Mach 3 turn constant sfm?

[DaOne]

Does mach 3 (lathe) have the ability to run a constant surface feet per minute? Basically as the tool moves closer to the center of the x axis  the spindle speed increases to compensate for the diameter to keep an even sfm? My Haas has this ability. Wondering if I can give my retrofit the same ability.

[Hood]

Yes. G96 turns it on, G48S**** sets the max permissible speed whilst in CSS and G97 turns it off.
Hood

[DaOne]

Thanks hood. So I just need to make sure its in my G code. Nothing else in mach setup that I need to turn on? You dont happen to know when I can locate a post for mastercam X4 turn? Thats what I use at work so would love to use that to program my retrofit too.

[Hood]

Yes G96 in the code and CSS should be active, G97 when you wish to turn it off and G48 with the max spindle speed you want, for example if you are facing a large dia you will likely not want it to spin too fast for safety reasons.

Regards the post processor, afraid I dont know.

Hood

[riporeno]

hi  
it is the first experiences with the lathe  
I have also done me this test.  
when I write G96 it tells me error,  
it tells me that he  wants G96S....  
is it possible that mistake?  
where G I can find the functions for the lathe?   
thanks 
regards

[DaOne]

Here are the ingredients for spindle control...

G48  "Sets the max RPM the spindle will turn (so you don't over speed your work /chuck)
G96  "Sets the mode for constant surface speed (CSS)"
G97  "Sets the mode for constant spindle speed (RPM)"
S  "This is the command to set the spindle speed. In CSS mode this is SFM. In RPM mode it is RPM (S after G48 is RPM)"
M3  "Turns the spindle on (clockwise rotation)"
M4  "Turns the spindle on (counterclockwise rotation)"
M5  "Turns the spindle off"

So lets say you want to use a front toolpost on a left hand spindle lathe for your code would look like this...

Variables for CSS mode: SFM=400, MaxRPM= 2000, Direction is clockwise.

G48 S2000
G96 S400 M3
M5

Or...
Variables for RPM mode: RPM= 2000, Direction is clockwise.

G97 S2000 M3
M5

Hope that helps.

Wes

[riporeno]

ok thanks. 

[WoodyCam]

Related Turn question in Vn 40. with parallel port. Say I'm doing:

M3 S1500 (rpm)
G95 (constant feed per revolution)
F 0.2 (mm/rev)
G01 Z blah

and its cutting, the STrue is 1500 rpm (finally got that working) and its too fast so I turn down the spindle speed (via the VFD by hand), the STrue drops and the S speed stays the same as expected but the feed (mm/rev) goes up and the rate the Z axis moves does not change. So its not reducing the feed rate so mm/rev calculated goes up. Is this normal? Is there a setting I can adjust so it keeps a constant mm/rev when speed changes? Even if I try to change the "S" via override, makes no difference.

Do I need to be in G96 mode for this interaction or is the feedrate fixed once the command is running and actual spindle speed has no input? I have the box "Use Spindle Feedback in Sync modes" ticked.

Next, I've played with G96 and found it messed up the "STrue" number as soon as this command was reached. 0 to 1500 rpm would read 2035 to 2355 or something like that. I must be doing something wrong. Can someone post a successful G-Code snippet with G96 used please - would be really helpful. In the meantime, I'll experiment some more.

(G96 is not in the Turn documentation I have.)

Thanks,

Woody.

[Graham Waterworth]

G21 G40 (metric and clear any comp.)
T0101 (select tool 1 offset 1)
G00 X100. Z10. (rapid to start point)
G48 S1000 (set max spindle speed)
G96 S50 M3 (select CSS)
G95 (set to feed/rev)
G01 X10. F.2 (feed to 10mm dia)
X100. (feed back to start point)
G97 S1000 M3 (set to rpm mode)
M30 (all done)

If you watch the speed it should range from 159 to 1591 rpm, this will not happen as the speed is capped at 1000 rpm, the G48 line can be changed to allow maximum if it is safe to do so.

Graham

[Promech]

When I use this code CSS works fine meaning as the diameter decreases spindle speed increases. What is not working is the G95 or constant mm/rev feed rate.  If I assign F=.2mm/rev this feed rate only takes place at the start of the cut when the RPM is still 1000RPM. As the RPM increases the feed rate in mm/rev decreases.  Has anyone had experience with this behavior? My observation is that RPM x F(mm/rev) remains a constant value which suggests to me that the feed  is remaing constant in mm/min and not in mm/rev as it should having set G95.