check out www. mazatrolonline .com
this is your solution.
I've recently been hired to work in a manufacturing facility, and am operating a Mazak VCN 510C-II. I was hired based on my previous (non CNC) machining and shop experience, and told I would be trained on the Mazak. It was intimidating, because the only CNC machines I've run are a benchtop 3 axis mill I own, and a CNC grinder I built which operated from the computer/controller that came with the mill (Microkinetics).
My training has consisted of being told the basics while I hurriedly wrote down notes, plus the daily operation of the machine. Someone else has done the set ups and loaded the programs, I merely load and unload parts and run the machining cycles.
I'm sure I'm capable of running this and similar machines, but am in need of advice and education. Primarily, I would like to take an online class or classes specifically aimed at running the Mazak. In fact, I feel that my keeping this job depends on my getting training beyond what I'm recieving at work, as machine time and the availability of instruction seems limited.
If courses of study aren't available, are there any resources on the internet where I can look up methods on how to set up and run this machine?
check out www. mazatrolonline .com
this is your solution.
I wrote this as a supplement in American english to Mazak program training materials. Hope it helps.
Mazatrol M Programming Concepts – a supplement in plain English for the rigorously detailed MAZAK Programming Manuals. (Like most factory programming manuals from any builder – great reference for the power user, but poor for a beginner)
Mazatrol is FIXED FORMAT PROGRAMMING. (EIA is the exact opposite, you can write anything anywhere be it correct or not)
First Unit in a new program is the COMMON UNIT. - it establishes material - for auto calc of feed, speed, D.O.C., based on CUTTING CONDITIONS TABLES, elsewhere in the control.
KEY CONCEPT - leftmost key at the monitor is DISPLAY - this always gets you to the main portions of Mazatrol. Rightmost is MENU - this will display further pages of the current WINDOW DISPLAY. All keys between these two are SOFTKEYS - the meaning of the key changes as displays change.
PROGRAM - there are actually TWO DISPLAYS - program display and program editor. Display lets you see the program, but not EDIT it. You know you are in the editor when the cursor can move throughout the entire program. Cursor position is CRITICAL! This is controlled by the arrow keys.
When the cursor is on the first line of a UNIT, you hit menu and get to the editing softkeys (can't get there if not in editor) Lots of cool stuff you can do here, but the most important for a beginner is the HELP s/k (softkey) Only if the cursor is on the first line, you can get a HELP SCREEN that's a CHEAT SHEET/DIAGRAM for the info your particular unit requires. It's not available for a few units - common unit, end unit, manual unit, mms unit etc.
The DIALOG BOX is in the lower right corner of the display. This gives you more info on the info needed at the cursor position than the column headings in the program. MOST USERS ONLY LOOK AT THE CURSOR in the body of the program. Instead, also look at the dialog box - it offers a better description of the info you need at that point!
KEY CONCEPT - A WPC UNIT should always be the FIRST UNIT after common unit - this is EXACTLY LIKE a EIA G54-G59 in EIA, EXCEPT, you can also have a "theta" number to rotate the program way you want. It is always 0, which is needed instead of null, no number at all.
KEY CONCEPT - there can be multiple WPC's in the body of the program. It works as a modal, last one read is the current valid one. The number you can put with it is MEANINGLESS. It's just a label there to help you organize as you see fit. A WPC can also “point” to the external EIA FIXTURE OFFSET REGISTERS, G54-G59 and optionally, G54.1P1 to P128, or more, depending on s/w options. There are also EXTERNAL WPC REGISTERS! There are WPC – A through WPC –H under the s/k “additional”. Therefore, the WPC Unit in your program may not contain numbers, but instead point to an external (or “global”) WPC’s. These would be a convenience when dealing with a fixture and set up that does not change. If it’s fixed to the machine, why bother indicating it in again and again?
KEY CONCEPT - Mazatrol has a lot of cool TEACH functions - to eliminate doing math at the machine. Including WPC input. It is an arcane procedure that's easy if you know it and impossible if you don't. (Lots of that kind of stuff in mazatrol!)
