Need Help!- machine moves WAY off part before next move

[rmason]

can some one take a look at my program- this was done in bobcad19 it is an array of rectangles. After the first few rectangles are done the machine moves way off (5-6") with z down then comes back to the next rectangle. I tried turning trig help off (special flag 001) but no difference. it seems I always have some sort of issue when using cutter comp. Probably me but still frustrating! The program verfies fine with no c.c. here is a partial of the program- I am using a 1/8 tool- I will email the prog to anyone who needs it

(ALN ARRAY REWORK)
N10 G17 G90 G12 G20 G41
N20 M06 T1 G43 H1
N30 G00 Z0.025
N40 X0.595 Y2.2975
N50 G01 Z-0.09F3
N60 X-0.595F20
N70 Y1.5025
N80 X0.595
N90 Y2.2975
N100 G00 Z0.025 G40
G41
N110 X-1.2038 Y2.0453
N120 G01 Z-0.09F3
N130 X-2.0453 Y1.2038F20
N140 X-1.4832 Y0.6417
N150 X-0.6417 Y1.4832
N160 X-1.2038 Y2.0453
N170 G00 Z0.025G40
G41
N180 X-2.2975 Y0.595
N190 G01 Z-0.09F3
N200 Y-0.595F20
N210 X-1.5025
N220 Y0.595
N230 X-2.2975
N240 G00 Z0.025 G40
G41
N250 X-1.4832 Y-0.6417
N260 G01 Z-0.09F3
N270 X-2.0453 Y-1.2038F20
N280 X-1.2038 Y-2.0453
N290 X-0.6417 Y-1.4832
N300 X-1.4832 Y-0.6417
N310 G00 Z0.025 G40
G41
N320 X-0.595 Y-1.5025
N330 G01 Z-0.09F3
N340 Y-2.2975F20
N350 X0.595
N360 Y-1.5025
N370 X-0.595
N380 G00 Z0.025 G40
G41
N390 X0.6417 Y-1.4832
N400 G01 Z-0.09F3
N410 X1.2038 Y-2.0453F20
N420 X2.0453 Y-1.2038
N430 X1.4832 Y-0.6417
N440 X0.6417 Y-1.4832
N450 G00 Z0.025 G40
G41
N460 X1.5025 Y-0.595
N470 G01 Z-0.09F3
N480 X2.2975F20
N490 Y0.595
N500 X1.5025
N510 Y-0.595
N520 G00 Z0.025 G40
G41
N530 X1.4832 Y0.6417
N540 G01 Z-0.09F3
N550 X2.0453 Y1.2038F20
N560 X1.2038 Y2.0453
N570 X0.6417 Y1.4832
N580 X1.4832 Y0.6417
N590 G00 Z0.025 G40
G41
N600 X2.482 Y0.746
N610 G01 Z-0.09F3
N620 X3.1705 Y1.1435F20
N630 X2.5755 Y2.174
N640 X1.887 Y1.7765
N650 X2.482 Y0.746
N660 G00 Z0.025 G40
G41
N670 X1.7765 Y1.887
N680 G01 Z-0.09F3
N690 X2.174 Y2.5755F20
N700 X1.1435 Y3.1705
N710 X0.746 Y2.482
N720 X1.7765 Y1.887
N730 G00 Z0.025 G40
G41
N740 X0.595 Y2.5225
N750 G01 Z-0.09F3
N760 Y3.3175F20
N770 X-0.595
N780 Y2.5225
N790 X0.595
N800 G00 Z0.025 G40
G41
N810 X-0.746 Y2.482
N820 G01 Z-0.09F3
N830 X-1.1435 Y3.1705F20
N840 X-2.174 Y2.5755
N850 X-1.7765 Y1.887
N860 X-0.746 Y2.482
N870 G00 Z0.025 G40
G41
N880 X-1.887 Y1.7765
N890 G01 Z-0.09F3
N900 X-2.5755 Y2.174F20
N910 X-3.1705 Y1.1435
N920 X-2.482 Y0.746
N930 X-1.887 Y1.7765
N940 G00 Z0.025 G40
G41
N950 X-2.5225 Y0.595
N960 G01 Z-0.09F3
N970 X-3.3175F20
N980 Y-0.595
N990 X-2.5225
N1000 Y0.595
N1010 G00 Z0.025 G40
G41
N1020 X-2.482 Y-0.746
N1030 G01 Z-0.09F3
N1040 X-3.1705 Y-1.1435F20
N1050 X-2.5755 Y-2.174
N1060 X-1.887 Y-1.7765
N1070 X-2.482 Y-0.746
N1080 G00 Z0.025 G40
G41
N1090 X-1.7765 Y-1.887
N1100 G01 Z-0.09F3
N1110 X-2.174 Y-2.5755F20
N1120 X-1.1435 Y-3.1705
N1130 X-0.746 Y-2.482
N1140 X-1.7765 Y-1.887
N1150 G00 Z0.025 G40
G41
N1160 X-0.595 Y-2.5225
N1170 G01 Z-0.09F3
N1180 Y-3.3175F20
N1190 X0.595
N1200 Y-2.5225
N1210 X-0.595
N1220 G00 Z0.025 G40
G41
N1230 X0.746 Y-2.482
N1240 G01 Z-0.09F3
N1250 X1.1435 Y-3.1705F20
N1260 X2.174 Y-2.5755
N1270 X1.7765 Y-1.887
N1280 X0.746 Y-2.482
N1290 G00 Z0.025 G40
G41
N1300 X1.887 Y-1.7765
N1310 G01 Z-0.09F3
N1320 X2.5755 Y-2.174F20
N1330 X3.1705 Y-1.1435
N1340 X2.482 Y-0.746
N1350 X1.887 Y-1.7765
N1360 G00 Z0.025 G40
G41
N1370 X2.5225 Y-0.595
N1380 G01 Z-0.09F3
N1390 X3.3175F20
N1400 Y0.595
N1410 X2.5225
N1420 Y-0.595
N1430 G00 Z0.025 G40
G41
N1440 X3.4436 Y0.5889
N1450 G01 Z-0.09F3
N1460 X4.1929 Y0.8544F20
N1470 X3.7955 Y1.976
N1480 X3.0461 Y1.7105
N1490 X3.4436 Y0.5889
N1500 G00 Z0.025 G40
G41
N1510 X2.9635 Y1.8499
N1520 G01 Z-0.09F3
N1530 X3.5564 Y2.3796F20
N1540 X2.7635 Y3.267
N1550 X2.1707 Y2.7373
N1560 X2.9635 Y1.8499
N1570 G00 Z0.025 G40
G41
N1580 X2.0414 Y2.835
N1590 G01 Z-0.09F3
N1600 X2.3893 Y3.5499F20
N1610 X1.3193 Y4.0706
N1620 X0.9714 Y3.3558
N1630 X2.0414 Y2.835
N1640 G00 Z0.025 G40
G41
N1650 X0.8147 Y3.3972
N1660 G01 Z-0.09F3
N1670 X0.8658 Y4.1906F20
N1680 X-0.3218 Y4.267
N1690 X-0.3728 Y3.4736
N1700 X0.8147 Y3.3972
N1710 G00 Z0.025 G40

