by modified with the post, i mean using custom operation parameters. There isnt too too much thats overly crazy involved in doing the programming for such a thing

it appears to me as being more than likely programmed as a 5 axis multisurface operation (probably modified with a post) running a high speed option. I know for sure that it is not a mazak option.

heres another one, the disclaimer again. Do as you wish with what i give you, but use all of these at your own risk, not my fault, whatever happens, you may use different parameter sets, just dont mess them up, or blame it on me. this works on my specific mkIV integrex, it may not work on yours. but it works on my machine. it might work on other types of machines, but i make no guarantees (other than the parameters will mean nothing on other brands and controls) ps, make sure your parameters are set to allow the eia subprogram to draw its offset from the mazatrol or eia master program. oh yeah, and make sure youre using a spring loaded ball bearing centre. lol lol and another thing. DONT MOVE YOUR LOWER TURRET WHEN ITS ADVANCED. lol that ones a no brainer. Parameters i used: J5=9001 (macro program number) J6=741 (gcode call address) J7=1 (macrocall type) J8=0 (cant rememmber, but mines set to 0. check it if you wish) ps. use in conjunction with the G611 in the other thread to turn mill long slender parts. hehe) Macro: (cant remember if i finished the Head 2 logic.) O9001(G741 LOWER TURRET TAILSTOCK MACRO) (LOWER TURRET TAILSTOCK MACRO) (PROGRAMMED BY BRANDON WALKER) (NORQUEST INDUSTRIES) (MARCH 18 2009) (TEST CALL) (#2=1.) (#3=0.25) (#4=0.38) (#5=1.) (#6=10.) (=========) (VARIABLES) (=========) #580=#1 (ARGUMENT A - TOOL NUMBER OF CENTRE) #581=#2 (ARGUMENT B - HEAD SELECTION CODE) #582=#3 (ARGUMENT C - CENTERING SUPPORT COORDINATE IN Z) #583=#7 (ARGUMENT D - CENTRE HOLE DIAMETER) #584=#8 (ARGUMENT E - Z CLEARANCE) #585=#0 (DEPTH FOR CENTRE) #586=30. (CENTRE POINT ANGLE) #587=#0 (Z MOTION COORDINATE VARIABLE) #588=#9 (ARGUMENT F - FEEDRATE FOR APPROACH) #589=-1 (Z COORDINATE VARIABLE 2) #590=#4 (APPROACH/RETRACT FLAG - 1 = APPROACH - ELSE = RETRACT) #591=#0 (CLEARANCE FOR RETRACT) (===========) (MACRO START) (===========) G20 G80 G49 G40 (SAFETY START BLOCK) G98 (FEED PER MINUTE) G53.5 (MAZATROL COORDINATE SYSTEM) G109 L2 (SELECT LOWER TURRET) (======================) (TOOL STATION SELECTION) (======================) (MODIFY TO USE VARIABLES FOR POCKET NUMBER AT LATER DATE) IF [#590 EQ 1.] GOTO1 GOTO700 N1 IF [#581 EQ 1.] GOTO10 (SELECT TOOL 8 POSITION FOR HEAD 1) IF [#581 EQ 2.] GOTO20 (OTHERWISE SELECT POSITION 108 FOR HEAD 2) GOTO600 N10 M901 T007007.01 GOTO30 N20 M902 T107107.01 GOTO30 (============) (CALCULATIONS) (============) (CALCULATE CENTRE DEPTH PAST Z COORDINATE GIVEN) N30 #583=#583/2 (DIVIDE CENTRE HOLE DIAMETER IN HALF) #585=#583/TAN[#586] (CALCULATE CENTRE DEPTH) (======) (MOTION) (======) IF [#581 EQ 1.] GOTO100 IF [#581 EQ 2.] GOTO200 N100 #587=#582+#584+#585 #589=#587-#584 G0 Z#587 G0 X0. G0 Z#589 G1 Z#582 F#588 #588=#588/2 #585=#582-#585 G1 Z#585 F#588 GOTO999 N200 #587=#582-#584-#585 #589=#587+#584 G0 Z#587 G0 X0. G0 Z#589 G1 Z#582 F#588 #588=#588/2 #585=#582+#585 G1 Z#585 F#588 GOTO999 (======) (ALARMS) (======) N600 #3000=103 (INCORRECT_HEAD_SELECTION) (=======) (RETRACT) (=======) N700 IF [#581 EQ 1.] GOTO701 IF [#581 EQ 2.] GOTO702 N701 #591=#584 GOTO703 N702 #591=-[#584] GOTO703 N703 G0 Z#591 G28 U0. G28 W0. (===) (END) (===) N999 (EXIT) G99 (FEED PER REV) M99 (MACRO END)

