Driving me a little NUTZZZ!

[Cellar Dweller]

Driving me a little NUTZZZ!

Mastercam X3
1995 BP Discovery DX-32 Controller.
Also posted in BP Forum.

Hi all,

I am attempting to perform a drill peck operation. However, I am having trouble. Please note line 5120. This is the first time I am (actually my PP is calling) using a G83, (deep hole, pecking, rapid out, on my control) and the VMC does not like it!

The tool loads, coolant on, rapids to CP, and starts to peck, and peck some more and then peck again. LOL But it is not dropping in the Z, it is getting stuck in some type of loop. It will sit their for an hour going up about .1 and back down about .1 over and over, never touching the part. To me the Z heights look odd in the post (see Below N5160) they should be –z values and the three z values following each other seem like they could confuse the controller. The reason I allowed the machine to run the program is because, as I said, it was my first use of the G83 and was am a little courageous or dumb, but I like to see what happens so I learn.

Also, important, I gave you the code from N3630 (which works very nice) because that is the same operation "drill peck", (with a different tool, in a different spot) but I selected all the same options in MC and I don’t understand why MC or PP is forcing me to use the G83??? I even copied and pasted the N3630 op and changed the tool hoping it would use G1 but somehow it refuses to use a G1. I even selected a .125 end mill and screen shot the MC set up and they look the same, but it keeps posting the G83 with the odd +z values.

First, do any of your fresh eyes see a clear mistake / problem?
Second, WHY wont MC post this op out as a G1 like it did with the .3125 cutter, instead of the G83. I cannot figure this one out?

