Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Okuma lathe guys, wait code issues.


DODGERFAN
 Share

Recommended Posts

We have had an LU 15 in here for years and we only use the top turret.  The boss man wants me to

start using the lower turret on it.  I have a post that works, but it doesn't put the "P" codes in the right places and on the lower turret, all of the X values are X minus.   I don't know if they are supposed to be negative or not.   So my question is:  Does anybody have a sample program for me to look at? 

 

Thanks guys.

Link to comment
Share on other sites

Bottom turret uses the same x values as a top turret, so X+ is away from the centerline. As for wait codes, I have to put them in by using manual entry. The post I have wants to put wait command at every damn toolchange but they're only necessary when when you need to time the turrets. Do you want a sample text program, or a sample Mastercam program?

  • Like 1
Link to comment
Share on other sites

Bottom turret uses the same x values as a top turret, so X+ is away from the centerline. As for wait codes, I have to put them in by using manual entry. The post I have wants to put wait command at every damn toolchange but they're only necessary when when you need to time the turrets. Do you want a sample text program, or a sample Mastercam program?

Thanks,   I so wasn't sure about the -X values.    Just the text would be helpful.   My Mastercam program I believe is correct.   (looks right in backplot)  LOL.

Thanks again.

Link to comment
Share on other sites

Here's something simple I just whipped up real quick. Only the drill is in the bottom turret, I highlighted the wait codes for you. I've got some much more complex stuff if you want to see that.

 

 

( PROGRAM   -  DEFAULT .min )
( DATE      - 10 /24 /2014 )
( REVISION     - )
( CYCLE TIME   - )

G13
N0002 G140 P0010
G123
G00 X20. Z32.
G50 S913
CALL OTOPM XDIA=3.832 LNGT=1.5354 FACE=.01 SSPD=1200 FDRT=.003

N2 (OD 431 MAIN)
G97 S490 M03
G95
G00 Z0. T020202
X4.2945
G96 S525
G01 G41 X4.0945 F.015
X0.
G40 X0. Z.1
G00 Z.2
X20.
Z32.
T0200

N4 (1/2 CENTER DRILL)
G97 S601 M03
G94
G00 Z.25 T040404
X0.
Z.1
G01 Z-.2 F5.42
G00 Z.25
X20.
Z32.
T0400

N4 (.062 PENTACUT SQUARE)
P100
P200

G97 S523 M03
G95
G00 Z-1.2727 T040404
X3.9734
G96 S525
G01 X3.832 Z-1.3434 F.015
G03 X3.324 Z-1.5975 L.254
G01 X3.524 Z-1.5974
G00 X3.896
X20.
Z32.
T0400

N152 (OD CUTOFF LEFT)
G97 S295 M03
G95
G00 Z-1.5354 T1535352
X3.896
G96 S288
X3.732
G01 X3.532 F.0015
X-.032
X.168
G00 X3.532
X3.896
M05
X20.
Z32.
T15200

( PROGRAM   -  DEFAULT .min )
( DATE      - 10 /24 /2014 )
( REVISION     - )
( CYCLE TIME   - )

G14
G140
X20.
Z32.

N110 (NO.2 DRILL)
P100
G97 S1361 M03
G94
G00 Z.25 T1111110
X0.
Z.1
G01 Z-1. F5.39
G00 Z.25
X20.
Z32.
T11000
P200

N9999 M02
 

  • Like 1
Link to comment
Share on other sites

Ray I made a post for that machine years ago. I have all of that dialed in for that machine. Might need to be updated from X4 to the version you are running, but all of the wait code stuff is worked out using the mi and mr values in the misc. The G13 and G14 is also sorted out in the post. I should have some old pinch turning programs I did years ago you can look at. Some of the long shafts we did and other little things. Machine still have that .002 dip near the chuck?

  • Like 1
Link to comment
Share on other sites

Ray I made a post for that machine years ago. I have all of that dialed in for that machine. Might need to be updated from X4 to the version you are running, but all of the wait code stuff is worked out using the mi and mr values in the misc. The G13 and G14 is also sorted out in the post. I should have some old pinch turning programs I did years ago you can look at. Some of the long shafts we did and other little things. Machine still have that .002 dip near the chuck?

