Lathe - set max RPM for CSS?

[DaveCVI]

Hi,
I'm playing with mach lathe -

1) is there a newer gcode language doc for lathe than what is in the old mach 1.84 manual?

2) G96 is not in the 1.84 manual - but I see that the mdi line accepts G96 S~
What is the syntax spec for mach's G96?

3) How do / can you set a max RPM for G96 mode?

Dave

[Hood]

1. No, nothing new in turrn since the first day it was released I would say
2. CSS doesnt work correctly
3.G48S**** is how you set max RPM when in G96.
Hood

[DaveCVI]

Hood,
1) is there a summary of the issues with css?
2) is there a repository of lathe lore where I can find things like G48 and G96 - that are not in the Gcode section of the 1.84 manual?

Dave

[Hood]

Issues with CSS are as far as I recall when testing. Feed per rev increases/decreases when spindle speed changes. Feed one way on X and it takes a lot lot longer than if feeding the opposite X direction, this BTW is going from point A to B or B to A so its not as if the distance or dia are different. You will probably find more details if you search the forum as its been a long time since I personally gave up testing it

Dont know of anywhere with the info, not much about for Turn except whats in members heads I supect.
Hood

[thosj]

So there are issues with CSS, G96. Does it not work at all, or is it goofy somehow?

Does Feed per revolution work correctly? I tried it, and when potting my speed override, the feed did not seem to change. I haven't tried any of this actually cutting, just in the air, so don't know if feed changes and just doesn't show on the screen.

Kind of too bad Mach Turn doesn't have the usage, hence fixing, that mill has. Would be nice!!

[Hood]

G95 works very well.
FRO works fine as well and if I recall the DRO changes on my screenset but I may be using a different DRO than the standard lathe screenset as I seem to have it in my mind that I had noticed it not changing on te standard screenset.
Hood

[chrisjh]

Hi All,

My experience is that Mach3 Turn responds to G94, G95, G96, and G97 well, if you follow the syntax structure as described in Smid’s CNC Programming Handbook. For example:

G96 S45 M3 G95 F0.1 (Turn on CSS @ 45m/sec and @ a Feed Tool @ a rate of 0.1mm/rev)

G97 S900 M3 G94 F100 (Cancel CSS and run Spindle @ 900rpm, Feed Tool @ a rate of 100mm/min)

I haven't had any experience with setting maximum rpm with G48, as my lathe maximum rpm is limited by my VFD settings, but I suspect that G48 would respond successfully if tested.

There is an example of G code that works successfully towards the end of the document at this link:
http://www.cjh.com.au/Gang%20Tool%20Block%20Offsets%20for%20CNC%20Lathes%20under%20Mach3%20Control.pdf

This link shows a part being turned using a method that switches various operations between CSS (G96) and normal rpm (G97), as well as feed/rev (G95) and feed/min (G94):
http://www.machsupport.com/forum/index.php/topic,14282.msg94797.html#msg94797

Hope this helps.

Regards
Chrisjh

[Hood]

Chris, it is quite hard to be sure from that vid, due to the short distances being travelled, but looks to me that the X travel is constant. Surely if you were in CSS and G95 then when the spindle speed increased the axis feed should also increase to keep the feed per rev constant?

If you have time and are willing to test it would be nice to know.
Can you run some code cutting air  in CSS as a test, what would be good is if you run from largest Dia you can turn into almost the centre and observe if the axis feed per rev stays constant as the spindle speed increases, ie the axis actually travels faster because the spindle is going faster. Also would be good if you can time that operation. Next reverse the operation, ie start from centre and work your way to largest dia and see if it behaves correctly and also see if there is a difference in the time it takes.

I will try when I get to the workshop later on, unfortunately I am stuck at home doing my tax but it gives me a good excuse to go down to the workshop later and forget about tax for a while
Hood

[Hood]

Ok just tested
G0X200
G48S1000
G96S200M3
G1X100F.1

Feed starts at 0.1mm/rev and as the x moves towards the 100mm dia the feed decreases steadily with spindle speed increase, goes down to 0.05mm/rev. Time taken is 1min 35 seconds


G1X200F.1

Feed starts at 0.1mm/rev and as X moves to 200mm dia the feed increases steadily with spindle speed decrease, goes up to 0.2mm/rev. Time taken is 47 seconds.

To me that is totally wrong, FPR should stay constant and axis velocity should increase when spindle speed increases and decrease when spindle speed decreases.
Maybe I am wrong? Is what I am expecting not correct? Is what actually happens correct?

Hood

[Hood]

Oh also Chis, the G48 is not for restricting max spindle speed of your machine as such, the reason it is used is you may have say a 300mm Dia lump in the chuck and you are facing it in CSS, you would want to limit the RPM to what you would consider safe. That way when you hit the centre of the move the spindle is not whizzing that 200Kg lump of steel at 5000rpm
Hood