Biesse post arcs vs linear moves

[dustmaker1]

Hi all, I am new to VCarve pro outputting to my Biesse Rover 22, run by NC1000 controller, programing in metric. The Biesse post processor seems to work well, no problems with the tool changer or origins etc. After watching the tutorial on converting to arcs, I am experimenting with this, to make the file sizes smaller and see if I can get the machine to run smoother. After converting a set of vectors to arcs I expected to have lots of arc moves in the code in place of linear moves. However this was not the case, so, I thought I would try the code from a simple circle. I find that if I create a simple single vector circle, send to tool paths as arcs and tool path as profile at one depth I get as I would expect as output code four arc moves to create the shape. If however I create a v carve tool path between two concentric circles made with arc's I get code output as linear moves. Is this how it is supposed to work? Can I only get compact files with arc moves when not Vcarving?

The other issue I am having is with processing speed. I V carved the Bulls head sign and had to set scailing to almost 4 to make the machine time equal to the estimate. This is with a machine with high feed rates rapid's at 100/m minute and has high acceleration rates, for its size anyway.

Any input on these issues would be appreciated.
Thanks
Paul R

[BrianM]

Hi Paul,

A V-Carve toolpath is normally moving in XY and Z so there are no arcs. The case you manufactured of two concentric circles is about the only case where arcs would occur and it is very rare to just be V-Carving concentric circles (a profile toolpath would be much more efficient in that special case).

has high acceleration rates, for its size anyway

I think the 'for its size' is the telling point there. A VCarve toolpath is usually made of lots of of small XYZ moves in 3 dimensions. Many of the big machines can accelerate pretty quick in X and Y but are often much slower in Z as they weren't typically designed for this sort of machining and they have a lot of mass to move. For a move in 3 axis, the acceleration will be limited to that of the slowest axis.

Brian

[ludovic815]

Hi
I am sorry for the late answer (4 years later) but I think it might be interesting for biesse cnc owners:
The problem is not about acceleration on the Z axis. I had the same issue on a Biesse Rover 23 a Biesse Rover 322 and a Biesse Rover B.
In fact these machines can accelerate as fast in Z as in X and Y.
The real problem is that the machine slows down and stops for a short amount of time after each non tangential step (ie: after each line of code).
When you have toolpaths with a lot of small moves, your cnc will take a lot of time with this behaviour but you can change this with one instruction in the code!
Try to add G47 at the begining of the code, just after G71. With this instruction I was able to bring the time scaling factor from 4.0 down to 1.0, but the cnc becomes less accurate (if somebody has a solution for this...)

This quote is taken from the biesse xnc programmers reference book:

G46: Commands the axes to arrest upon movement end, for non-tangential steps, while maintaining the attainment of the target co-ordinates within the positioning tolerance. Reset by G47, G27, G28

The G46 instruction is the default behaviour of Biesse machines.

G47: Avoids arrest or slowing of the axes on sharp edges formed between non-tangential steps. Reset by G46, G27, G28

If you use this instruction, the machine will move at "constant speed" and it will reduce a lot the machining time, but it is less accurate.

Tomorrow I will try G27 and G28 instructions to see if I can find a compromise between accuracy and machining time

G27: Commands the axes to arrest upon movement end, for non-tangential steps, without waiting for the target co-ordinates to be reached, within positioning tolerance

G28: Commands the axes to slow down upon movement end, for non-tangential steps, function of the angle formed with the succesive step.

I think G28 could be really interesting... Will try it tomorrow.

You can change the Biesse Rover Arcs PP to use these instructions:
Replace this line:

Code: Select all

"N10 G71 HC=1 LY=[YLENGTH] PLPZ=[ZLENGTH] PDM=0 PUOS=0 FIL=0 BLO=0 ACC=0 RUO=1 PRS=1 PRL=1 PPWQ=0.000 KA=256.000 LZ=[ZLENGTH] LX=[XLENGTH] "

With:

Code: Select all

"N10 G71 G47 HC=1 LY=[YLENGTH] PLPZ=[ZLENGTH] PDM=0 PUOS=0 FIL=0 BLO=0 ACC=0 RUO=1 PRS=1 PRL=1 PPWQ=0.000 KA=256.000 LZ=[ZLENGTH] LX=[XLENGTH] "

I hope this could help Biesse owners...