I think you only made one program for that machine Ron.  I tried to find it but I had no luck.  

As far as that little dip,   I just started using a second offset to cancel that out.   works perdy good.

I like the machine, just never had the time to figure out programming the second turret.

Link to comment
Share on other sites

Ron, this is from your post. 

 

 

(TEST)
G13
(UPPER TURRET)
(MACHINE      - OKUMA LU-15)
(CUSTOMER     - ADD CUSTOMER)
(PART #       - Machine Group-1)
(MODEL #      - Machine Group-1.MCX)
(PROGRAMMER   - RAY B)
(PROGRAM NAME - LUTEST3.MIN)
(DATE         - OCT. 24 2014)
(TIME         - 8:11 AM)
(PROGRAM REV  - N/C)
(TOOL - 1   - INSERT - CNMG-432 - HOLDER - DCGNR-164D)
(TOOL - 3   - INSERT - NONE - HOLDER - NONE)
(TOOL - 2   - INSERT - VNMG-431 - HOLDER - MVJNR-164D)
G14
(LOWER TURRET)
(TOOL - 1 OFFSET - 1)
(OD ROUGH RIGHT - 80 DEG. INSERT - CNMG-432)
N100 G0 X20. Z20. N100 P10
N110 T0101
N120 G18 G95
P20 N130
N140 G50 S2000
N150 G97 S179 M03
N160 G96 S325 G111
N170 G0 X6.95 Z9.7883 M8
N180 G1 Z9.6883 F.012
N190 X4.3425
N200 X4.4839 Z9.759
N210 G0 X6.95
N220 Z9.6917
N230 G1 Z9.5917
N240 X4.3425
N250 X4.4839 Z9.6624
N260 G0 X6.95
N270 Z9.595
N280 G1 Z9.495
N290 X6.7395
N300 X4.3402
N310 X4.4817 Z9.5657
N320 M9
N330 G0 X20. Z20. N330 P30
M05
N340 M01
(TOOL - 1 OFFSET - 1)
(OD ROUGH RIGHT - 80 DEG. INSERT - CNMG-432)
N350 G0 X20. Z20. N350 P40
N360 T0101
N370 G18 G95
P50 N380
N390 G50 S2000
N400 G97 S188 M03
N410 G96 S325 G111
N420 G0 X6.6091 Z9.6985 M8
N430 G1 X6.6438 Z9.6 F.015
N440 Z4.3843
N450 X6.7443 Z4.3341
N460 X6.8857 Z4.4048
N470 G0 Z9.6985
N480 X6.5087
N490 G1 X6.5434 Z9.6
N500 Z4.4346
N510 X6.6638 Z4.3743
N520 X6.8053 Z4.4451
N530 G0 Z9.6985
N540 X6.4082
N550 G1 X6.4429 Z9.6
N560 Z9.449
N570 G3 X6.445 Z9.4388 I-.0502 K-.0102
N580 G1 Z4.4838
N590 X6.5634 Z4.4246
N600 X6.7048 Z4.4953
N610 G0 Z9.6985
N620 X6.3078
N630 G1 X6.3425 Z9.6
N640 Z9.49
N650 G3 X6.445 Z9.4388 K-.0512
N660 G1 Z4.4838
N670 X6.4629 Z4.4748
N680 X6.6044 Z4.5455
N690 M9
N700 G0 X20. Z20. N700 P60
M05
N710 M01
G13
(UPPER TURRET)