[HuFlungDung]

I am not sure what the problem would be, however, I would not cancel compensation (G40) on a Z movement alone, because the intended use of radius comp requires that the tool move from one XY position that is radius compensated, to another XY position that is not compensated.

When you cancel compensation on a Z move, relying on the modal XY values, the control has no sense of 'from' and 'to' because the axis address is not changing.

So G00 to a starting XYZ point, then feed down in Z, turn comp on with a new XY feed move (lead-in) to put the tool tangent to the path geometry. When finished with the cut, feed to a final XY position clear of the geometry (lead-out) as you cancel comp with the G40. Then rapid to clearance and continue on with the same basic sequence.

[One of Many]

rmason,

It looks like your post processor could use some rework. I do not use bobcad, so I can't help there.

What I did was replace the header you have with one I use, then added my ending at N1711-1730.

G12 is modal(once set, it remains active until changed by another code) for clearing the floating zero after a G92 set floating zero. I cannot imagine it necessary in the initializing header.

G41 is also modal. Once the cutter comps to the left it stays to the left. Your progam turns comp off then back on again several times. No ryme or reason for that which could cause strange glitches. The cam system I use places the cutter offset within the path, so all path positions are centerline of the cutter. If I choose to have cutter comp on, then it is used for fine tuning the cut dimensions.

On the initial startup, the Z rapids to the clearance plane then rapids in x and y. I have edited that so that it is in X,Y position before the Z comes down. Could be critical in some circumstances. I have also added in G90 for absolute dimensions and using G54 work coordinates as the center of your array. The machine default is G54, but I take no chances just in case a stray finger has switched in on me when I wasn't looking.

Other than that, your description reminds me of one condition I had found in a pocket clearing program that baffled us. It also verified good on the cam system, but took off in a 30" arc on the machine in an attempt to go back to where it was. Changing the step over or cutter diameter by .0001 resolved the problem. Not sure if that is another example of floating decimal point arithmatic conflicts or not. Frustrating when it happens!

