LinkBack URL
About LinkBacks
are you drip feeding
I have a NC milling machine FANUC with FANUC 3M control (rom version D71-04). I have a problem when milling sharp corners. The corners are not sharp or edged but are rounded instead. The machine already continues with the movements of the commands from the next line before it has reached the 100% exact accuracy of the before. Withe the increased speed the deformation is also increased.
I usually work with the axis movements F1000 to F7000 (1M/min to 7M/min). I checked the mechanical guides with a micrometer and the deviation is within tolerances 0.05mm.
With smaller programs I solve the problem by adding a mark "*" (EOB) for a blank line at the end of the command line (command block). With this the axis movements stop at the end of the command for a fraction of a second and this way the movements are exact on coordinats as they should be and only then the movements go on to the next line. But this way I am wasting a lot of time and the memory which is already small.
I would really like to know if this "defect" or imperfection can be removed somehow with the modify of parameters (which and to what value) or if there is some other way. By the way, the deformation results in all 3 axis.
I will appreciate any help.
Regards,
Renato
are you drip feeding
At that speed, if you want sharp corners, you have to be in G61 (exact stop mode). For blended lines and arcs, G64. G64 means that the faster you move, the larger the "radius" between segments.
Maybe program a .001 radius on the corners?
Software For Metalworking
http://closetolerancesoftware.com
I agree with Beege G61 should do the trick for you. Mrainy's idea should work as well but this will not save memory space and time as you are looking to do.
Stevo
We had a case of two supposedly identical machines. One would accelerate very hard and the other just looked lazy as it run the same program. The program did a lot of peck drilling and the one machine would run it in almost half the time.
After turning up the accel settings in the slow machine the two run very much the same even pulled the same peak power for the servo motors.
So not all machines get properly tuned at the factory.
And the accel settings will have a big effect on how much corners get rounded.
Thanks.
Unfortunately I'dont have G61, G64, G09 commands. When writing commands appears ERROR NO. 10 (unusable G code was commanded)
There might be an "in position window" parameter to shrink. This allows the machine to start processing the next block as soon as the window is reached. I've seen them as high as .100". Find your parameter book, or someone here can chime in...
Thanks.
Unfortunately I'dont have G61, G64, G09 commands. When writing commands appears ERROR NO. 10 (unusable G code was commanded)
What is the in-position parameter number for 0i series?
Thanks
On my 10TF, it's parameter # 1827, one for each axis. Yours is probably different.
I looked into the parameter manual. It is 1827 only, but the manual says that this parameter would be valid only if 1801#4 is set to 1.
The value is to be specified in "detection unit". What is that? The permissible range is given to be 0-32767.
Posting Permissions