(TOOL - 3 OFFSET - 3)
(ID ROUGH MIN. 1.0 DIA. - 75 DEG. INSERT - )
N720 G0 X20. Z20. N720 P70
N730 T0303
N740 G18 G95
N750 G50 S2000
N760 G97 S249 M03
N770 G96 S300 G110
N780 G0 X4.6072 Z9.6707 M8
N790 G1 X4.4657 Z9.6 F.015
N800 Z4.2539
N810 X4.3758 Z4.2089
N820 X4.2344 Z4.2796
N830 G0 Z9.6707
N840 X4.6971
N850 G1 X4.5557 Z9.6
N860 Z4.2989
N870 X4.4457 Z4.2439
N880 X4.3043 Z4.3146
N890 G0 Z9.6707
N900 X4.7871
N910 G1 X4.6457 Z9.6
N920 Z4.3438
N930 X4.5357 Z4.2889
N940 X4.3943 Z4.3596
N950 G0 Z9.6707
N960 X4.877
N970 G1 X4.7356 Z9.6
N980 Z4.3888
N990 X4.6257 Z4.3338
N1000 X4.4842 Z4.4046
N1010 G0 Z9.6707
N1020 X4.967
N1030 G1 X4.8256 Z9.6
N1040 Z4.4338
N1050 X4.7156 Z4.3788
N1060 X4.5742 Z4.4495
N1070 G0 Z9.6707
N1080 X5.0569
N1090 G1 X4.9155 Z9.6
N1100 Z4.4788
N1110 X4.8056 Z4.4238
N1120 X4.6641 Z4.4945
N1130 G0 Z9.6707
N1140 X5.1469
N1150 G1 X5.0055 Z9.6
N1160 Z9.4887
N1170 G2 X4.9255 Z9.4388 I.0112 K-.05
N1180 G1 Z4.4838
N1190 X4.8955 Z4.4688
N1200 X4.7541 Z4.5395
N1210 G0 Z9.6707
N1220 X5.2369
N1230 G1 X5.0954 Z9.6
N1240 Z9.491
N1250 X5.0367 Z9.49
N1260 X5.028
N1270 G2 X4.9855 Z9.4854 K-.0512
N1280 G1 X4.8441 Z9.5561
N1290 M9
N1300 G0 X20. Z20. N1300 P80
M05
N1310 M01
G14
(LOWER TURRET)
(TOOL - 2 OFFSET - 2)
(OD FINISH RIGHT - 35 DEG. INSERT - VNMG-431)
N1320 G0 X20. Z20. N1320 P90
N1330 T0202
N1340 G18 G95
P100 N1350
N1360 G50 S2000
N1370 G97 S242 M03
N1380 G96 S300 G111
N1390 G0 X4.732 Z9.585 M8
N1400 G1 Z9.485 F.005
N1410 X6.3737
N1420 G3 X6.435 Z9.4543 K-.0306
N1430 G1 Z4.4908
N1440 X6.7351 Z4.3408
N1450 X6.8765 Z4.4115
N1460 M9
N1470 G0 X20. Z20. N1470 P110
M05
N1480 M01
G13
(UPPER TURRET)
(TOOL - 3 OFFSET - 3)
(ID ROUGH MIN. 1.0 DIA. - 75 DEG. INSERT - NONE)
N1490 G0 X20. Z20. N1490 P120
N1500 T0303
N1510 G18 G95
P130 N1520
N1530 G50 S2000
N1540 G97 S225 M03
N1550 G96 S300 G110
N1560 G0 X5.0958 Z9.586 M8
N1570 G1 Z9.486 F.005
N1580 X5.0369 Z9.485
N1590 X5.028
N1600 G2 X4.9355 Z9.4388 K-.0462
N1610 G1 Z4.4817
N1620 X4.3941 Z4.211
N1630 X4.2527 Z4.2817
N1640 G0 Z9.515
N1650 M9
N1660 G0 X20. Z20. N1660 P140
N1670 M05
N1680 M02
%
 

