Increased efficiency programming trouble with CSS

[Guren]

Hi,

I noticed that if I change my programming style just a little, I can make any detail 2-5 seconds faster than I nomally do. (see the before->after sample)

But my machine goes looney if I try the same thing with Constant Surface Speed. For example if I tell it to go Z0, it will go Z145, yes it makes no sense, time for examples:

before->after sample

hire is a simple program I used before:

G97 S600 M3
T0606
G0 X30
Z1
G1Z-15
G0Z150 X150

And hire is an improved version

G97 T0606 S600 M3
G0 X30
Z1
G1Z-15
G0Z150 X150

Basically I simply put the tool change & the spindle speed change on the same line. So that the machine will change the tool & spindle speed simultaneously = win in time.

But if i use the same program & CSS it goes nuts: sample:

G97 T0606 G50 S2400 M3.................<> set spindle speed limit cap
G97............................................... .......<> disable CSS
G96 S250.............................................< > enable CSS & set it to 250
G0 X30
Z1
G1Z-15
G0Z150 X150

I also tried it like this & same problem

G97 G50 S2400 T0606 M3

Any ideas how to overcome this?

[MMMMM]

It may be nothing but, I don't think you can establish the limit AND set the RPM on the same line.

Have you tried this?;

G50 S2400
G97 T0606 S2400 M3
G96 S250
G0 X30
Z1
G1Z-15
G0Z150 X150
...
...

[Guren]

Originally Posted by MMMMM

It may be nothing but, I don't think you can establish the limit AND set the RPM on the same line.

Have you tried this?;

G50 S2400
G97 T0606 S2400 M3
G96 S250
G0 X30
Z1
G1Z-15
G0Z150 X150
...
...

Yes I have & i cant use it because we set the CSS & then start moving our tool to the cut off position (while the tool moves the spindle speed also changes & it consumes time.)(the distance is from [X150 Z150]-> to [X45 Z -15] )

So I was thinking & I think I came up with the solution, Its working right now & it seems to be doing quite well.

The only downside of this solution is that I must calculate the current spindle speed (in rmp) at the cut off position beforehand.

Tho I coded me a calculator to calc the speed at any given diameter & at any CSS. & since im using a notebook to do the programs its not big deal.

How ever, If you guys think there is a better way to do it, feel free to let me know.

Idea is to change the spindle rpm to the rpm it will have at the position of X45 Z-15 while we change the tool, then move the tool to the cutting off position & set CSS.

At this point css will be already 707 rpm so we wont waist time

imagine cutting off pos to be at the following coordinates: X45 Z-15 & css 100 m/min

G97 T0101 S1800.......tool 1
G0 X0......................do some stuff hire
......
G0 X150 Z150...........move tool 1 away from the detail
M1
G97 T0202 S707......cutting off tool 2
G50 S1000.
G0 X46 Z-15
G96 S100
G1 X45 F0.3
.......

[angelw]

Originally Posted by Guren

Yes I have & i cant use it because we set the CSS & then start moving our tool to the cut off position (while the tool moves the spindle speed also changes & it consumes time.)(the distance is from [X150 Z150]-> to [X45 Z -15] )

Your statement doesn't make sense to me. What Doug suggested is the same as your 1st Post example using G96, except he suggested putting the max clamp speed command G50 S2400 in the block preceding the G97 and Tool call up. I understand why you don't want to start the spindle in G96 mode, but the original question was regarding the strange behavior of the machine.

Originally Posted by Guren

So I was thinking & I think I came up with the solution, Its working right now & it seems to be doing quite well.

The only downside of this solution is that I must calculate the current spindle speed (in rmp) at the cut off position beforehand.

Idea is to change the spindle rpm to the rpm it will have at the position of X45 Z-15 while we change the tool, then move the tool to the cutting off position & set CSS.

This method is well exercised by programmers and has been around a long time. As well as not winding the spindle up to speed as the tool is moved to the first cut diameter, (you haven't identified the control yet, however, if a Fanuc, the behavior of the spindle RPM in G96 mode whilst rapid traversing in X, is determined by parameter setting), it also eliminates wild fluctuations in spindle speed when the turret is sent to the tool change position, if its a large X coordinate. In this case, the RMP of the Next Tool start diameter is calculated, and that RMP programmed with G97 before moving to the tool change position. Alternatively, G97 with no "S" value specified will hold the spindle RPM at whatever they were when in G96 mode at the last diameter before moving to the tool change position.

If CAM software is used to generate the CNC program, the above method can be made happen via the Post Processor.

Regards,

Bill