Thanks a lot, this forum has been invaluable.
CD

' 5/16 FLAT ENDMILL - TOOL3 - DIA .312 '
N3630 T3 M6
N3640 S4897 M03
N3650 G0 X2.2765 Y-.2973
N3660 G0 Z.25 M08
N3670 G0 Z.1
N3680 G99 G1 X2.2765 Y-.2973 Z-.1084 F6.4
N3690 G99 X2.2767 Y-.2972 F12.1
N3700 G99 X2.2768 Y-.297
N3710 G99 X2.2767 Y-.2968
N3720 G99 X2.2765 Y-.2967
N3730 G99 X2.2765 Y-.2968 Z-.0084 F6.4
N3740 G0 Z.25
N3750 G0 Y-.2973
N3760 G0 Z-.0084
N3770 G99 G1 X2.2765 Y-.2973 Z-.2168
N3780 G99 X2.2767 Y-.2972 F12.1
N3790 G99 X2.2768 Y-.297
N3800 G99 X2.2767 Y-.2968
N3810 G99 X2.2765 Y-.2967
N3820 G99 X2.2765 Y-.2968 Z-.1168 F6.4
N3830 G0 Z.25
N3840 G0 Y-.2973
N3850 G0 Z-.1168
N3860 G99 G1 X2.2765 Y-.2973 Z-.3252
N3870 G99 X2.2767 Y-.2972 F12.1
N3880 G99 X2.2768 Y-.297
N3890 G99 X2.2767 Y-.2968
N3900 G99 X2.2765 Y-.2967
N3910 G99 X2.2765 Y-.2968 Z-.2252 F6.4
N3920 G0 Z.25
N3930 G0 Y-.2973
N3940 G0 Z-.2252
N3950 G99 G1 X2.2765 Y-.2973 Z-.4336
N3960 G99 X2.2767 Y-.2972 F12.1
N3970 G99 X2.2768 Y-.297
N3980 G99 X2.2767 Y-.2968
N3990 G99 X2.2765 Y-.2967
N4000 G99 X2.2765 Y-.2968 Z-.3336 F6.4
N4010 G0 Z.25
N4020 G0 Y-.2973
N4030 G0 Z-.3336
N4040 G99 G1 X2.2765 Y-.2973 Z-.542
N4050 G99 X2.2767 Y-.2972 F12.1
N4060 G99 X2.2768 Y-.297
N4070 G99 X2.2767 Y-.2968
N4080 G99 X2.2765 Y-.2967
N4090 G99 X2.2765 Y-.2968 Z-.442 F6.4
N4100 G0 Z.25
N4110 G0 Y-.2973
N4120 G0 Z-.442
N4130 G99 G1 X2.2765 Y-.2973 Z-.552
N4140 G99 X2.2767 Y-.2972 F12.1
N4150 G99 X2.2768 Y-.297
N4160 G99 X2.2767 Y-.2968
N4170 G99 X2.2765 Y-.2967
N4180 G0 Z-.1084
N4190 G99 G1 X2.0745 Y-.2968
N4200 G99 X2.0745 Y-.2968 Z-.0084 F6.4
N4210 G0 Z.25
N4220 G0 X2.2765
N4230 G0 Z-.0084
N4240 G99 G1 X2.2765 Y-.2968 Z-.2168
N4250 G99 X2.0745 Y-.2968 F12.1
N4260 G99 X2.0745 Y-.2968 Z-.1168 F6.4
N4270 G0 Z.25
N4280 G0 X2.2765
N4290 G0 Z-.1168
N4300 G99 G1 X2.2765 Y-.2968 Z-.3252
N4310 G99 X2.0745 Y-.2968 F12.1
N4320 G99 X2.0745 Y-.2968 Z-.2252 F6.4
N4330 G0 Z.25
N4340 G0 X2.2765
N4350 G0 Z-.2252
N4360 G99 G1 X2.2765 Y-.2968 Z-.4336
N4370 G99 X2.0745 Y-.2968 F12.1
N4380 G99 X2.0745 Y-.2968 Z-.3336 F6.4
N4390 G0 Z.25
N4400 G0 X2.2765
N4410 G0 Z-.3336
N4420 G99 G1 X2.2765 Y-.2968 Z-.542
N4430 G99 X2.0745 Y-.2968 F12.1
N4440 G99 X2.0745 Y-.2968 Z-.442 F6.4
N4450 G0 Z.25
N4460 G0 X2.2765
N4470 G0 Z-.442
N4480 G99 G1 X2.2765 Y-.2968 Z-.552
N4490 G99 X2.0745 Y-.2968 F12.1
N4500 G0 Z-.1084
N4510 G99 G1 X2.0743 Y-.297
N4520 G99 X2.0745 Y-.2972
N4530 G99 X2.2765 Y-.2973
N4540 G99 X2.2765 Y-.2973 Z-.0084 F6.4
N4550 G0 Z.25
N4560 G0 X2.0745 Y-.2968
N4570 G0 Z-.0084
N4580 G99 G1 X2.0745 Y-.2968 Z-.2168
N4590 G99 X2.0743 Y-.297 F12.1
N4600 G99 X2.0745 Y-.2972
N4610 G99 X2.2765 Y-.2973
N4620 G99 X2.2765 Y-.2973 Z-.1168 F6.4
N4630 G0 Z.25
N4640 G0 X2.0745 Y-.2968
N4650 G0 Z-.1168
N4660 G99 G1 X2.0745 Y-.2968 Z-.3252
N4670 G99 X2.0743 Y-.297 F12.1
N4680 G99 X2.0745 Y-.2972
N4690 G99 X2.2765 Y-.2973
N4700 G99 X2.2765 Y-.2973 Z-.2252 F6.4
N4710 G0 Z.25
N4720 G0 X2.0745 Y-.2968
N4730 G0 Z-.2252
N4740 G99 G1 X2.0745 Y-.2968 Z-.4336
N4750 G99 X2.0743 Y-.297 F12.1
N4760 G99 X2.0745 Y-.2972
N4770 G99 X2.2765 Y-.2973
N4780 G99 X2.2765 Y-.2973 Z-.3336 F6.4
N4790 G0 Z.25
N4800 G0 X2.0745 Y-.2968
N4810 G0 Z-.3336
N4820 G99 G1 X2.0745 Y-.2968 Z-.542
N4830 G99 X2.0743 Y-.297 F12.1
N4840 G99 X2.0745 Y-.2972
N4850 G99 X2.2765 Y-.2973
N4860 G99 X2.2765 Y-.2973 Z-.442 F6.4
N4870 G0 Z.25
N4880 G0 X2.0745 Y-.2968
N4890 G0 Z-.442
N4900 G99 G1 X2.0745 Y-.2968 Z-.552
N4910 G99 X2.0743 Y-.297 F12.1
N4920 G99 X2.0745 Y-.2972
N4930 G99 X2.2765 Y-.2973
N4940 G99 X2.2765 Y-.2973 Z-.452 F6.4
N4950 G0 Z.25
N4960 G0 Z.1
N4970 G83 X2.1755 Y-.297 Z.95 Z.1 Z.1 F7.3
N4980 G80
N4990 M09
N5000 G00 M25
' .1875 SPOTDRILL - TOOL6 - DIA .188 '
N5010 T6 M6
N5020 S4889 M03
N5030 G0 X.704 Y-.297
N5040 G0 Z.1
N5050 G81 X.704 Y-.297 Z.195 F9.8
N5060 G80
N5070 G81 X2.573 Y-.297 Z.3 F9.8
N5080 X1.778
N5090 G80
N5100 M09
N5110 G00 M25
' 1/8 DRILL - TOOL4 - DIA .125 ' (PROBLEM OP!!!!!!!!!!!!!!)
N5120 T4 M6
N5130 S7334 M03
N5140 G0 X.704 Y-.297
N5150 G0 Z.1 M08
N5160 G83 X.704 Y-.297 Z.5976 Z.0375 Z0. F8.4
N5170 G80
N5180 M09
N5190 G00 M25
' NO. 6-32 TAPRH - TOOL5 - DIA .138 '
N5200 T5 M6
N5210 S300 M03
N5220 G0 X6.1282 Y-.2959
N5230 G0 Z2. M08
N5240 M29
N5250 G84 X6.1282 Y-.2959 Z.3 F9.4
N5260 G80 M28
N5270 M09
N5280 G00 M25

[colton_m]

At first glance it looks like your post is not posting proporly!