Anyways, try this little bit and see if it resolves your main issue.

DC


O100
(PROGRAM: ARRAY)
(OPERATION: 1)
(TOOL 1: 0.125 DIA.)
N10 G17G20G32G41G80
N20 T1M06 G43 H1
N25 G90G54 G00 X0.595 Y2.2975
N30 G00 Z0.025
N40 (X0.595 Y2.2975)
N50 G01 Z-0.09F3
N60 X-0.595F20
N70 Y1.5025
N80 X0.595
N90 Y2.2975
N100 G00 Z0.025
N110 X-1.2038 Y2.0453
N120 G01 Z-0.09F3
N130 X-2.0453 Y1.2038F20
N140 X-1.4832 Y0.6417
N150 X-0.6417 Y1.4832
N160 X-1.2038 Y2.0453
N170 G00 Z0.025
N180 X-2.2975 Y0.595
N190 G01 Z-0.09F3
N200 Y-0.595F20
N210 X-1.5025
N220 Y0.595
N230 X-2.2975
N240 G00 Z0.025
N250 X-1.4832 Y-0.6417
N260 G01 Z-0.09F3
N270 X-2.0453 Y-1.2038F20
N280 X-1.2038 Y-2.0453
N290 X-0.6417 Y-1.4832
N300 X-1.4832 Y-0.6417
N310 G00 Z0.025
N320 X-0.595 Y-1.5025
N330 G01 Z-0.09F3
N340 Y-2.2975F20
N350 X0.595
N360 Y-1.5025
N370 X-0.595
N380 G00 Z0.025
N390 X0.6417 Y-1.4832
N400 G01 Z-0.09F3
N410 X1.2038 Y-2.0453F20
N420 X2.0453 Y-1.2038
N430 X1.4832 Y-0.6417
N440 X0.6417 Y-1.4832
N450 G00 Z0.025
N460 X1.5025 Y-0.595
N470 G01 Z-0.09F3
N480 X2.2975F20
N490 Y0.595
N500 X1.5025
N510 Y-0.595
N520 G00 Z0.025
N530 X1.4832 Y0.6417
N540 G01 Z-0.09F3
N550 X2.0453 Y1.2038F20
N560 X1.2038 Y2.0453
N570 X0.6417 Y1.4832
N580 X1.4832 Y0.6417
N590 G00 Z0.025
N600 X2.482 Y0.746
N610 G01 Z-0.09F3
N620 X3.1705 Y1.1435F20
N630 X2.5755 Y2.174
N640 X1.887 Y1.7765
N650 X2.482 Y0.746
N660 G00 Z0.025
N670 X1.7765 Y1.887
N680 G01 Z-0.09F3
N690 X2.174 Y2.5755F20
N700 X1.1435 Y3.1705
N710 X0.746 Y2.482
N720 X1.7765 Y1.887
N730 G00 Z0.025
N740 X0.595 Y2.5225
N750 G01 Z-0.09F3
N760 Y3.3175F20
N770 X-0.595
N780 Y2.5225
N790 X0.595
N800 G00 Z0.025
N810 X-0.746 Y2.482
N820 G01 Z-0.09F3
N830 X-1.1435 Y3.1705F20
N840 X-2.174 Y2.5755
N850 X-1.7765 Y1.887
N860 X-0.746 Y2.482
N870 G00 Z0.025
N880 X-1.887 Y1.7765
N890 G01 Z-0.09F3
N900 X-2.5755 Y2.174F20
N910 X-3.1705 Y1.1435
N920 X-2.482 Y0.746
N930 X-1.887 Y1.7765
N940 G00 Z0.025
N950 X-2.5225 Y0.595
N960 G01 Z-0.09F3
N970 X-3.3175F20
N980 Y-0.595
N990 X-2.5225
N1000 Y0.595
N1010 G00 Z0.025
N1020 X-2.482 Y-0.746
N1030 G01 Z-0.09F3
N1040 X-3.1705 Y-1.1435F20
N1050 X-2.5755 Y-2.174
N1060 X-1.887 Y-1.7765
N1070 X-2.482 Y-0.746
N1080 G00 Z0.025
N1090 X-1.7765 Y-1.887
N1100 G01 Z-0.09F3
N1110 X-2.174 Y-2.5755F20
N1120 X-1.1435 Y-3.1705
N1130 X-0.746 Y-2.482
N1140 X-1.7765 Y-1.887
N1150 G00 Z0.025
N1160 X-0.595 Y-2.5225
N1170 G01 Z-0.09F3
N1180 Y-3.3175F20
N1190 X0.595
N1200 Y-2.5225
N1210 X-0.595
N1220 G00 Z0.025
N1230 X0.746 Y-2.482
N1240 G01 Z-0.09F3
N1250 X1.1435 Y-3.1705F20
N1260 X2.174 Y-2.5755
N1270 X1.7765 Y-1.887
N1280 X0.746 Y-2.482
N1290 G00 Z0.025
N1300 X1.887 Y-1.7765
N1310 G01 Z-0.09F3
N1320 X2.5755 Y-2.174F20
N1330 X3.1705 Y-1.1435
N1340 X2.482 Y-0.746
N1350 X1.887 Y-1.7765
N1360 G00 Z0.025
N1370 X2.5225 Y-0.595
N1380 G01 Z-0.09F3
N1390 X3.3175F20
N1400 Y0.595
N1410 X2.5225
N1420 Y-0.595
N1430 G00 Z0.025
N1440 X3.4436 Y0.5889
N1450 G01 Z-0.09F3
N1460 X4.1929 Y0.8544F20
N1470 X3.7955 Y1.976
N1480 X3.0461 Y1.7105
N1490 X3.4436 Y0.5889
N1500 G00 Z0.025
N1510 X2.9635 Y1.8499
N1520 G01 Z-0.09F3
N1530 X3.5564 Y2.3796F20
N1540 X2.7635 Y3.267
N1550 X2.1707 Y2.7373
N1560 X2.9635 Y1.8499
N1570 G00 Z0.025
N1580 X2.0414 Y2.835
N1590 G01 Z-0.09F3
N1600 X2.3893 Y3.5499F20
N1610 X1.3193 Y4.0706
N1620 X0.9714 Y3.3558
N1630 X2.0414 Y2.835
N1640 G00 Z0.025
N1650 X0.8147 Y3.3972
N1660 G01 Z-0.09F3
N1670 X0.8658 Y4.1906F20
N1680 X-0.3218 Y4.267
N1690 X-0.3728 Y3.4736
N1700 X0.8147 Y3.3972
N1710 G00 Z0.025
N1711M09
N1715G32
N1720M05
N1725G53G0Y0
N1730M30