Step 1 - cursor to common unit.
get OUT OF the editor
This should dislay a WPC SEARCH s/k, turn the s/k switch on, hit input, and that should get the cursor to the X WPC and reveal a TEACH softkey. There are 3 settings for parameter L56, which determines how the TEACH works for WPC. I recommend setting 2, which means "what is the coordinate value of this axis with respect to PART PROGRAM ZERO? This is the EIA WAY. You can also set it to TEACH "where is program zero from my tool point?" this is setting 0, which sucks.
X and Y are easy concepts - Z maybe not so much, for the following reasons;
KEY CONCEPT - Mazatrol uses TOOL SET LENGTH METHOD (aka GAGE LENGTH) to offset tool lengths. (put the tool length correction in the coordinate system so the machine is driving the SET POINT of the tool, which is the spindle centerline in X-Y and Gage Length in Z. This Gage Length method is the only methods used for OFF LINE TOOL PRESETTING. (As opposed to the crappy FANUC method of slipping paper between the tool point and part face - which sets the tool TO THE WORKPIECE, not the machine!) There are 2 ways to establish tool length - the TOOL SETTER, or teaching off the table (in case your tool setter breaks) The calibrations for the mazatrol auto-calc are mutually exclusive and unless both sets of parameters are calibrated properly, there will be different numbers resulting if the two methods are mixed. The proper way to calibrate both the Tool Setter measuring Parameters and the TABLE TEACH PARAMETERS is with a GAGE TOOL, which is a precision gage in the form of a CAT TOOLHOLDER with a gage length built to gage making accuracies.
KEY CONCEPT - The Tool Length goes with the tool change into the spindle and stays in effect even with reset! EIA TLC (tool length comp)is invoked by program code (G43 Zx.xxxx Hxx, typically) and vaporizes when hitting reset! TLC invoked with the tool change allows you to do the WPC TEACH for Z PART PROGRAM ZERO. You cannot TEACH WPC-Z without first setting a tool!!!!!
KEY CONCEPT - with this MAZAK WAY, once the tools are set, they can be used as is on any set up on the machine! The tool length is the tool unto itself and is not dependant on any specific set-up, like the “Fanuc paper slide” way.
KEY CONCEPT - Mazatrol meat and potatos programming are POINT, LINE and FACE machining. There are other units, but they are ancillary to making chips - these include M CODE units, MANUAL units (abbreviated G code type programming in a fixed column format, helpful when you have something simple Mazatrol can’t handle), MMS UNITS (for spindle probing only. MMS = MAZAK MEASURING SYSTEM) SUBPROGRAM UNITS and a few others I can't remember.
POINT MACHINING - you choose the UNIT TYPE by what your finished part hole feature will look like. Point is only for machining where the feature is generated by Z axis only - drill tap bore, etc. some of the choices are cockamamie - like reverse back c-bore. Mazatrol selects, or suggests, a series of tools it thinks you need. You can erase any tool you don’t want, but you have to create a whole brand new unit if you want a tool back in.
Point machining confusing thing - there is a CIRCLE MILL UNIT contained in point machining. It can generate a contour milled circle ONLY at any X-Y location. Mazatrol does not consider it milling, but being under POINT machining can be confusing.
KEY CONCEPT - once you set up the tools and auto set feed, speed ,D.O.C., there is always the FIGURE PORTION in mazatrol. Point machining is awesome at all forms of patterns and multiple holes for point machining. CHORD PATTERN is painful and mostly useless. Save that for when you become a POWER USER!
KEY CONCEPT - mazatrol surface finish designation are those funky numbers 1 through 9 you get when setting up your tools. It's used with the cutting conditions tables to auto calc F.S D.O.C. It is metric based and arcane. Memorize that 6 correlates to a 32 microinch, 7 is 16, 5 is 63, etc. It is nothing more than a little nudge of info maztrol needs to auto calc.
KEY CONCEPT - the F,S, D.O.C. Auto calcs are bogus in many cases. You as the cnc machinist can overwrite what mazatrol gives you and put in exact numbers for your set up. It's there so anybody that can read a blueprint can become an instant machinist. It gets you in the ballpark, but it is by no means optimized. That comes from the set-up and your judgment and experience as a CNC machinist
Point Machining - at the end of a figure patter there is a question "omit spt machining" THIS DOES NOT MEAN ELIMINATE THE CENTER DRILL. It's a cockamamie concept of mazatrol so you don't double drill a starting point of a pattern. You need two overlapping patterns and the starting point of one has to be coincident with any point in the other pattern. This falls into the delightful category of “solving problems almost nobody has”.
