[Machineit]

Hi all,

I have an issue with my CHNC 1. Just got it back up and it is running fine except for one issue that is driving me crazy.

If I program the spindle with G97, Direct RPM Programming, the spindle will start at the programmed speed and as soon as a linear movement is made, the spindle stops or drifts slightly backward. I thought it was an issue with the feedrate, in IPM instead of IPR, so I changed that. If I program say an S1000 M03, the spindle will start, but as soon as the next block comes it will stop. So even programming an F100. feedrate, the spindle still stops, but the carriage does the programmed movement (like a drill cycle) without the spindle turning.

This is of course giving me fits and I have parts I need to run.

Any Ideas!!!!

Mike

[Machineit]

I'll add this so you understand better.

%MPF0111
G90 G54
T01 D01
G92 S1000
G97 S1000 M03
G00 X.2 Z0.(AT THIS LINE, THE SPINDLE STOPS, BUT MOVEMENT CONTINUES)
G01 G41 X0. F.002
G01 X.615
G03 X.625 Z-.005 B.005
G01 Z-.8812
G01 Z-.7812
G00 X6.
G00 Z12.
M05
M09
D0
M30

[txcncman]

Why the G92 S1000 line if you are using G97?

[Machineit]

Why the G92 S1000 line if you are using G97?

Just the way the CAM system writes it, but makes no difference when removed or written without.

I knew I should have removed it before posting this!

Mike

[txcncman]

What about direct setting of G98/G99?

[Machineit]

What about direct setting of G98/G99?

Not available, mine ends at G97. I believe this will end up being a machine setting that needs to be fixed. The machine was just recommissioned and we may have missed something.

Calling Hardinge later today.

thanks for the help.

Mike

[txcncman]

Will be interested in hearing the results since I still occasionally work with Hardinge machines.

[Machineit]

I did a little test and it does not appear to matter what the next line of code is, it still shuts off.

I programmed it with an M08 as the next line and it shut off then too. So, it has nothing to do with linear or other movements. Just leave that line of code and it stops.

It will be interesting to find out what it is. For now, I just need my lathe up.

Mike

[Machineit]

Hey mystery lovers!

Okay, I have it down to the gnat's ass now.

I tried (G97) in every block, but it would stop. However, putting the speed command, S_ _ _ in the block does fix it. Just need the S_ _ _ and it does what it should and even reverses okay.

So it is loosing the Speed command and reverting to the last G96 CSS speed command if there was one. If there was no G96 (CSS) command prior, it just stops.

I just tested that theory. Programmed a S1000 G96 (CSS) then a S100 G97 (direct). It started in G96 at 1000 RPM then went to the G97 at 100 RPM and ran fine, but when I went to the next block it went back to 1000 RPM!!!!

So that is it, it is not holding the speed command in Direct or G97 mode. It has to be some setting for the control. For now, I can get around it by putting an S_ _ _ _ in every line under G97 mode and get some parts done. Now I just hope to find the real answer.

Mike

[txcncman]

Seems this might be a PLC ladder problem with a keep relay. But what do I know, I am a programmer and machinist, not a repair tech.

[Machineit]

Ya, beats me. My repair guy is on the road coming home from up North. I talked to him yesterday, but did not have all of the info I have now.

The work around of putting the "S" command in each line where I am in G97 mode is working and I am making parts right now.

Mike

[mark562]

Mike

I have not been on the zone for a while so missed this, The Siemens control uses the G97 to set the direct RPM and you must program a G96 SXXX (surface per minute) on a separate line every time you want to change the RPM.

For example if you are contouring with tool 1 you will program the G97 S1000 M03 line first and then the G96 with the desired S/F/M

Then to drill with tool 2 at a steady RPM you will need just the G97 SXXX line. The next time you need the variable RPM you must program another G96 SXXX line.

It is not a setting issue it's just the way the Siemens is programed. I have never tried to reverse the spindle before, you might have to program another G96 line

Hope this Helps
Mark

[neilw20]

Try this: Got rid of mysteries on an Okuma.
G50 S800. Sets maximum RPM.
Without a max rpm setting the constant surface speed calculator can get confused.

[Machineit]

Try this: Got rid of mysteries on an Okuma.
G50 S800. Sets maximum RPM.
Without a max rpm setting the constant surface speed calculator can get confused.

Nielw20,

G92 is my MAX RPM setting and works fine. My problem is under my Direct RPM programming Mode. CSS works fine.

Thanks---Mike