Hi everyone, figured i would share my integrex turn milling macro for personal interest. here it comes. I am in NO WAY SHAPE OR FORM RESPONSIBLE WITH WHAT YOU DO WITH THIS CODE OR PARAMETERS!!! if you are in the habit of crashing and blaming it on some guy on the internet said... then turn away! lol Now here it is. NOTE: you will require the grindermode option and have the appropriate O parameters set for your machine. This macro works as a Gcode call. Works for straight turning cuts ( like turn milling astralloy with inconel overlay. lol). Theres some functionality i would like to add later, but this is it for now. these parameter sets are what i have used, you may use other custom Gcode parameter sets if these ones are used. Parameter settings: J13 = 9002 (this is the macro program number) J14 = 611 (this is the custom Gcode address) J15 = 1 (macro call type) J16 = 0 (cant remember, but check if you want) Macro program: (if the formatting shows up right) O9002(G611 TURN-MILLING MACRO) (TURN MILLING MACRO) (PROGRAMMED BY BRANDON WALKER) (NORQUEST INDUSTRIES) (MARCH 31 2009) (===============) (CLEAR VARIABLES) (===============) (ADD SECTION TO CLEAR ALL VARIABLES OF PREVIOUSLY STORED DATA) #101 = 595 WHILE [#101 LE 609] DO1 #[#101] = #0 #101=#101+1 END1 (=========) (VARIABLES) (=========) #595=#1 (ARGUMENT A - TURN MILLING TOOL NUMBER) #596=#2 (ARGUMENT B - MILL SPINDLE RPM) #597=#3 (ARGUMENT C - TURNING SPINDLE RPM) #598=#7 (ARGUMENT D - TOOL DIAMETER) #599=#8 (ARGUMENT E - HEAD SELECT) #600=#9 (ARGUMENT F - FEEDRATE) #601=#4 (ARGUMENT I - Z COORDINATE OF START) #602=#5 (ARGUMENT J - Z COORDINATE OF END) #603=#6 (ARGUMENT K - X AXIS START DIAMETER) #604=#12 (ARGUMENT L - X AXIS FINISH DIAMETER) #605=#13 (ARGUMENT M - DEPTH OF CUT) #606=#18 (ARGUMENT Q - CLEARANCE DISTANCE) #607=#602 (CURRENT X CUTTING DIAMETER) #608=201. (C AXIS ENABLE CODE) #609=4. (SPINDLE DIRECTION CODE) (=====================) (CHECK USER INPUT DATA) (=====================) IF [#595 EQ #0] GOTO802 IF [#596 EQ #0] GOTO803 IF [#597 EQ #0] GOTO804 IF [#598 EQ #0] GOTO805 IF [#599 EQ #0] GOTO806 IF [#600 EQ #0] GOTO807 IF [#601 EQ #0] GOTO808 IF [#602 EQ #0] GOTO809 IF [#603 EQ #0] GOTO810 IF [#604 EQ #0] GOTO811 IF [#605 EQ #0] GOTO812 IF [#606 EQ #0] GOTO813 (===========) (START MACRO) (===========) G20 G80 G00 G49 G40 (SAFETY START LINE) G53.5 (MAZATROL COORDINATE SYSTEM) G109 L1 (SELECT UPPER TURRET) T#595 M06 (CALL TURNMILLING TOOL) G99 (FEED PER MINUTE) G0 B90. (CALL B AXIS TO POSITION) #610=#610+#599 (SET HEAD SELECT M CODE) #608=#608+#599 (SET C AXIS MCODE) IF [#599 EQ 1.] GOTO60 (SET SPINDLE DIRECTION) IF [#599 EQ 2.] GOTO70 GOTO801 (IF DATA MISSING GOTO ALARMS) N60 (PREPARE FOR HEAD 1) #609=4. (SET SPINDLE DIRECTION REVERSE) GOTO90 N70 (PREPARE FOR HEAD 2) #598=-[#598] (REVERSE Y AXIS COORDINATE FOR HEAD 2) #601=-[#601] (REVERSE Z AXIS COORDINATE FOR HEAD 2) #609=3. (SET SPINDLE DIRECTION FORWARD) GOTO90 N80 IF [#607 EQ #604] GOTO900 (CHECK IF FINISHED LAST PASS ALREADY) #607=#604 (IF NOT TAKE LAST PASS) GOTO100 N90 M#610 (ENABLE SELECTED HEAD) M#608 (ENABLE C AXIS OF ENABLED HEAD) M610 (ENABLE GRINDER MODE) M611 S#596 M203 (START MILL SPINDLE) S#597 M#609 (START TURNING SPINDLE IN PROPER DIRECTION) N100 G0 Z-[#601] (RAPID TO Z AXIS CUT START POSITION) G0 X[#603+#606] (MOVE TO CLEARANCE POSITION IN X AXIS) G0 Y-[#598*2] (MOVE CLEAR IN Y - 2 X TOOL DIAMETER) G01 X#607 F[#600*2] (FEED TO CUTTING START DEPTH AT 2X FEED) G01 Y-[#598/4] F[#600/2] (FEED INTO PART Y AXIS 1/4 DIA BEHIND CENTRE) G01 Z-[#602] F#600 (FEED TO Z END POINT) G01 U0.1 F#600 (FEED OUT AXIALLY) G0 X[#603+#606] (RAPID TO INITIAL CLEARANCE) #607=#607-#605 (INCREMENT AXIAL POSITION OF NEXT CUT) IF [#607 LE #603] GOTO80 (CHECK IF LAST PASS) GOTO100 (======) (ALARMS) (======) N801 #3000 = 101 (INCORRECT*HEAD*SELECTION) N802 #3000 = 102 (MISSING*TOOL*NUMBER) N803 #3000 = 103 (MISSING*MILL*RPM) N804 #3000 = 104 (MISSING*TURNING*RPM) N805 #3000 = 105 (MISSING*TOOL*DIAMETER) N806 #3000 = 106 (MISSING*HEAD*SELECTION) N807 #3000 = 107 (MISSING*FEEDRATE) N808 #3000 = 108 (MISSING*Z*START) N809 #3000 = 109 (MISSING*Z*END) N810 #3000 = 110 (MISSING*X*START) N811 #3000 = 111 (MISSING*X*END) N812 #3000 = 112 (MISSING*DEPTH*OF*CUT) N813 #3000 = 113 (MISSING*AXIAL*CLEARANCE) (===============) (RETRACT AND END) (===============) N900 G28 U0. V0. (RETRACT X AND Y AXES) G28 W0. (RETRACT Z AXIS) M612 (GRINDER MODE CANCEL) M205 (STOP MILL SPINDLE) M99 (END MACRO)