[merl]

I would have to agree with one of many,
don't keep tuning the comp on and off , turn it on at the beging of the program and leave it on. You said the program "verifies" with the cutter comp off, if it doesn't verifiy with the comp on as well then you have an error in your program (maybe trying to crowd the comped tool into too tight a space...?) I'm sure the programing is faster with the cam system but why don't you try to wright the program in conversational format at the machine and see if that works. Then you might show a problem with your post or your cam system and your machine compatibility...?

[HuFlungDung]

I've never worked with a control that applied radius compensation to a G00 movement, therefore, I would be wondering about the validity of the argument that turning comp on and off is harmful. Even though radius compensation is a modal command, some controllers will not compensate a positioning (rapid) movement. This amounts to the same thing as turning comp off involuntarily, and the machine will require one feed movement after each rapid, in order to get the cutter tangent to the profile again.

The problem I see by viewing the backplot of the original code is that there is no lead in and no lead out provided for each profile. Cutting inside of a rectangle requires a minimum of 6 movements: one for lead on, 4 for the profile, and one move to get off the profile before comp cancels (if it does when reading the G00 Z movement).

I use full radius compensation, not wear comp, so I'd definitely notice a starting gouge whereas the guys who run wear comp might not notice anything.

In all situations that I can think of, I'd certainly not want the tool descending immediately tangent to the profile under the conditions of obtaining a good finish. Hence, my perceived requirement of a lead in and a lead out to every profile. Under these conditions, it does no harm whatsoever to turn comp on and off, all that matters is that it be done properly, and with command syntax that is acceptable to the control.

[mactec54]

Hi rmason
one of many has said to put your Z move after the X&Y move this is a mistake as if you do a G0 X&Y move & the Z is down you will crash your tool into your job

Always move the Z to a safe work clearance before a G0X&Y move!! you will crash if you don't,

If you are having trouble with cutter comp turn it off & just do your program to suit the tool dia you are using

[One of Many]

Originally Posted by mactec54 Hi rmason one of many has said to put your Z move after the X&Y move this is a mistake as if you do a G0 X&Y move & the Z is down you will crash your tool into your job Always move the Z to a safe work clearance before a G0X&Y move!! you will crash if you don't, If you are having trouble with cutter comp turn it off & just do your program to suit the tool dia you are using

No, One of Many sayz the exact opposite, sooooo re-read my suggestion, see my edited version and rem'd out the X,Y move after the Z move and placed it before the Z move. The way it was originally, which is technically a dangerous condition as noted in my previous post.

