if I reverse them in the code (G3 first then G2) it is the G2 that will speed up.
 I will have a word with Brian and see what he makes of it.
Hood

Yes, you never really can tell this is happening if you think that the sounds are just the two steppers making noise at the same time, and you only take small cuts in aluminium or soft materials. BUT, try it with a larger cut in stainless and you know pretty quick there is something not right, and you can watch the RPM drop significantly as proof. A recent part I did, in stainless, I had some large amounts of material to remove so I was taking decent cuts, but when it got to the G3 it almost caused the toolpost to move and I had to check tool settings afterwards just to make sure it was ok.
   DaveA.

Oh, I always use G95, feed per rev.

I have certainly not moticed this in the past when I have done half round  ends on stainless rods for cleats I sometimes make but that only has a G3.
 The other things I do all the time have lots of G2 and G3 rads but they are small so I am unlikely to notice that but I will keep an eye on the DROs in the future, my turn screen has the same DRO in it as a mill screen so I see feedrates of mm/min even when I am in G95.
Hood

Is this anything to do with it -

If the axis continue to travel at their same speed, the compund "feedrate" will be faster (Pi D). I don't know how the maths is done to get the "circle" but it may be that one axis keeps a constant speed and the other then adjusts speeds to give the circle. The alogrithim on the two axis in a straight line would appear to be that the axis moving further gives the initial speed and the other axis adjusts it's speed appropriatly. It may be that this also applies to the "circle", but the compund speed would be greater.

Yes, I'm betting that this has something to do with the actual circumference of the arc being calculated in. Mach calculates at a greater distance because of a circumference error used in the feedrate calc.

Seems to be because I and K are used for your arcs, I use R for G2 and G3 and think that is why I have not seen the problem. I made a file up and tested it out on the lathe and it was rock solid. Brought it home to test on your xml and again rock solid , its similar shape to the first one so certainly seems it has to be that anyway.
Hood

Ok just been talking to Brian and as he pointed out it must have been there for a long time as 1.84 is pretty old version. When Rev4 Mill has been tested then turn will get attention so should get  fixed up.
 If possible can you code with R instead of IK as I have never experienced it so looks like that is the problem and hopefully will tide you over until turn gets worked on.
Hood

I didn't know that R worked in turn, will try it. It certainly would save me a lot of time when handwriting code that's for sure.

Heres what I made up earlier, have edited out the roughing and just the finish, certainly works fine on my lathe.
Hood