In profile mode Mach cuts corners off? Shortest distance issue?

[JAZZCNC]

Your simply trying to go too fast for such small text with CV mode. 3600mm/min is way too fast for this size txt.
No way can a constant velocity be maintained at this feedrate on such small radius. You could try exact stop mode by typing G61 in the MDI before running code but it will shake the machine around.

You can play with the CV settings and increasing look ahead to get better but you won't get it to maintain travel at these feedrates in CV mode without rounding it's just not possible.!!

Unfortunately you will have to slow things down. I'd also increase accelleration in motor tuning as 100 is quite low.
Often with moves that are short like engraving etc your better lowering velocity and increasing accelleration in motor tuning. Often this lowers cycle times on small move work.?
Reason for this becomes obvious when you think about how each move or direction change works.?
Every move as to accelerate to commanded feedrate, travel at this feedrate then de-accelerate all before the next direction change happens.
Now on long moves it's no problem hitting the commanded feedrate even if high has we have plenty of time before the next move happens.
On short moves the time interval between moves comes very quickly and no way can high commanded feedrate be reached before having to slow down for next move so some speed clipping occurs. On large jobs like 3D work this clipping can amount to large time increase in cycle times.

Think of it like a race traffic light to traffic light between a F1 car tuned for speed and Bus tuned for stop to stop. When lights are streets apart then no problem F1 car wins every time but put the lights every kerb stone apart and Bus will smoke it.!!

Same thing happening here.!! No matter what you command the feed to be in G-code the machine can only go so fast before having to slow down again.
The feedrate reached will depend on the motor tuning but in general with higher acceleration the machine will produce shorter cycle times as it can reach a higher feed before slowing down again for next move or direction change.

CV is like trying to go around corners without slowing down. This is impossible in tight corners so rounding occurs, how much depends on the CV setting. With high feedrates then even when CV settings are dialed in good for best balance rounding will occur if feeds are set too high.

Edit: Oh and your G-code doesn't help matters by creating arcs with tiny lines. Try using a post processor that uses (i) (j) Arc moves instead of breaking each arc into tiny straight lines. Could also be a setting in the Cam software.?

[Clive S]

Dean. You took the words right out of my mouth I was just about to say all that. ..Clive

[JAZZCNC]

Dean. You took the words right out of my mouth I was just about to say all that. ..Clive

Ye I know you was Clive and I'm just a faster typer thats only reason I beat you to it.! . .

[marbles]

Thanks for the thoughts. All very helpful.

I'm amazed that i've not found this to be a major issue before? The machine was built for one purpose which its managed very well, running for several thousand hours quite happily. I did a basic setup when I built the machine but not much fine tuning. Its a belt drive running directly of a 15T sprocket. Still i've always wondered why it cut radius (none critical) in an odd way sometimes. looks like this combination of feed, velocity and acceleration is critical.

You suggest increase acceleration in motor tuning, as 100 is quite low. What would be your suggestion there?

Based upon your advice to lower velocity and increase acceleration whats your guess for a decent feed speed?

Thanks for all advice.

[komatias]

Edit: Oh and your G-code doesn't help matters by creating arcs with tiny lines. Try using a post processor that uses (i) (j) Arc moves instead of breaking each arc into tiny straight lines. Could also be a setting in the Cam software.?

Aspire has an option to simplify the vectors you are intending to cut. I think it is called "smooth" or some such. you can change the setting in that option to make the number of line segments less. Gives you machine a much easier time. You will hear the difference from the sound of the axis motors.

[marbles]

Thanks for the Aspire info. i shall seek out "smooth" and amend.
Cheers

[komatias]

Thanks for the Aspire info. i shall seek out "smooth" and amend.
Cheers

the button looks like an S with a line through it.

I have had this with small jobs too, the finish looked very rough and the machine was very jerky at higher speeds. With the smoothing, because you are actually telling the machine to do circular sector, it interpolates intrinsically and is just so much smoother.

[marbles]

Thanks!

I'm just in Aspire now and using the 'S' fit curves to selected vectors tool. I can see the difference in file size immediately. I just need to remember to tick the 'replace selected vector' box otherwise end up with two files on top of each other.

I see a 'T' tool in vectror curves section of Aspire which is convert objects to curves. Similar or not, or for another day I wonder?

thanks

[komatias]

That is for converting text fonts into curves so you can profile them or edit them like vectors.