Link to comment
Share on other sites

Look in the mi and mr and put the values in there. Have to use the toolpath editor in roughing operations to make it a complete pinch turning program. Remember to offset the process when doing the programming. Example would be take double the normal depth of cuts in the upper turret. Then take the same amount of of cuts, but start 1/2 of the 1st cut in on the lower turret. Then what I did was using the toolpath editor using cantext 20 was pick where I wanted the output to be to wait code the operations form upper to lower turret. I normally dd it at the retract of the cut and the rapid to of each cut to keep everything as balanced on the cutting as I could. Yes the backplot will not be real. Yes the Verify will not be real. Yes you have to pray to everything you know you got it all figured out, but I could make a program and post it and felt pretty good going out to the machine to run it. The Shafts with Splines inside were also done on that machine. All the turning and broaching was been doing on that machine along with a few other parts we messed around with years ago.

 

If you you not put anything into the mi or mr you would not get wait codes so what you posted is normal output. To get wait codes if memory serves me correct needed to put values in the operation to get the wait codes to be output. Could always contact ICAM and they can whip you up a post and simulation for that machine. :laughing:

Link to comment
Share on other sites

Here is some sample code from a part that I worked on years ago. I was doing a time study on pinch turning with increased feed versus staggering the tools with a heavier depth of cut. The pcodes in this sample were manually edited by myself while setting up the machine, so they may or may not be the 100% correct way to do it. But it did run and did what I wanted it to do.

HTH

$SAMPLE.MIN
G13
N1
( *** )
( ***** TURRET A ***** )
( ROUGH FACE AND TURN  )
( RH ROUGH TURN    INSERT -  1/32 TNR )
G50 S1200
G0 M8
X50. Z50.
T0101 M42 P09
G96 S650 M3 P10
G0 X3.35 Z.01
G1 X-.0625 F.01
G0 Z.05
X3.3 P20
G85 NLAP1 D.4 U.04 W.005 F.016 P21
NLAP1 G81
G0 X1.3021 Z.05 P22
G1 Z-.0162 P23
X1.3768 Z-.0535
G3 X1.398 Z-.0792 I-.0257 K-.0257
G1 Z-1.7987
X1.759 Z-1.9792
G3 X1.789 Z-2.0154 I-.0362 K-.0363
G1 Z-4.3625
Z-5.7123
G2 X1.8865 Z-5.761 I.0488
G1 X2.7365
G3 X2.8001 Z-5.7798 K-.0362
G1 X2.8431 Z-5.8014
X3.15
G80
G0 X50. Z50. P25
T0202
M1 P40
 
G14
N2
( ***** TURRET B ***** )
( ROUGH FACE AND TURN  )
( RH ROUGH TURN    INSERT -  1/32 TNR )
G50 S1200
G0 M8
X50. Z50.
T0202 M42 P09
G96 S650 M3 P10
G0 Z.150
X3.1 P20
G85 NLAP1 D.4 U.04 W.005 F.016 P21
NLAP1 G81
G0 X1.3021 Z.15 P22
G1 Z-.0162 P23
X1.3768 Z-.0535
G3 X1.398 Z-.0792 I-.0257 K-.0257
G1 Z-1.7987
X1.759 Z-1.9792
G3 X1.789 Z-2.0154 I-.0362 K-.0363
G1 Z-4.3625
Z-5.7123
G2 X1.8865 Z-5.761 I.0488
G1 X2.7365
G3 X2.8001 Z-5.7798 K-.0362
G1 X2.8431 Z-5.8014
X3.15
G80
G0 X50. Z50. P25
T0303
M1 P40
Link to comment
Share on other sites
  • 3 years later...

Im just trying to find the meaning behind the G110 and G111 and when they're necessary and when they are not.. I think you guys were referring to them as timing codes or something between the two turrets maybe? So are they only necessary when running the two turrets simultaneously? My mastercam posts all my programs with the G110 when only using Turret A and now Im trying to learn how to use Turret B and don't know what i need to make it run.. G111?.. Neither?.. Both?.. I dont know lol Any advise would be greatly appreciated. Also, brand new to the forum (or any forum ^_^) so show me some love. Thanks guys!

Link to comment
Share on other sites
24 minutes ago, MachineMuch? said:

Im just trying to find the meaning behind the G110 and G111 and when they're necessary and when they are not.. I think you guys were referring to them as timing codes or something between the two turrets maybe? So are they only necessary when running the two turrets simultaneously? My mastercam posts all my programs with the G110 when only using Turret A and now Im trying to learn how to use Turret B and don't know what i need to make it run.. G111?.. Neither?.. Both?.. I dont know lol Any advise would be greatly appreciated. Also, brand new to the forum (or any forum ^_^) so show me some love. Thanks guys!

G110 and G111 have to do with CSS speed control for the spindle. G110 puts turret A position in control of CSS. G111 puts turret B in control.

Link to comment
Share on other sites
  • 2 years later...

I have a similar situation i was wondering how you post with masterCAM and program with TWO turrets at the same time. those programs are good but how do you actually program ? can you someone post instructions please? is it a different POST that buy?

