584,808 active members*
5,242 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Milltronics > machine moves WAY off part before next move
Page 1 of 2 12
Results 1 to 20 of 24
  1. #1
    Join Date
    Mar 2008
    Posts
    15

    machine moves WAY off part before next move

    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

  2. #2
    Join Date
    Mar 2003
    Posts
    4826
    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.
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  3. #3
    Join Date
    Aug 2005
    Posts
    1622
    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

  4. #4
    Join Date
    Nov 2006
    Posts
    114
    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...?

  5. #5
    Join Date
    Mar 2003
    Posts
    4826
    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.
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  6. #6
    Join Date
    Jan 2005
    Posts
    15362
    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
    Mactec54

  7. #7
    Join Date
    Aug 2005
    Posts
    1622
    Quote Originally Posted by mactec54 View Post
    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

  8. #8
    Join Date
    Jan 2005
    Posts
    15362
    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
    Mactec54

  9. #9
    Join Date
    Aug 2005
    Posts
    1622
    Quote Originally Posted by mactec54 View Post
    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

  10. #10
    Join Date
    Jan 2005
    Posts
    15362
    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
    Mactec54

  11. #11
    Join Date
    Aug 2005
    Posts
    1622
    Quote Originally Posted by mactec54 View Post
    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

  12. #12
    Join Date
    Mar 2008
    Posts
    15

    thanks gentlmen

    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

  13. #13
    Join Date
    Mar 2003
    Posts
    4826
    I wonder what the syntax is for your control to turn on radius comp without calling a particular address from the comp register. Standard format would require a "D" address call, but perhaps your control implements this directly from the T number? Worth a look.
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  14. #14
    Join Date
    Aug 2005
    Posts
    1622
    Quote Originally Posted by rmason View Post
    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
    Other than my haste in cut and paste without grabbing the spindle startup line N**S800M3, it ran flawless on a Cent 7. I'd need more time to try it on a Cent 1 or 5, as we don't have any Cent 6 machines.

    Makes me wonder if this could be a parameter issue? Very Strange in deed!

    DC

  15. #15
    Join Date
    Aug 2005
    Posts
    1622
    Quote Originally Posted by HuFlungDung View Post
    I wonder what the syntax is for your control to turn on radius comp without calling a particular address from the comp register. Standard format would require a "D" address call, but perhaps your control implements this directly from the T number? Worth a look.
    Here is a sample out of another tooling program I use that shows comp syntax.

    N30G17G20G32G40G80
    N35T1M06
    (OPERATION: 1)
    (TOOL 1: 0.5 DIA.)
    N50S800M3
    N55G90G54G0X3.459Y-0.831
    N60G43Z0.3H1D1M7

    DC

  16. #16
    Join Date
    Nov 2006
    Posts
    114
    I'm sorry to say that I no longer have access to the Milltronics machines I ran last year but, I do recall that any program I ran on the Cent5 I could run on the Cent6 and visa versa.
    Hu, as I recall when you program a pocket of corse it just starts in the middle and works its way out and, when you call for a frame, either inside or out depending on left or right comp and cw or ccw direction, it would start in the middle of the longest side and just to the outside of the part by, I think, 2 X the tool Rad and arc in , cut the part and arc out at the same point leaving a nice little circle pocket at the side of the part.
    I used to carve 100 small electronic enclosures from a single sheet of .25 Mic 6 by simply programing the first one then looping the part in the x 9 times then looping the first set of loops 9 times in the y. If you have different sizes you might have to program them into your first row seperatly and then be creative with your looping but...
    The only time I ever used the cam was to generate a tool path for compressor wheel vanes or, an eliptical path.
    We had ProCam and Solid Works but the way things were set up it was faster to program at the controle for most of the stuff we did and the complex stuff was already programed and proven so it was not edited except by some change from the customer.
    As you might gather I'm a big fan of the operator/machinist /programer ... fully knowing their machine and its capabilities and not relying on off line programing, less of a chance for the guy on the floor to be hog tied to a problem with a program they did not wright or a machine they don't normaly operate... just my opinion guys, don't take my head off.

  17. #17
    Join Date
    Mar 2008
    Posts
    15
    I beleive this is some how a machine parameter error. I get the same error on both of my milltronics and have sent the program to milltroinics support for review
    i will post up any info. as it comes available.

  18. #18
    Join Date
    Aug 2005
    Posts
    1622
    Quote Originally Posted by rmason View Post
    I beleive this is some how a machine parameter error. I get the same error on both of my milltronics and have sent the program to milltroinics support for review
    i will post up any info. as it comes available.
    The only one I can think of is in the basic machine info "Max corner deviation" ours is set to .002. Other than that, maybe;

    "look ahead in run mode" set to YES
    "90 deg cutter comp" set to NO

    These are from a Cent 7, so they may not be included in the Cent 6 parameters.

    DC

  19. #19
    Join Date
    Mar 2008
    Posts
    15
    Here is the reply from milltronics -looks like I was on the right track- any thoughts /comments are appreciated

    The problem lies with the way cutter comp works. If you look in the Milltronics programming manual for G41, it will describe and show you how it works. The problem that you are having can be avoided by turning cutter comp off after each rectangle and then turning it back on. I hope this helps you. Please let me know if you have any other questions. Thank you

  20. #20
    Join Date
    Mar 2003
    Posts
    4826
    Your problem is that your program does not utilize the commands correctly. As I pointed out earlier, you cannot just throw in comp on and comp off commands willy nilly and expect the machine to work properly.

    First: you need a D value to call a comp value for the applicable tool, from your machine radius comp register. This is not present in your original program. So basically, you were running without any tool compensation at all.

    Second: you need to provide a lead on and a lead off of each profile. Your program lacks this, so each time the tool descends on the finish profile, cc turns on, a gouge will result at least equal to your tool radius, whatever amount you actually call from the relevant comp register.

    Cutter comp should be turned on after the tool has descended to cutting depth: not as the tool descends to depth but afterwards. Turning comp on with a Z movement is not a preparatory movement, and does not substitute for a lead in movement in X and or Y.

    The same rule applies at the end of each profile. You must cancel the cutter comp with a G40 in combination with a G01 feed movement to a safe position in X and/or Y. Then you can retract in Z and move to the next position. Your commands which turn comp off during the Z retract move are non-sense to the control.

    I've attached a file, based on a backplot of your original program. This is suitable for running on Haas machines, so I am not sure how that compares with your controller requirements. Anyways, the syntax within this program bears a look, as it is legal syntax of all programming elements which I have described. OneCNC makes it easy to add cutter lead in and also overlap on the profile which eliminates any little blip caused by the tool coming off the profile at high feedrates.

    I made the assumption that the tool is cutting inside the rectangles. If you want it the other way, that can be arranged
    Attached Files Attached Files
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

Page 1 of 2 12

Similar Threads

  1. Move machine zero
    By arendal in forum Calibration / Measurement
    Replies: 1
    Last Post: 04-30-2008, 03:14 PM
  2. HOW TO MOVE A MACHINE
    By DONNYBRASS in forum Uncategorised MetalWorking Machines
    Replies: 7
    Last Post: 11-17-2007, 01:56 AM
  3. Simple (dumb?) question . . .Machine move
    By brgrii in forum Uncategorised MetalWorking Machines
    Replies: 3
    Last Post: 04-17-2007, 09:51 PM
  4. Move part origin
    By vertcnc in forum Solidworks
    Replies: 1
    Last Post: 11-06-2005, 09:15 PM
  5. Move part
    By Thungvilai in forum GibbsCAM
    Replies: 1
    Last Post: 10-23-2003, 06:09 AM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •