EIA programing on a mazak 350 with c axis

[the mill kid]

I am currently trying to do some complex milling on the face of a part using edgecam software. I have been able to get through the program only problem I seem to be having is with the cutter comp, it does not seem to be picking up the tool dia. from the tool data page. I have tried changing parameter f92 bit 7 to a 1 when I retry program I get a tool offset interference alarm, there is no value in that tools offset. I am using cutter comp left (G41) in the program. This is a new machine with matrix control I have extensive experience on mazak lathes but only in mazatrol, I also have been running a mazak 510 miller for 4 yrs using edgecam so I know g code milling very well. There has to be something stupid that I am missing I have tried several ways and reposted my program several times I feel my programming and posted code are correct I just need some suggestions to help lead me in the right direction. Any help would be greatly appreciated.

[jimiscnc]

Parameters:
F92.7 is CRC switch for 'mazak way' or 'g code way'.

1 = cutter c/l is shifted by HALF of 'act-dia' in Mazatrol Tool Data and is invoked with G41/42 only.

0 = offset is contained in "TOOL OFFSET" page, a sub page of TOOL DATA. These registers are intended to be comparable to a G code machine. The G41/42 line also needs a D word to point to the register the programmer assigned.

They are either one value per register or four.

You can do tool path check off the program editor and store tool paths and do experiments and change one thing at a time per scientific method.


and you have to match your programming method to CRC method. The two conventions are

"MAZAK WAY" - program part shape and let crc shift the toolpath as necessary. This would usually be half the effective cutting diameter, plus wear offset sizing correction.

"MASTERCAM WAY" - you tell it the intended nominal cutter dia and the cuttter centerline is shifted in the program coordinates by the cutter radius. This means that any wear offsets applied would be small numbers to correct for effective cutting dia only.

In G code, I think the Mastercam way is the current paridigm for G code machines, and Mazak's using G code, and the Mazak way is woven in to 30 years of mazatrol development.

-Jim

one more point - the sequence of G code commands is critical. Mazak's have a small number of proprietary G and M codes to handle the unusual - most is standardized. For example - there is M200 and M202, which means lathe or mill mode. (I always forget which is which) These are essential to go from lathe to milling and back.

To see what Mazak's like G code wise, just whip up a simple elemental mazatrol program for X-C cutting. nothing more than a rectangle. prove it out, keep it simple and run it through program check and then set it up to cut air.

after the air cuts are successful, go to position page with the small characters - distance to go, buffer modals etc.

put the machine in single block and simply write down the eia commands as single block operation changes them. This would be completely unnecessary if you post was an exact match for the machine. Mazak G code is so similar to standards that a "generic fanuc" post could be edited to suit mazak without a lot of effort.

[the mill kid]

So if I have a 0 in bit 7 and in my cam software program with cutter comp. the program shifts half the dia. of the cutter, then I can use the tool offset page with small increments, wich is what I want, to control size. I believe I've tried this already and I can't remember but I think I got an alarm of incorrect arc data just as it gets to the G41 line. Like I said I have tried so many different combos that everything is running together now. I do have the D word in my program to point to that specific offset. Also on this pc I am cutting some scallops on the O.D. with a 1/2 endmill so I am using a straight lead onto the pc. I have a lead length of.600 to be sure the endmill does not plunge into the face of part there should be enough of a move that I shouldn't have any issues with cutter comp. Also a quick question do you know if a c axis move into cutter comp could cause some problems? Hopefully tomorrow I will have more time and try a series of tests to see what works and what doesn't. Thanks for your help.

[jimiscnc]

first suggestion - get your program to run with G41/42 removed or commented out. if your program runs, good for you. if not, tweak it to run.

secondly - G41/42 can only be invoked with G0 or G1 - definately NOT G2/3!

The coordinate system you are using is the same as the X-Y plane on a machining center, EXCEPT:

C letter address is used instead of Y.

C is true distance and X stays in diameter programming. (theres a G code G122? to turn X into radial/true distance for milling work)

X plus direction vector (axis) corresponds to C0. C plus axis is C 90.0 degrees. this is to control clocking for other milled features that have to be timed to each other.

pg 5-15 in the eia programming manual has it all mapped out and a breif metric sample program. H740PB0071E is the manual number I got.

the tool path check in the program editor is a great tool. it will pinpoint program errors, which are coded. you get an alarm number, and then 3 numbers, which are:

program number,

n sequence number,

line # after this sequence number where the program problem is.

ALARM HISTORY in diagnostics is also good for program prove out.

jim

my instincts are telling me your post processor isn't well matched to your machine as of now?