You do back up my point, though this is a post processor excuse in poor practice. One must learn the difference before knowing safer from potential disaster. A hair trigger on the feed over ride knob is a backup plan, not a fail safe for the unknown.

DC

[mactec54]

Hi one of many
Your write up says for the Z to move to the clearance plane

But your EDITED VERSION OF THE G CODE the X&Y will RAPID before the Z Axes moves
which Means CRASH

Your FIRST LINE OF CODE IS G00 X0.595 Y2.2975 THERE IS NO Z MOVE BEFORE THIS
CALL

rmason had this part of the program correct & only has the cutter comp messed up

[One of Many]

Originally Posted by mactec54 Hi one of many Your write up says for the Z to move to the clearance plane But your EDITED VERSION OF THE G CODE the X&Y will RAPID before the Z Axes moves which Means CRASH Your FIRST LINE OF CODE IS G00 X0.595 Y2.2975 THERE IS NO Z MOVE BEFORE THIS CALL rmason had this part of the program correct & only has the cutter comp messed up

Here is what I said that first refers to the way it WAS WRITTEN and how I changed it; My apologies if it is not clear enough.

On the initial startup, the Z rapids to the clearance plane then rapids in x and y. I have edited that so that it is in X,Y position before the Z comes down.

In addition to my edit and you may have missed, since I didn't mention it earlier. The initial Z is still up( from the G32 "Z to tool change" in the header) and is also BEFORE the first X,Y move.......so, what is going to crash?

I THOUGHT this was the very concern you were making in putting the Z at clearance before a rapid in X,Y as poor practice. Now you are saying it was correct in the original? Which is exactly what that program does.

My edit placed the first X,Y move BEFORE the Z comes down from the tool change position. N40 has (X0.595 Y2.2975) the () rems out the line.

When the program initializes, the Z goes up to tool change, the X,Y rapids to position and then the Z comes down to the clearance plane. That is the safest method I'd offer as a precaution, but to each his own.

I hope this is clearer.

DC

[mactec54]

Hi one of many

Sorry I did miss the G32 But this is a wast of Z movement which could be as much as 15" from the part if the operator has just touched off the tool the Z will go to the tool
change position & then have to come back down again another 15" a total of 30'' of movement that is not needed if you set the Z to your clearance plane, & is the first move the machine does you save all that extra Z movement that you have added by
not having to go back up to the tool change position Ballscrews will last a lot longer to

[One of Many]

Originally Posted by mactec54 Hi one of many Sorry I did miss the G32 But this is a wast of Z movement which could be as much as 15" from the part if the operator has just touched off the tool the Z will go to the tool change position & then have to come back down again another 15" a total of 30'' of movement that is not needed if you set the Z to your clearance plane, & is the first move the machine does you save all that extra Z movement that you have added by not having to go back up to the tool change position Ballscrews will last a lot longer to

Waste of Z movement........Huh?

This is our standard post processor header and good habits to prevent a crash; At the start of a program there should be a tool change call. At the end of a program the Z would normally be sent all up or to tool change. Then the program would move the y axis to the front in a production run every cycle of the program(which could be considered a waste of Y axis movement, but convenient for the operator).

I'll agree with hand written code, there is a lot more that can be done, but should it? I'd classify that as individual preference, not necessarily sound advice.

As I have stated, to each his own. Now with the added caveat...within in his level of safety, comfort and experience and/or procedural company policy. No mill was crashed or harmed in this exchange.....but the potential always remains high. Be on guard!

DC

[rmason]

First off -thanks to all who have responded. I added the additional g40/g41 commands in the hopes of fixing the problem. Bobcad entered the GO commands as well as the x/y moves. The header is also entered by me. Both (my original post and the edited version posted by "one of many" have the same issue -that is, the first 3 rectangles are fine, the 4th thru last all move approx. 8" while down (-.09) then G0 z.025 and move to next rectangle. Why it works fine for the first 3 then goes awry is the issue. I also appreciate the input regarding the proper protocol for when to enter the Z rapid - you guys are sharp!
As for the move on /off the work, I only need to remove approx. .010 from the edge of a laser cut pattern of this arrray. These openings are just a bit too small to fit the parts. I drew the part in bobcad then had the laser house cut the plate. I am using the same print (bobcad) and generated the code from the print. My idea was to use a .125 and open up the rec. till parts fit. adjusting the tool dia. (G41) till all is good. Sounded like an easy project. THe array actually has 95 rectangles so manually entering into cent control is too slow. So the problem remains -why is the control moving way out after doing the first three good? If any of have a cent 6 or later control maybe you could load it and see if you have same issue. Thanks R