Is there a simple fix to this problem?
We're using a Fanuc 6M control to run a 3 axis simultaneous (X,Y & Z) surface milling program at a 2000mm/min feedrate.
The program is made up of thousands of small (1mm) X,Y,Z movements.
In practice, the machine never reaches the programmed feed because it is always accelerating and decelerating between each co-ordinate.
We are not working to tight tolerances (+/-0.2)
Is there some way of either configuring the control or modifying the CNC program so that the moves are "smoothed" out in order to achieve a higher feed rate?
I'd be very interested to read any suggestions you have.
Lots of things to think about here. The Fanuc 6M has two "speed limits" for running a 3D surface program.
One speed limit is the control's internal "block processing" speed. The control can only process so many blocks per second, no matter how far each block moves the machine. If your point-to-point distance is very small (say, .005 inches per block), then your feedrate will be very low and there's not much you can do about it.
Another speed limit is the number of characters per second that the control can process, and here is where there are LOTS of ways to speed things up. If you're running through a DNC link of some sort, your character speed is about 300 cps. This is the speed of a Fanuc paper tape reader, and any Fanuc 6M would only be drip-fed through that tape reader port with a BTR (Behind the Tape Reader) link of some sort. At 300 CPS, you can only read so many blocks of data per second, and this is where the number of CHARACTERS per block makes a big difference. Here are some tricks:
1) Don't use N-numbers. They're not needed
2) Don't have space characters in your program
3) Use only a LF (Line Feed) at the end of each block. CR (Carriage Return) isn't needed
4) Take out redundant numbers and G-codes
Now, for the scary part:
5) Use incremental mode (G91). Yes, you heard me ... G91
6) Take all the decimal points out of your numbers
The six suggestions mentioned above will take this program:
N0001 G90 G00 X0.0000 Y0.0000 Z0.0000
N0002 G01 X0.0050 Y0.0050 Z0.0050
N0003 G01 X0.0100 Y0.0100 Z0.0100
into this program:
As you can see, the program has a lot fewer characters, but the moves are the same.
If your point to point distances are small, it may be better to make a series of short G02 or G03 moves instead of even shorter G01 moves. Most CAM systems can produce a series of arcs to make a 3D surface rather than a series of straight G01 moves.
On the 6M, you can also "open up" the parameters for the "in-position" zone. These are set with parameters 70 (X) 71 (Y) and 72 (Z). Normally, they're set to a small value, like "10" or "20". By making this value a bit larger, you open up the tollerance of the in-position zone. Each G01 move must let the servos get into position by less than this tollerance before the next block can be executed. Opening up this tollerance lets the servos begin one block a little before the previous block has finished it's move.
One more hint: If your machine has INCH ballscrews, program in inch. If your machine has METRIC ballscrews, program in metric. If your program is in the same increment system as the ballscrews and servos, the control does not need to perform an inch/metric conversion on each block, saving some processor time.
I checked some programs I posted years ago for a Bridgeport BOSS 9 and it seems that the Accel/deaccel code is G99. Basically your telling the control to turn off the deacceleration between moves, it speeds up the moves quite well although accuracy isn't on the priority list. Your code may be different but if I remember correctly the BP software emulated a Fanuc 6M pretty close (I used to own a BOSS 9)
Sometimes you only need to code it once in a feed move, sometimes it needs to be in every line.
Also, as Dan pointed out, you could start by stripping the (N) numbers and spaces, it's relatively easy to do in an editor as they usually have a utility to do this. Give it a try and see if it helps.
A force of one
I was initially interested in the parameter settings, which you have stated so that's something I want to try. I have already crunched the program down using most of your suggestions except for the incremental idea. I can convert the code to incremental using an excel spreadsheet.
I was not aware of the significance of the CPS processing speeds but will be mindful of this in future.
Did try getting the CAM system to fit arcs where possible a few years back but the CNC control didn't interpret the moves as intended causing a poor quality finishes.... I may re-visit this option now I try out on a test piece.
You've been very helpful...I've printed your response off for future reference
Thanks for your help Dave, I will cautiously try your suggestion as you're indicating that it may not work. If it does...it will be an easy fix.
G99 is usually stated after a drilling canned cycle as opposed to a G98.
G99 = return to R value
G98 = return to previous Z value
I'm assuming G99 has another function by what you're saying.
Thanks for your suggestion
You know, I believe your correct. Although some G codes are somewhat standard, some are at the digression of the machine tool builder. G99 in your case is already used. That code is also used in the Milltronics for return to reference point. In the BOSS software it was not. Maybe your 6M doesn't allow for turning off the deaccel within the code, check the manual for accel/deaccel or even possible exact stop?
A force of one
What software are you using to program with? I know mastercam has a filter in the operations to limit small moves on 3d programs. and the code I remember was G68 exact stop mode I think you call up g67 or g69 and it cancels exact stop mode. Sometimes I've found slowing the feedrate will help in the jerkiness to achieve a better finish without sacrificing cycle time, your not getting to 2000mm/min anyway so look at the highest feed you achieve and program a little less. Good luck
on one mill i was running a found parameter to change how many lines the controller would read ahead. i changed it from reading 3 lines to 10 lines and it was much smoother
test run with G64 , some Fanuc 6M use this G code run more faster , and the transmision way ( DNC) must good .I think Fanuc 6M can not use look ahead running ( feed forward process ) , some software can do filter a long lines program become arc move , it easy to run faster .