A peck cycle should have more letters following the G83 (Z, F, R, Q, P).

First off, on line 5140 you rapid to the location for the hole, this means you do not have to re-specify the location at the G83. Next you are missing R, Q and P. P is a dwell (at the bottom of the hole) so it can be left out if you desire, but the R and Q are important!

Your G83 line should look something like this,

N5160 G83 Z-.5976 F8.4 Q0.125 R0.1

Where:
Z = total hole depth
F = feed
Q = Peck ammount
R = Retract ammount

Give this a try, It should work better:

1/8 DRILL - TOOL4 - DIA .125 ' (PROBLEM OP!!!!!!!!!!!!!!)
N5120 T4 M6
N5130 S7334 M03
N5140 G0 X.704 Y-.297
N5150 G0 Z.1 M08
N5160 G83 Z-.5976 F8.4 Q0.125 R0.1
N5170 G80
N5180 M09

[Superman]

N5040 G0 Z.1 N5050 G81 X.704 Y-.297 Z.195 F9.8 N5060 G80 N5070 G81 X2.573 Y-.297 Z.3 F9.8 N5080 X1.778 N5090 G80 N5100 M09 N5110 G00 M25 ' 1/8 DRILL - TOOL4 - DIA .125 ' (PROBLEM OP!!!!!!!!!!!!!!) N5120 T4 M6 N5130 S7334 M03 N5140 G0 X.704 Y-.297 N5150 G0 Z.1 M08 N5160 G83 X.704 Y-.297 Z.5976 Z.0375 Z0. F8.4

Is Z0 the top of your part ?
Why come down to Z0.1"
And the Z depths are above this point

I understand the multiple Z's on N5160 being pecking depths but the 1st one is still above the Z.1 ??????

In Mastercam, recheck all your levels ( clearance, retract, depth, abs/inc etc ) as something is not set correctly

Colton_m is giving a solution for Fanuc type controls,
But yours is a bridgeport and a little bit different

[Cellar Dweller]

MMMMM, ok. Well, I have some cleanup work and figuring out with regard to why the Z.1 appears all over and so forth when I am not calling it out as a retract.

Yes, the top of the finished part is Z0.

In my first post explaining my problem and looking at the Gcode I made an error. The program DOES actually call a G83 prior to this one. Please note line 4970. That op works correctly?? But it does. The whole program produces a dimensionally accurate part (so far) and moves as expected until line 5160 in which the “looping” starts. Thankfully no crash.

I though perhaps the control was running out of space (older machine) or something. So I deleted the problem op and added the tapping op you see at the end. (it is just tapping off the part in free air) That all executed properly with no problem. Program ended, table parked, quill up, coolant off, etc. So I don’t think it is a controller “head room” problem.

During this looping, the controllers “next” line appears to be a copy of line 5160, but as you can see, there is no copy of 5160, it does not repeat.???? Why does the controller display it as next? I was thinking that it was a video card type of glitch and when the real looping problem was discovered this would not appear. Basically, I am assuming the video card can’t display the correct line info for the same reason the machine is looping.

Also, why the conflicting Z values, but it works?
Line 4970 lists all ZPlus values, but it drills a hole down correctly into the part to the correct depth. In the last op listed here you see the tap listed at z.3 when I know for a fact it is set to -.3 in MC and also I watched it tap in a z- fashion with my own eyes. As I am typing this right now, I am starting to think that my controller or mc understands “drill cycles” as zplus for zneg and the post is written correct, at least in that aspect. Like I said, 4970 drills down and MC parameters are set to depth = -.95, not .95 as stated in the post.

The only thing I see different in terms formatting of 4970 (working correctly) and 5160 (not working correctly) is the prior M08 on 5150 verse it not being there on 4960.
Thanks all,
CD

[ObrienDave]

I think the problem is the 3rd Z value in line 5160.
I assume the 2nd Z is the 1st peck value and the 3rd Z is subsequent peck value.
Since the value is zero you get the endless loop.
Since M08 is a flood coolant call, I doubt it has anything to do with the coding problem.

[Cellar Dweller]

Update.
First, I got some confirmation, and field verified that my controller treats drill cycles with positive z values, which is why the part is In tol to this point. It does make reviewing the code a pain in the butt. Anyway, the z+ values are actually z- values as it relates to part zero, in my case the top of the part.

Second, the looping issue. No matter what I did in MC, it refused to post the correct z values. So, moved the part to a different PC, and it started posting correctly. So, I told the tech guys who simply replaced the workstation and all was cool. It would seem, that something type of bug occurred in MC, my post, or Windows XP, etc. It posted the first drill cycle correctly, but just refused on the next ones. I will not spend any time trying to figure that one out. One of the lesson I learned this go around was if you can, jump to another workstation and remember to always look for the simple solutions first.

I also learned that whoever designed that BP controller is crazy!! ZNEG = ZNEG Period! LOL, IMHO.

Thanks to everybody,
CD