Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: DAlgie on May 04, 2009, 12:52:25 AM
-
Melee and myself have been noticing a problem with turn in that the feedrate doubles when in G3. I thought it might just be that I'm too chicken to upgrade my old reliable version 1.84, but he is running version 3.4xx and the problem is identical. Even stranger is that when you use a G0 after the G3 the feedrate in the G3 goes to about 6 times the displayed amount! If there is a G1 after the G3 then it only goes to about double the displayed rate. We thought it might be something to do with Melee's new M71 roughing macro but it does the same thing with a simple G code run. Kind of interesting to watch if you're only taking light cuts in aluminium, but heavy cuts in stainless can be cause for concern!
DaveA.
-
I have not noticed that on my lathe, was going to test out today to make sure but afraid my workshop got flooded from the office above so I had to switch the mains off. Hopefully I will get a chance tomorrow, that is if all the electrics have dried out.
Hood
-
That sucks Hood, hope nothing expensive got wet. Until Hood gets his stuff back running, anyone else ever program a G3 on turn and notice this?
-
Hi Hood
I started a thread here:-
http://www.machsupport.com/forum/index.php/topic,11420.0.html
not realising Dave was doing the same.
There are 2 simple .NC programs attached on that thread which demonstrate the problem.
Try them on your kit when it dries out and let us know
cheers
Melee
-
PS
I have effectively closed that thread now so as not to dilute any input
All replies to this thread please, the test .nc files are attached here
regards
Melee
-
Can you post a screenshot of the toolpath of these bits of code please.
Hood
-
Hi there,
I usually work in G95 mode (feed per rev) as I'm more used to that in the lathe, and I've not had this problem with G2 or G3. But I'm a bit paranoid and set the F on every non "G0" line as attached. Does this file show the feed problem on your setup?
One thing I did notice just once, Mach3 got the feedrate completely wrong on one line (G1) (much too fast, but not G0 fast), then the next line was extremely slow, after that it was OK. Code was fine as far as I could tell.
Do you still get the problem in G95 mode? Also, I'm not sure how to get a feel for feed per min when turning. Why would you use that in the lathe? If no spindle speed feedback?
Regards,
Woody.
-
Hi Hood,
The tool path images are now attached below.
Hi Woody
I think G99 is the lathe equivalent of G95, which is milling G Code for feed per rev.
I use feed over time simply because I am used to it and have a pretty good off the top of my head idea of what ratios I need for different jobs and finishes.
using higher spindle speed, slower feed for finishing cuts etc. etc.
I don't tend to take heavy cuts and prefer to write programs that will just run unattended whilst I do something else, it doesn't matter how many loops it takes.
So I don't tend to suffer from spindle slow down and get away quite happily using feed over time
I will try using G99 and see what happens.
I have tried setting the feed rate specifically on the G3 line and it does not work, the rate still doubles.
This leaves open the temporary solution of setting half the feed rate you actually require and ending up just about right, but it is hardly satisfactory.
I will copy your file over to my Mach setup and let you know what happens.
regards
Melee
-
Hi Melee,
I think Mach3 may use G99 differently looking at the Mach3Turn manual, G95 is feed per rev and G99 is "R point level return after canned cycles" whatever that means! Page 10.10.
By the way, are you using Mach3 R3.042.027? Maybe worth trying because a number of turn related problems have been fixed, including a driver error in threading. I wonder if that also affected your issue?
Cheers,
Woody.
-
can you attach your xml as well please
Hood
-
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
-
Hi Hood
I will have to test some more but using R parameter does seem to 'cure' the problem for now.
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.
I knew R could be used in turning centres but also that some controllers do not support it.
Specifying the centre point with I K (and J on mills) seems to work everywhere, which I why I tried to use it.
Hopefully those parameters will be fixed before too long
cheers
Melee