Mazak 250MY Circlular Pocket Milling

[250my]

Can anyone tell me if the following is possible.
On the Mazak Matrix 250my i want to machine a circular pocket in a face, but i want the tool path to spiral out from the center of the pocket to the outside diameter of the pocket.
Because of limits of the X and Y axis when used together, i need to be able to do this using X and C axis.
Anyone help please.

[shafter]

You can use the x and c Axis to pocket mill.
I find that pre-machining with a different tool or drill first helps.
You can mill a tight limit bore this way and it gives you a good pcd.
Program your co-ordinates in (you may have to use the centre of the cutter).
If your machining a circle or an arc and you want to change the size, try changing the radius in the program slightly.
I know this is a bit vague, let me know how you get on. If you can,t get it to go i'll give you my email address and i'll give you a program example.

[250my]

Thanks for the reply shafter, maybe i am not fully understanding your reply, but milling a circle is not the issue.
Lets say i have a 100mm circular pocket to machine 10mm deep, which is not on the x axis center line of the lathe(otherwise i would just bore it), lets just say it is 50mm off center.
I want to use say a 25mm cutter to machine this pocket. On a milling machine i can machine this pocket using circular pocket but in a helical motion, ie spiralling out from the pocket center.
I want to know if i can somehow do this on the lathe.
I cannot use circular pocket as it it outwith the limits of the x y axis.
I somehow need to do this using the x and c axis, with z being my depth.

[jimiscnc]

On axial/face oriented machining, most of the units for point, line and face machining, in the figure portion of the unit describing the finish part shape, it will allow you to chose between two coordinate systems. Polar=R for Radius, C=degrees OR X-Y input r/X and c/Y. The headings of the columns in the unit are R/x and C/y. Rather than look at the column headings, which serve multiple purposes, look at the wording to the left of the dialog box in the lower right where you enter your program info. This dialog box is always "attached" to cursor position and the text to the left is a lot more meaningful than the column header abbreviations.

If you select X-C, the motion is always polar - rotation in C degrees and in-out movement in X. You can choose between programming the figure portion in polar coordinates or rectangular coordinates. If you use "X-Y input", then you are looking at the face of your part EXACTLY AS IF YOU WERE making it on a machining center, with program zero being the centerline. To overlay the feature timing between polar coordinates and X-Y coordinates, C0 degrees is the X plus axis direction, C90 degrees is the Y plus axis direction, C180 is X-, and C270 is Y-. C330 is also the same angle as C-30. 330 degrees implies clockwise and C-30 goes to the same point counter clockwise. this may be moot, as C is describing a coordinate point, not an angle direction vector. (Or not - it may be a factor if contour milling using R/C coordinates?)

If you are using X-C polar motion the worst programming crime is simply to go through part centerline. Given a 2" dia part, starting at X1.0Y0 to X-1.Y0 creates a phenomenon when the feed hits centerline. The C axis will "instantly" rotate 180 degrees and X will go from minus direction to plus direction also "instantly". This is because Mazatrol don't do any machining on the negative side of the X axis! Older Mazaks will trip out the servos trying to do this "instantly". Newer Mazaks can actually handle this, the feedrate slows down enough when C is rotating for the servos to handle it. The reversal error marks on your part will be noticeable and all the error in tool set, centerline of driven tool head and actual cutting diameter (where mazatrol gets the number for CRC) will be apparent in the walls of the cut part.

It's helpful to think of the cutter to the tool to program stuff like this. Thinking of machine motion while programming will trip you up and you don't have to with mazatrol!

One last note - in the tool path check, the face view clocking puts C0 at 12:00. Go into I think scale or plane change and you can reset the angle of the display. offsetting the angle by 270 degrees clocks C0 with X plus direction, so it makes it more understandable. It gives you the same view as if you were programming on a generic 3 axis VMC. Find the STORE softkey - menu gets to second page of softkeys to find it. This will keep your scaling adjustments ON, so you don't have to tweak up your scaling every time you use tool path check. Your store setting goes back to default when control is turned off, however.

Hope this helps!

-jim

[CNCRim]

250my,

Simple answer to your question is I don't think so, see the problem with any conversational is you have to do what they want to instead you want it to do. However you can have it done your want with NPM

[shafter]

You won't be able to helical mill in 'x' and 'c'.
You can slot drill using several circular motions to produce a large eccentric bore/hole i've done it a few times. I'll scan a copy of a program and post it at the weekend.

[shafter]

I have done this simple program, once modified to suit your part it works fine.
You won't need a finishing cut on each process and if you want a fine tolerance leave just .3mm / .010" after a roughing process then put in a final pass. If you want a finish pass at the centre of a pocket just put a line across the centre line.http://www.cnczone.com/forums/attach...1&d=1269699776

[jimiscnc]

I COULD BE WRONG, but point machining - circular mill may be able to helix. There's a column to set TORNA - which is a binary switch for circular milling or TORNADO, helical milling. (Not too many people in the US equate "tornado" with "helical tool path", but that's the fixed format Mazak chose when dealing with a few helical path scenarios - such as the type of pocket entrance for face machine-pocket, and also for threading by thread mill instead of a tap.)

Because this is a subset of point machining, the only finish geometry you can generate is a circle.

Got this from the manual and it is untested on a machine.

I don't think there's another possibility for X-C machining helical entrance, as this only allows POINT AND LINE machining. I'm pretty sure you can helix a lot more stuff in X-Y machining, as this allows FACE MACHINING Units, which are all variations of milling bounded AREAS, instead of POINT OR LINE MACHINING, which deal only in points or lines, NOT AREA.

There may be a slim possibility that you can helix using Line Machining, LINE IN? Line in or out has to have a closed shape to work, like FACE units, but is only driven by the outer line boundary and only allows a rough and finish pass(es) about the line shape. FACE unit would clear out the entire area.

jim

[jimiscnc]

I MADE A MISTAKE IN POST FOUR

original sentence:

330 degrees implies clockwise and C-30 goes to the same point COUNTER clockwise.

Should be

330 degrees implies COUNTERclockwise and C-30 goes to the same point clockwise.

sorry

Jim