Need Help!- 640t programming abbrieviations

[Trogdor]

Hey all,

New to cnc machining and self learning while at work.

just having trouble understanding some parameters while using mazatrol programming.

1) if i'm using bar fce it ask for cpt-x and cpt-z which are cutting points, what does that actually mean? compared to spt-x and spt-z.

2) when using drlfce it ask for dep-1 dep-2 and dep-3 how do you define these/meaning of

3) when using grv out, how do you define #and No. whats pitch and is width, width of tool or width of grv?

thanks for your help

Dave

[jimiscnc]

When you are in the program editor, hit the menu button on the extreme right (the extreme left button is display). If the cursor is on the first line of your new Mazatrol Unit, the menu button will reveal another page of softkeys. Use HELP - it will give you a cheat sheet for all mazatrol units except maybe the end unit and m code unit and manual unit. (The other softkeys are editing related. Help is located on the lower right side of the softkeys)

Bar Face - CPT X and Z are concepts needed for that unit. In long hand english it means "The approximate point in which the cutting tool with hit uncut material FOR THIS UNIT." It determines where mazatrol will start rough machining to eventually generate your mazatrol shape.

BAR OUT, IN, FACE and BACK are the four possible feed directions. OUT and IN require you describe the shape from RIGHT TO LEFT, or HORIZONTALLY. FACE and BACK require you describe the shape from up to down, or VERTICALLY.

OUT - starts at cutting point and works its way DOWN to your shape.
IN - starts at cutting point and progresses UP to your shape.

FACE - starts at CPT on right and makes facing cuts to reach your final shape - progressing right to left.

BAK - same as FACE, but the progression is left to right, as it would be for back facing, and CPT X and Z would be the leftmost point.

BAR FCE and BAK are kind of painful to program, because your workpiece view must be tilted 90 degrees from what a lathe programmer is accustomed to.

These are MAZAK CONVENTIONS. It is better to do some UNLEARNING and wrap your brain around mazatrol conventions, rather than expect to change Mazatrol to match your programming methods.

DRL FCE - depth 1 = length of first feed.
depth 2 = how much each subsequent feed DECREMENTS
depth 3 = minimum length of each peck

All Mazatrol drilling is peck drilling - the name chosen determines the flavor of pecking and there's a lot of varients. The most profound difference is BOTTOMING or THROUGH. Bottoming is programming with the drill point, through is programming the hole depth plus allowance for drill point and cut off.

Groove Units - pitch and # of grooves are for multiple grooves. leave this out if only one groove.

Groove Units really benefit from using the HELP pull down. You have six choices of groove geometry type 0 being a no geometry square 'utility' groove and Type 1 is mirrored geometry on both sides of the groove. 2 and 3 are LH and RH varients of 0 and 1 - one side is geometric and the other is straight. Type 4 and 5 are intended for CUT OFF to center, with corner break on right or left being the difference.

The main benefit of the HELP cheat sheet for grooving is that sometimes you sometimes program the right side of the groove and sometimes the left!

Type 0 will allow you to program corner breaks and taper angles - except this info is ignored all all you'll ever get is a straight walled groove with no geometry.

All mazatrol grooving is PECK GROOVING. There is a word in there that usually defaults to .078", which is length of feed per peck. Like drilling, if you make this length of peck greater than your groove depth, it never pecks.

Type 4 and 5 have a means by parameter to proportionally slow down the spindle RPM for CO break through. It's pretty slick and like many Mazatrol benefits, requires some experimentation to master. Surprisingly, this feature is easier to master on the Fusion than the newer Matrix, where this simple feature gets turned into rocket science minutia. Instead of using these cut off RPM benefits, many users just overlay two units over each other - one to get CSS for most of the cut off, and another to get to direct RPM so the falling part does not get shot about the work area.

Hope this helps. I used to teach this stuf.

-90% Jimmy

[fizzissist]

All the above is good stuff.

Note though, that cpt-x and cpt-z can give you an alarm IF they don't jive with the material description in the first line, or if the previous unit has removed material .....

Don't freak out, just play with it until you start to get a sense of how the Mazak thinks. It only took me about 3 years. Others should pick it up a little bit quicker.

Do NOT forget to set a proper change point, or you can change a tool when you haven't retracted the turret first to a safe location. Most of us call that a crash. Owners call that expensive. On my 640T Fusion, it's a '1'.

