forum.cncdrive.com

I posted this code in the thread at CNC Zone, but am adding it here as well.
I took the original code and edited out the G1 ramps, so that this is all G3 moves.
The display is showing multiple arcs as straight segments. According to the poster at CNC Zone, the cuts seem to match the display.

Hi Gerry,

I have checked out this code yesterday and contacted the gentleman.
The issue is different than what is described, the error is kind of missleading and tricky to see.

The issue is how these numerically small arcs are displayed, basicly it is a bug in how the small arcs are drawn on the screen.
The exact problem is that these small arcs are drawn from too few vectors and so they appear polygonal on the screen.
What appears incorrectly is not the ramp part, the ramp is from small line segments and not from arcs, but again, it is tricky to see on the drawing what is really the issue is. The G3 moves are no ramps, they never contain a Z coordinate programmed, what ramps are the small line segments, not the arcs.

The execution does not happen like on the drawing, but it can be also missleading if the CV tolerances are set too high, because then however not even the ramp down path is drawn incorrectly,
but the user can easily think that it is also executed like on the drawing, because those ramp tool path parts are on the same radius as the arcs, so it is tricky to see what the real problem is.
And if the tolerances are too high then a similar effect will happen on execution as on the wrong drawing. The issue in real will still not happen how it is wrong on the drawing,
but what happens is that the arc becomes polygonal also in the code execution, because of the high tolerances. Again, this is not the same as the drawing, just similar and so it is missleading.
Lowering the tolerance enough should fix the workpiece issue, however it will not fix the displaying issue, because the display issue is a bug.
I also adviced the customer to try make the acceleration higher in the UCCNC, because it is a wellknown bug in Mach3 which he comparing to that it overaccelerating and deccelerating the acceleration parameter settings, so it can be tricky to compare using the same acceleration values and so the UCCNC should make a better "overal performance" with higher acceleration, because it will still not stall the motor where mach3 does and because mach3 is cheating with the trajectory overaccelerations, however that cheating causes more problems in summary than how much good it is doing, probably not on this particular path though, but I did not have time yet to measure it out what mach is interpolating for this exact code with the user's settings, I only checked the UCCNC. But again, I also adviced to higher the acceleration in the UCCNC, about 2 times will likely not cause any problems if mach3 can run with it without loosing steps then the UCCNC should be able to run with 2 times higher acceleration and then the overal path performance and execution times should become shorter and better than in mach3.

So, in summary it looks to be a double issue, one is a display bug and the other is too high CV tolerance settings and the 2 problems look like if they were the same, but they are not.

Also, it seems that the user who started the thread on CNC zone was not aware that the default parameters are for mm use, he uses inches, so he must divide the units with 25.4 to get the right values. I don't remember if this is stated in the manual or not, but seems that now and then it creates some confusion in the USA.

Hi Josef,

In my opinion it is important for the user to understand how the tolerances work and that is described in the UCCNC manual in details.
The default if I recall is 0.03 units which is really OK for most millimeters jobs, but may be still high for example to cut a pocket to hold a bearing.
So, I think that we could say that the default units are for millimeter.
Another things is that if the user did not find out how tolerances work in the software means they did not read the manual and so even if we describe that the default value is to be OK with most jobs in millimeters the user will not find and not read that info either just like he did not read about the tolerances.

On the other hand I think I will add a note about this as you adviced, but I have doubts if that will help much... but anyways if it will be there then we can at least expect the users that they will read and understand.

The people that really need to read the manual, will likely never read the manual.

Yes, I fully agree. The ones who need the most reading think they need the least.
Maybe Artsoft was right about their new licensing scheme that they give zero support and if you need support then you pay $1000+, so customers read or pay.

Yes, it's confirmed now on CNC Zone that his problems are now gone, so no bug but an RTFM error.

A proposal:

Next time the manual is updated (next formal release) I think a short sentence should be inserted somewhere at the beginning saying something like:

Please note, that the default parameters are only examples and are for metric use. If you are using imperial units then you have to check the default settings and change accordingly.

Of course, this can be expanded even more, but I think a simple clarification should clear out similar issues, at least for people who read the manual.

Yes, it's confirmed now on CNC Zone that his problems are now gone, so no bug but an RTFM error.

There is a bug in the toolpath display, which needs to be fixed.

Yes, but that's different. It would be more worrying if the bug would effect the results.

Yes, it's like in the early AutoCAD implementations, you zoomed in too much on arcs and you got polygons.
We will fix it soon.