LINE MACHINING - this is milling and ONLY roughs and finishes a string of line/arc figures. Can be closed or open. The step distance for your rough tool is determined by TOOL FILE, which is a table you create yourself for the 4 types of milling tools. I think the depth of cut really means "step distance for rough miller? The TOOL FILE PAGES are a sub set of TOOL DATA. (As is EIA TOOL OFFSET) It's very easy to select the wrong page - put face mill info on to the chamfer tool, for example. The control sorts this info by SIZE PLACE!, so if you last put in an 1/8" dia end mill, (.12 nom dia, as the nominal is a fixed format round off that cuts off a lot of our American fractional to decimal number conversions) when you go back to look at it, it is towards the beginning, instead of the end, where you first put it.
Line machining - spt X and Y in the tool definition lines should be left as "?". When you run a tool path check it will look at the figure you have and certain parameters and automatically calcs decent starting points. You need to turn back to "?" if you change your figure!
FACE MACHINING - I find really cool. It deals with milling AREAS, not line portions. When dealing with areas that have two boundaries - the big outer area is always first and the minor area is always second. The icons in the program make the different possibilities pretty understandable.
KEY CONCEPT - The rough and finish tools have profoundly different jobs to do. The rough tool will work to leave finish axial and radial stock for the finisher to clean up only. You can use the same tool for roughing and finishing, however. The “step distance” the roughing end mill uses is defined in TOOL FILE)
END UNIT - every program must have - you can run continuous loop (great for barfeed lathes, useless for ost m/c's), branch to another program and stop or continue, and park at home or some other place and tool change out or not.
Figure in milling - simple rectangle, circle, or ARBITRARY SHAPE! This will be mostly lines and cw/ccw arcs. Mazatrol has 4 misleading softkeys after line cw arc and ccw arc that are used to POLAR ROTATION of a patter segment or LINEAR REPEATING of a pattern segment. THIS IS FOR POWER USERS! And makes mazatrol unnecessarily confusing! STARTING POINT AND END OF PATTERN s/k's must be used to mark the lines that have additional info for making these patterns. Mazatrol allows the usee of unknown point "?", as long as you feed it enough geometry info for it to make the calu. ONCE A "?" has been filled in, it WILL NOT REGENERATE. you have to turn it back into a "?" and redo shape check or tool path check to regenerate. You can give a line an angle or indirectly define a line backed on the I(X) and J(Y) vector of a right triangle you may have.
At the end of each figure, you can call a TRANSITIONAL CHAMFER OR RADIUS! transitional in that the chamfer is equidistant to the two lines regardless of angle and the radius is always tangent. This is pretty cool, as you only need to program to sharp point instead of calculating all this stuff. You can even use a MINUS R to bridge between two arcs that dont intersect! and it reverses the transitional radius on top of that!
UP/DOWN/LEFT/RIGHT are used with arc that have"?" in them. All it's doing is letting you the programmer choose which of 2 possible line to arc (or arc to arc) intersection points to use in your program. It is only in mazatrol and is funky and is only used if there is "?" in the program. Great for the 1985 CNC paradigm but cumbersome for the 2010 CAD freeware paradigm. I always CADDED out unknown points before mazatrolling because I could!
KEY CONCEPT - Mazatrol does nothing cool for rotary table machining. You can't program an unwrapped cylinder in mazatrol m/c. All you can do is use the RT like an indexer.
Conclusion - This isn't everything, but it should get you over some humps. Mazatrol is PLANAR ONLY - no 3D milling (unless you get the obscure mazatrol 3D option - came and went from 1985-88 or so.)
I learned on Fusion 2002-2009. M1, M2, M32 M+, Fusion and Matrix is the evolution. M1 to Fusion programs almost the same. Matrix was a major overhaul and takes a lot more energy to master completely. Especially the barriers. Main cool thing with matrix is that FACE MACHINING pocket-mountain can have up to 99 inner islands. And the 3D graphics and barriers are remarkable.
If you just copy the program examples attached (CLASSBOOK-M-good-one-cgmcpt0070e.pdf ) it will sink in. You may get frustrated with the pattern repeat examples, save them for later.
I needed to write this anyway, so you're not going to be the only one out there to benefit from the above. it's my first second draft.