Hi everyone, Weve been working on some compensation issues, and I know of a fair selection of other people who have this issue, so i figured i would post up some information on the matter to help out some others. On our mkIV Integrex (its a 400st but should be true to any MkIV), we had issues compensating in EIA, Since we normally run mazatrol with some EIA subprograms, it never mattered too much, the comp would work at B90, but on angles we had issues. So before I go any further, ill put this courtesy statement. If you are not qualified to be doing this. Dont! tell someone who is and maybe you can work on it from there. This is how I do it, but not necessarily how you should do it. anyways my parameters regarding this are set as follows F92 bit 7 set to 0 F93 bit 3 set to 1 F94 bit 2 set to 1 F94 bit 7 set to 0 F92 bit 7 and F94 bit 7 may be set to one, but mine arent currently set that way. If you wish to use mazatrol tool data, then set them to 1. For compensating properly on compound angles, i program our holes (circle mill) using compensation in Control. You must also output a G68.5 tilted work plane command. This greatly simplifies the code and it is output as it would be in G17 plane. We use G68.5 will all addresses to 0. but R is equal to the B axis angle. When cutter comp is activated (as per our parameter settings) the machine looks to the tool offset page, then to the nose R value of the selected tool (geometric requires the actual tool radius, and wear is the amount to shift). (obviously you must call Txx and Dxx somewhere before calling G41. Also G41 MUST be activated on linear motion. Alarm will result if activating on circular interpolation. if you wish to use mazatrol tool data, actual diameter you should be able to change the 2 parameters mentioned above and you can change the actual diameter to achieve compensation. Just figured i would mention it, as we had issues without the G68.5 (look in the misc values to activate it) because the cutter comp would change sides because our code was output with XYZ motions while interpolating angled holes. hope this information helps some integrex guys out there.