Link to comment
Share on other sites
14 minutes ago, 88WP said:

I have a similar situation i was wondering how you post with masterCAM and program with TWO turrets at the same time. those programs are good but how do you actually program ? can you someone post instructions please? is it a different POST that buy?

If you want to be able to program and sync in Mastercam you need to have the MT module and the appropriate machine def/post for your machine. I have used the Okuma Multus U3000 MT machine def/post for Mastercam and it does a decent job at handling wait codes. 

  • Like 1
Link to comment
Share on other sites
15 hours ago, 88WP said:

I have a similar situation i was wondering how you post with masterCAM and program with TWO turrets at the same time. those programs are good but how do you actually program ? can you someone post instructions please? is it a different POST that buy?

Well you can program in Standard Mastercam using the method I developed and shared on the forum around 2005-2007. Since then Post developers have done good things to add sync code output in the operations using misc integers and reals. Nothing to the level I was doing with Cantext where I was able to do Pinch Turning and control it down to the rapid points in the outputted code using Tool Path Editor. My way was not an easy button method. 

MT has added this ability to Mastercam and when you go into Code Meter you can add your SYNC code. In the MT you grab your Upper and Lower Stream you want for Pinch turning and it sync them and the carries that over to Code Expert and that is done for you. I believe the OSP control has improved the Pinch Turning codes as well to make it a lot easier. You should get ahold of your local Mastercam Dealer and let them walk you through the different options and go from there. 

Link to comment
Share on other sites
18 hours ago, 88WP said:

I have a similar situation i was wondering how you post with masterCAM and program with TWO turrets at the same time.

Generally the people using MP posts for multi turret machines have many years hands on programming AND running these machines.

They are able to completely mentally  visualize the sequences and can put the wait codes in the appropriate places. And it is not always intuitively obvious...there just is no substitute for experience here.

The MT module provides a GUI solution which allows you to virtually crash the machine, then apply "linking" which controls the turrets in the virtual verify which in turn co-ordinates the posting of wait codes. This is of great value to people with less extensive "sharp end' multi turret lathe experience.

There is of course no free lunch and there are downsides to the MT module in terms of control of the machine environment.

Link to comment
Share on other sites
29 minutes ago, nickbe10 said:

Generally the people using MP posts for multi turret machines have many years hands on programming AND running these machines.

They are able to completely mentally  visualize the sequences and can put the wait codes in the appropriate places. And it is not always intuitively obvious...there just is no substitute for experience here.

I had a customer earlier this year disagree with that mind set. Brand new machine and new programmer that was a mill guy. 4 crashes and 3 months later they realized experience does mean something and you do need to take your time and do it right the first time.

Two ways to prove out a program. At the machine or in a CAV environment. At the machine is rolling the dice, but I still say is the best way. CAV is really great for getting it 95% there, but that last 5% should really be done at the machine with someone with years of experience. Looking at every possible way to improve the process when that matters. One off parts who care CAV it and call it a day, but anything where time and speed are important then CAV to get it running then finish it off in front of the machine.

I was proving out one part years ago that was down at 3 minutes 30 seconds to start. I was given 5 minutes as a goal. I was down to 3 minutes 10 seconds and they told me to quit. I felt I could get another 8 seconds out of the parts. They were concerned the operators wouldn't be able to handle all the movement without stressing them out I was doing with the 3 Turrets and asked me to slow it back down to 4 minutes 10 seconds. They were running 20k pieces a year and I tried to explain to them the ROI on the time savings, but their Union guys were already very upset at the time reductions and I was told to slow it down. 

  • Like 1
Link to comment
Share on other sites
1 hour ago, crazy^millman said:

4 crashes and 3 months later they realized experience does mean something and you do need to take your time and do it right the first time.

I don't even hesitate to run 4 axis verticals or horizontals (including multiaxis) without CAV, simply because I spent so many years running these machines I have no problem visualizing what is going on.

Once I move up to 5 axis I really prefer to work with CAV, just because the code can be somewhat arcane and the possibilities of crashes are much more likely with so much movement.

Same with lathes, single turret live tooling, 4 axis no problem, I just don't have enough , well any, hands on multi turret experience so I defer to our lathe experts for those machines.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...