Home/Start Bug?

[4DThinker]

I use Aspire version 10.515. I run a LinuxCNC driven Probotix CNC and have come to appreciate the Home/Start Position feature under Material Setup. It lets me set where the bit starts and returns to so the bit won't hit any clamps on the perimeter that hold the workpieces down while also using the bottom left corner to set as my x/y zero position. It also lets me have the bit move out of the way between repeating cuts while I change out the part being cut.

Today I used Aspire to create toolpaths for a Multicam CNC. The project was parts cut from a 5'x5' by 18mm Baltic Birch plywood sheet, and I set the Home/Start to the center of the board but left the X/Y zero at the bottom left corner.
File loaded fine, but when started to run the machine did a horrifically fast jog to the center of the board so fast that it generated an error and the machine came to a dead halt. We had to reset/rehome the Multicam before we could try the file again. I can't find anywhere in the software to set a jog speed value but that Multicam certainly didn't like whatever command it got to go to 30,30. I eventually had to set the Home/Start X/Y values back to zero and recalculate to get the file to run fine.

Anyone else using Aspire with a Multicam CNC? Is there any machine jog speed control in Version 11 by chance? I know my Probotix CNCs have a hardware limit of 200ipm in their LinuxCNC configuration, but don't know if the Multicam CNC has any internal jog limit to keep it from trying to tear itself apart. I've been making files for the Multicam for several years with no problem, but this time was the first time I've set Home/Start values greater than zero.

Thanks for any suggestions/advice.
4D

[Adrian]

There is no machine jog speed control in V11. It's like previous versions. The speed of all rapid moves is set by the control software itself.

[4DThinker]

That's what I presumed Adrian. We've got a new person operating the big Multicam CNC, and he's not as familiar with it's settings as the previous operator was. All other machine moves (to 0,0, to change tools, etc.) went at reasonable speeds for the machine while the only code in the file was a tool number change or end of file. The move to a Home/Start position comes after a few setup codes in the G-Code generated using a Multicam post processor.
Without a 30,30 Home/Start move:
M90
G90
G17
G70
G74
G00T6
G97S16000
G00Z-0.8000
G00X0.0000Y0.0000
M12

With a move to 30,30:
M90
G90
G17
G70
G74
G00T6
G97S16000
G00Z-0.8000
G00X30.0000Y30.0000
M12

The G97S16000 command looks like the only thing that might cause a jog speed above the machine limits. We do not have a 4th axis on this machine. Tell me I'm on the wrong track.

[Adrian]

How far are the moves that work compared to those that don't? Say the machine was at 5,5 and the move was to 0,0 it wouldn't be able to accelerate/decelerate that much so the move would be slower even though the rapid speed is the same as when the machine moves a larger distance.

I'm very far from an expert on g-code (hopefully one will chime in) but I can't see how the G97 could be causing it. G96 maybe but not G97.

[TReischl]

Hmmm, I looked this up (my machine does not use G97).

"G97 constant spindle speed command. S RPM of the spindle/workpiece. M03 spindle direction. When switching between G96 and G97 always define a spindle speed. Since G50 command does not work with G97, care must be taken to ensure that the lowest allowable speed of the chuck and fixture is not exceeded."

Sooo, it controls spindle speed, not rapid motion.

I am also not familiar with the Multicam machine, but is it possible your new operator or someone else changed the max rapid rate or accelerations in the control software?

[adze_cnc]

According to this PDF: http://www.amtcnc.com/Files/Router_User_Manual.pdf (on page 282) the MultiCAM machines, referred to by the manual, accepts an "F" feed rate for G0 moves.

On could hard-code into the post processor something like:

Code: Select all

"[N] G0 [X] [Y] F200"

To cap the traverse speed to 200 units per time setting (or whatever you think is an acceptable speed).

Having said that, best to change the settings at the machine.

[TReischl]

.....

On could hard-code into the post processor something like:

Code: Select all

"[N] G0 [X] [Y] F200"

.....

Interesting you brought that up. Over a year ago I set up my various post processors (mill, laser, mill rotary, laser rotary) to output rapids as G1 with a fixed feedrate. When I am doing something that is worrisome I set that feedrate for the rapids very low so I can see what is going on, if all goes according to plan then I bump it back up. Mostly this happens if I am cutting aluminum with slow feedrates and I do not want to use feedrate override because that causes the cut moves to be ridiculously slow. Remembered that trick from the dinosaur days when I programmed a VMC that had all sorts of fixtures and clamps scattered around the table. Wrecking fixtures never seemed to impress management.