Note too that in grooving you need to pay attention to where the start point is on the tool, and where it is on that operation.....on one type of groove, it's on one side, on another, it's on the other side...like type #2 and #3....
It's shown on the Help screen.

Getting someone to help walk you through it on the machine will save countless hours and beer.

[Trogdor]

thanks for your help guys, will check out the help menu.
i've got all the operating manuals, just not one for the mazak conventions which is annoying but at least theres the help menu.

it's bloody scary progamming and hoping not to crash the machine when your new at it.

i'm having issues with bar fce atm, trying to do a tapered face.

my values are cpt-x 27, cpt-z 0, spt-x 27, spt-z 0, fpt-x 54, fpt-z 1.75.

issues is the taper isnt working properly starting at the wrong place and not deep enough on the outside edge. the part is a 54mm washer with 27mm hole with the taper from the hole to outside edge (0-1.75mm). any hints?

[jimiscnc]

I think this will work for you.

BAR FACE
CPT-X 54. CPT-Z0
TAPER SPT-X54. SPT-Z1.75 FPT-X27. FPT-Z0


You seem to want to face from small to large. Unfortunately, the above is for large to small. I honestly don't know how to mazatrol facing cuts from small to large like you're trying to do. A BAR OUT Unit will get you a finish pass from small to large like you want, but all the roughing passes in BAR OUT are longitudinal, not diametrical. THE TRICK to at least get a good small dia to large dia FINISH PASS is to simply leave out the ROUGH TOOL number in the Unit. If no rough tool, then the Unit will only drive a finish tool. This is what I call MAZATROL TECHNIQUE, which is nothing more than tricks and techniques to be effective in Mazatrol, which aren't covered in the books so much.

A couple of more points to spare a newbie some HARD LEARNED LESSONS.

All Mazatrol Units have Mazatrol indexing built in to them. Parameter P17 chooses which indexing point you want to use. I personally like setting 4, which is a fixed point by parameter in machine coordinates.

The one exception to this turret index rule is the MANUAL UNIT! At the beginning, you can program a new tool (or not), but at the end of the unit, you the programmer must program the tool point to the turret index position. MAZATROL WILL NOT DO THIS FOR YOU! Please don't make this mistake! Indexing into the workpiece is TRAGIC!

TOOL PATH CHECK - you should get accustomed to using this. It's important to know that the red dot and plotted points in tool path check are FROM THE CENTER OF THE NOSE RADIUS, not part shape! To get the actual coordinates for your part shap, SHAPE CHECK and SHAPE CHECK, STEP, will give you the coordinates of your shape. You can also get finish part shape if you change tool nose radius in tool data to ZERO!, do your check, then change it back to actual rad. This is asking for trouble if you forget to put the real radius back in. (There is also a TRACE display when running in auto - this is a real time tool path check and the numbers for trace use the tool SET POINT, not the tnr center point that TOOL PATH CHECK uses.)

Navigation - forgive me for stating what Mazatrollers will find PAINFULLY OBVIOUS, but it's important to be on the same page. Leftmost key is the DISPLAY KEY - this gets you to the main pages of all mazatrol. The rightmost key is the MENU KEY, which gets you to additional pages of what ever active page is displayed. First hit of display key gets you to the same set of softkeys - the rightmost one is DISPLAY MAP, which is navigated with arrow keys and input keys and allows you to find pages by this map instead of navigating the DISPLAY and MENU buttons.

KEY CONCEPTS

Mazatrol programs use the MAZATROL COORDINATE SYSTEM. The main tenets of this are the tool offset GOES WITH THE TURRET INDEX, not program code. And RESET does not turn off the active tool offset. It's in the coordinate system until indexing to another tool.

Each program has it's own Z offset. (Look at the SET UP PAGE) The tools are set "to the machine" with the tool eye. The Z-offset shifts the Z program zero to be coincident with the finished face of your part, as it sticks out into the work area. The Z offset is invoked by the active program call and once again does not RESET. The tools are SET TO THE MACHINE and only need to be changed to adjust for wear or if the tool is swapped out. Only the Z OFFSET is set to the workpiece. There's a TEACH function to establish the Z offset and also teach for tool setting, if your tool eye is down. Touching off a tool to your workpiece requires the additional step of INCREMENTALLY correcting the taught value by exactly the Z offset. For X it's always taught to X centerline and needs no massaging. The Z offset will shift the entire program depending on the magnitude and direction of the number. The tool set in tool data only applies to the individual tool.