if you are working on an integrex (and not using the lower turret simultaneously), delete the section for the G109 L2 and leave the lower turret out completely, do not post any G950 and up codes, or P codes, they will all cause change to lower turret. make sure all tools are set (on mill turn in the tool edit page in mastercam) to upper turret and the selected head) also make sure your axis combinations are set to use the upper turret and selected head as well. also if for example you are working on head 2, search your code for G110. if you see G110 C2, your machine is selecting head 2 for its commanded c axis response. im not sure what you mean dropping TC planes out of the blue tho. Also if youre like me, you dont use any G50 shifts, so if you see like G50 #500 in your code, delete them, (since i use macros, there are values in these variables, and shifting the work plane by that amount could have disasterous consequences) i havent worked with X4s multiaxis toolpaths much yet though, so i cant help you much on the toolpathing side of things, but i can definetly help you with what the code is doing.

i second the lead lag comment, tilt a copy mill cutter (radius inserts)

look at ICAM CAMPOST. It will actually take your toolpath and make decisions while it posts, (along with full machine simulation), it will show you where it hits limits, and if you choose it will make decisions to change the posted output to fit within the machine limits (if it has a means of doing so, ie tilting and rotating.) Id say it puts vericut to shame. hope youre made of money though lol but either way, give them a call (even if you have no interest in buying.), its worth a look to see whats out there. trust me you wont be sorry you did.

ill have to check this out myself. Ive only used the FBM drill once so far, and I found that even setting it to sort a few differnt ways it jumped around a lot. Not to mention it took like 3 hours to calculate. My part was round though with hundreds of different toolplanes. i had to go and manually arrange the toolpaths how i wanted them lol

if that doesnt work, sometimes theres an actual shutoff valve behind the cover. if you go into the back of the machine youll see it there on the back of the Z axis cover. (theyre not all like that though)

I have this problem from time to time, try it in another format, i use IGES sometimes if i have to. Sometimes if the surfaces come out funny, Ill make some edge geometry and patch it up, but it depends on how good you are at surface modelling. Its quite a PITA sometimes, and some people are better at it than others.

router posts were the worst for me. I hated them, especially block drilling.

I dont feel that you didnt call me on anything. I made a point of how to do what was asked. im not here to babysit how people do things, its up to the programmer and operator to make sure they dont slam their machine. I just showed EXACTLY what was asked. I didnt realize i had to provide step by step what had to be done, and what to watch for. you basically told me that it wouldnt do rotary properly. I called you on it. i proved that it would. Thats all. and honestly if some kid came on here and said wow cool, and tried it and it didnt work. the barrier would kick in and stop a collision. (because these are mazaks). if they dont he didnt set it up right and he SHOULDNT be running, let alone programming, a multitasking machine. The big blue circles show an erroneous collision that doesnt actually occur. I showed a way do do so without having the misleading verification. Furthermore, I know Randy, and I know his machine. He works right down the street from me, I even saw his machine trucked in and unloaded at his shop because his shop bought it from us when I was back when i was installing mazaks and training people on them. Im quite aware of his capabilities, and I simply showed him, the person who asked the question, how to do what he asked. and i backed myself up all the way along. i did nothing wrong, and nothing irresponsible. period. also about the head being in the way. well regardless of what the mastercam verify shows you, it will never be there anyways, you would need full machine simulation for that, and just so you know, mazaks have this to begin with, mastercam will do nothing to show that either way, so that is irrelevant. And if because youre verifying by NCI and it wont be guaranteed not to slam the machine, you could say that about anything mastercam does in general. The only way to guarantee it is to verify the Gcode, thats not something mastercam does anyways. look to vericut, ICAM, mazatrol simulation, etc for that one. and also, most of the time, the machine will retract before any sort of unwind, that depends on post, programming etc. that has nothign to do with what ive shown. I get the feeling you were proven wrong, and you are backtracking. but hey no one holds grudges. And i apologize if you felt i was attacking your knowledge, I wasnt trying to do so. I just love to have a good debate. lol Thats how we learn to push ourselves. Ill also take this opportunity to mention, this is just business. lol nothing personal, not trying to start a fight or any grudges either. lol [ 08-27-2009, 01:58 AM: Message edited by: Bwalker ]

http://www.mastercam.com/Support/Downloads...X4/Default.aspx

certain toolpaths dont make full motions, helical boring and circle milling are two examples of this. There are softwares that will show this type of thing however. The backplot should show the same toolpath moving around its helix or circular interpolation though. Kinda off topic: If you want really detailed verification, ICAM and Vericut are good exaples. expensive, but ICAM was probably the most impressive piece of cnc software ive seen to date. ICAM with material removal will show you the chips coming off the part in the verify. its very cool stuff. it really shines in multiaxis posting, the way it will modify the toolpath in the posting process to avoid collisions or overtravels.