[DasNewb]

Hi everyone,

I have a 770 machine and I noticed that when the Z is feeding, it changes its feed rate at the last second and plunges into the part really hard. Usually it takes the feed rate that it on the next line for some reason. I'm using CAMworks and I don't know if this could be a post processor problem. Please help.

Is it possible that it is combining the z feed and the next line x feed? I bolded the part where it changes its Z feed rate.

Here is the snippet of code that it is doing it with:

N30 T52 M06 G43 H52
(9/16 EM HSS 4FL 7/8 LOC)
N40 G00 G54 X3.507 Y.93 S4000 M03
N50 Z.1 M07
N60 G01 Z-.05 F6.25
N70 X3.369 F50.
N80 X2.795
N90 G02 X2.556 Y1.055 R.291
N100 G01 X.813
N110 G02 X.574 Y.93 R.291
N120 G01 X0
N130 X-.138
N140 Y.762
N150 X0
N160 X.574
N170 G02 X.813 Y.637 R.291
N180 G01 X2.556
N190 G02 X2.795 Y.762 R.291
N200 G01 X3.369
N210 X3.507
N220 Y.93
N230 X3.369
N240 X2.795
N250 G02 X2.556 Y1.055 R.291
N260 G01 X.813
N270 G02 X.574 Y.93 R.291
N280 G01 X0
N290 X-.138
N300 Y.762
N310 X0
N320 X.574
N330 G02 X.813 Y.637 R.291
N340 G01 X2.556
N350 G02 X2.795 Y.762 R.291
N360 G01 X3.369
N370 X3.507
N380 Y.93
N390 G00 Z.1
N400 Z.05
N410 G01 Z-.1 F6.25
N420 X3.369 F50.
N430 X2.795
N440 G02 X2.556 Y1.055 R.291
N450 G01 X.813
N460 G02 X.574 Y.93 R.291
N470 G01 X0
N480 X-.138
N490 Y.762
N500 X0
N510 X.574
N520 G02 X.813 Y.637 R.291
N530 G01 X2.556
N540 G02 X2.795 Y.762 R.291
N550 G01 X3.369
N560 X3.507
N570 Y.93
N580 X3.369
N590 X2.795
N600 G02 X2.556 Y1.055 R.291
N610 G01 X.813
N620 G02 X.574 Y.93 R.291
N630 G01 X0
N640 X-.138
N650 Y.762
N660 X0
N670 X.574
N680 G02 X.813 Y.637 R.291
N690 G01 X2.556
N700 G02 X2.795 Y.762 R.291
N710 G01 X3.369
N720 X3.507
N730 Y.93
N740 G00 Z.1
N750 Z0
N760 G01 Z-.15 F6.25
N770 X3.369 F50.
N780 X2.795
N790 G02 X2.556 Y1.055 R.291
N800 G01 X.813
N810 G02 X.574 Y.93 R.291
N820 G01 X0
N830 X-.138
N840 Y.762
N850 X0
N860 X.574
N870 G02 X.813 Y.637 R.291
N880 G01 X2.556
N890 G02 X2.795 Y.762 R.291
N900 G01 X3.369
N910 X3.507
N920 Y.93
N930 X3.369
N940 X2.795
N950 G02 X2.556 Y1.055 R.291
N960 G01 X.813
N970 G02 X.574 Y.93 R.291
N980 G01 X0
N990 X-.138
N1000 Y.762
N1010 X0
N1020 X.574
N1030 G02 X.813 Y.637 R.291
N1040 G01 X2.556
N1050 G02 X2.795 Y.762 R.291
N1060 G01 X3.369
N1070 X3.507
N1080 Y.93
N1090 G00 Z.1
N1100 Z-.05
N1110 G01 Z-.2 F6.25
N1120 X3.369 F50.
N1130 X2.795
N1140 G02 X2.556 Y1.055 R.291
N1150 G01 X.813
N1160 G02 X.574 Y.93 R.291
N1170 G01 X0
N1180 X-.138
N1190 Y.762
N1200 X0
N1210 X.574
N1220 G02 X.813 Y.637 R.291
N1230 G01 X2.556
N1240 G02 X2.795 Y.762 R.291
N1250 G01 X3.369
N1260 X3.507
N1270 Y.93
N1280 X3.369
N1290 X2.795
N1300 G02 X2.556 Y1.055 R.291
N1310 G01 X.813
N1320 G02 X.574 Y.93 R.291
N1330 G01 X0
N1340 X-.138
N1350 Y.762
N1360 X0
N1370 X.574
N1380 G02 X.813 Y.637 R.291
N1390 G01 X2.556
N1400 G02 X2.795 Y.762 R.291
N1410 G01 X3.369
N1420 X3.507
N1430 Y.93
N1440 G00 Z.1
N1450 Z-.1

[keen]

Hi - I don't see the G20 or g21 section. If you are in inches - G20 - then 6.25 is very fast. Or are you in metric G21?

keen

[DasNewb]

I'm in inches (G20). This is just a quick program that I genereated with CAMworks and haven't worked out the feed/speed/RPMs yet. I'm just noticing this issue while air cutting.

[keen]

OK well typically you want a Z feed in metal around F2

Keen

[wildwhl]

I'm not familiar with CAMworks - but have you set the cutting/ramp/plunge feedrates for the operation and/or tool appropriately? If so - are you seeing the rates you've setup in the code you've posted?

Bill

[DasNewb]

Ok, I think I know whats going on here. It seems like the controller is trying to execute the next line of code too early, which is why the X feed rate is being applied to the residual Z travel. If I change all of the feed rates to one common number, the problem stops. But that isn't really a solution because I'm not going to cut in X and Y at F2.

Maybe I can insert a dwell command after every Z movement to distinctly separate the execution time. That would really be a pain if I had to do that for every single z movement in every program I make -_-.

Any suggestions?

[keen]

Just checking you don't have one of the sliders choking off the feed rate ?

This shows up more on the faster feeds and caught me out in the beginning.

keen

[DasNewb]

Problem solved. I hope this helps for anyone facing this issue.

Path Pilot had blending enabled. Inserting G61 at the beginning of my code solved my issue.

Thanks for the help everyone.

[tmarks11]

I think there is something else going on here.

G64 (the opposite of G61) is the default mode for linuxcnc (and PP).

Indeed, Tormach specifies in their manuals to have this in your "safety block" at the beginning of your cnc programs;

N2 G90 G80 G40 G54 G20 G17 G50 G94 G64 (SAFETY BLOCK)

G64 specifies that the cut can depart from the programmed path by the specified P & Q values, whereas G61 demands "exact cut", which could make your cut path somewhat jerky. The trajectory planner was an area of the core linuxcnc that Tormach funded development of. Note the Linuxcnc manual warning quoted below.

What version of PP are your running?

G61 (exact stop mode): G61 tells the planner to come to an exact stop at every segment's end. This ensures exact path following but the full stops can be harmful to the workpiece or the tooling, depending on the particular cut.

G64 (continuous mode): G64 tells the planner to sacrifice path following accuracy in order to keep the feed rate up. This is necessary for some types of material or tooling where exact stops are harmful, and can work great as long as the programmer is careful to keep in mind that the tool's path will be somewhat more curvy than the program specifies.

LinuxCNC Documentation Wiki: TrajectoryControl

None of which explains why you are plunging at greater than the specified speed. Sounds like a bug.