Mazatrol is counter to the FANUC PARADIGM, where Z zero is established by G54 Z register, and tools are usually touched off to the workpiece. Note that tool offset and G54 Z value are wiped out by RESET. Not the case for mazatrol programs!

I consider mazatrol 2 axis lathe to be the most beautiful way to make good lathe programs that currently exist on this earth.


-90% Jimmy

[fizzissist]

You have manuals?
There are 3 manuals that are critical.....Operation, Programming, and Parameters. If you've got those, no matter how obtuse or cryptic they seem (or in fact are), you've got what you need.

The Z convention doesn't seem consistent to a regular G-coder, and, well, it isn't. Normal programming will have a +Z value from the face of the part towards the chuck with your Z0 at the right-hand end of the part. Always. Otherwise you're asking for nightmares. Doesn't matter how the part is drawn or dimensioned.

--In your stock setup on the first line you'll have a value under Work Face..that's the amount of stock in Z to the right of your Z0 that you'll face off. That value is a +Z. That very same value, again positive (which is one example which screws up the convention) will be used in the normal Face operation for the CPT-Z . That's where the tool will go to start cutting. CPT-X will be the same as the OD-MAX. ..........The Parameters book will show you how close to those settings the tool will actually come, and how you can adjust that to your own preference. ...but DON'T GO MESSIN' WITH THEM IF YOU DON'T NEED TO. (boring bars being the lone exception...more later)

We're gonna go backwards for a minute....First order of business is setting your chuck jaws on the machine,,,then going to SetUP, and input the values into the jaw table. Do this for the program, AND for safety barriers.

Set your tools, input their descriptions and use the Tooleye or test cuts to input their respective offset values. Have to assume you know how to do that??

At the same time you start to compose the program, make that same program active on the control (Unless there's another part that needs to be running while you're programming). This will allow you to check your program as you go because it'll display the chuck jaws, tools, and any alarms will mean something.

So like jimiscnc is saying, it looks like you're trying to cut a taper that goes from the hole towards the O.D., and tapers back towards the chuck...right?

I haven't used the BAR FAC the way he is suggesting, and honestly don't know how that performs. (I'm at home, so can't even try it, and I think in inches... )

Instead, I'd use BAR OUT CPT-X is O.D. of stock, CPT-Z is Z0 (since you've faced the stock already using EDG FAC....?). This will cut from the front towards the back, I.D. to O.D.

(gonna pretend that the actual stock is 54.1 O.D., there's a 27 hole in the mat'l, and the finished part is 3 thk)

The code would look like
BAR OUT CPT-X54.1 CPT-Z0
TPR SPT-X27 SPT-Z0 FPT-X54 FPTZ1.75
LIN SPT-X54 SPT-Z1.75 FPT-X54 FPT-Z6 (turns O.D. back past 3mm wide cut-off tool

....safe to assume you were going to use grooving to cut off??

Next Unit would be GRV, and I'd use #4 which will chamfer (or radius) the back edge.

GRV OUT #4 WIDTH (your tool)
S-CRN (desired chamfer) SPT-X54 SPT-Z3 FPT-X26 FPT-Z3

--Note...you can use the FINISH to set the tool to go past the end FPT-X to compensate for tip radius , I usually just tell it where I want it to go.

Now, this is where you can get into alarms that don't seem to make sense. You're telling the control to go to FPT-X26, but there's no material there, because your material description in the very first line has an ID-MIN of 27, right? This could trigger a MazAlarm (the other name for Mazatrol). You'll stand there scratching your head, throwing things, and wondering what the hell you did wrong. This is where you learn how to lie. Mazak likes being lied to. You could change the ID-MIN to 26 and it'll be happy as a clam.

jimiscnc calls it Mazatrol Technique. He's being nice. Tricks and technique is where you duplicate a Unit and rerun it without a roughing pass and a slightly deeper kiss cut because of chips, or whatever. There's a whole bunch of those, and practically NONE of 'em are in the books. You have to use tricks, AND lie to it.

...'Nuff for the moment..jimiscnc has given you some very good stuff to chew on!!

[Nexus700D]

I am a Mazak CNC machinist of 10 yrs plus. I am familiar with many controls in the Mazak line of machine tools. I would gladly do setup work and/or programming as needed for extra cash. If you are interested don't hesitate to contact me via CNC Zone. I would very much like to do journeyman work on weekends. Thanks!