Mazatrol subprogram

[vxss57]

Hi everyone, first off what a great site. I have a very simple job at the moment, roughing 16 teeth on a spur gear. Is it possible to write milling units in Mazatrol language and then use subprogram (EIA/ISO) for indexing the C axis. At the moment I have my main mazatrol program which contains WPC, second mazatrol programs which contains cutting units and third ISO prog which contains indexing code. I get the cutters to rough out the first tooth it indexes to the next tooth but it then goes back to first tooth and it repeats this 16 times. what am i doing wrong. thanks for any help in advance,

[bildoo]

I believe that your programming technique is correct. There is a parameter that allows or disallows the repeat of an eia program that is a sub program. I ran into this issue a couple months ago when I had to repeat an eia program (that had an elipse shape cutting) that was the sub of a mazatrol program. The machine kept repeating the shape in the same place. I think it is an "F" parameter but I will look it up when I can get to a parameter book tomorow morning at work. What control are you using (M32, T+, Fusion)?


Thanks.

[vxss57]

I believe that your programming technique is correct. There is a parameter that allows or disallows the repeat of an eia program that is a sub program. I ran into this issue a couple months ago when I had to repeat an eia program (that had an elipse shape cutting) that was the sub of a mazatrol program. The machine kept repeating the shape in the same place. I think it is an "F" parameter but I will look it up when I can get to a parameter book tomorow morning at work. What control are you using (M32, T+, Fusion)?


Thanks.

Thanks bildoo, its an integrex so I think its fusion

[bildoo]

Parameter "F70" is to validate multiple machining of an EIA program. Set it to "1" to allow multiple machining.


Let me know if this works for you.

[vxss57]

Parameter "F70" is to validate multiple machining of an EIA program. Set it to "1" to allow multiple machining.


Let me know if this works for you.

thanks mate that worked excellent, I appreciate the help thanks again

[vxss57]

I probably spoke few months too early. we finally got the gear job and I had it programmed few months earllier. the F70 parameter solved the problem when running the tool path simulation. but for some reason when actually running the machine, just before it needs to index the c-axis I get an error "128 Outside interlock axis" which in the mannual reads "an axis is interlocked because the interlock function has become active" and to solve this "clear the active state of the interlock function" maybe this sounds dumb but how exactly do I do this? thanks for your help

[bildoo]

Alarm 128 comes up because you are trying to move the C axis with the C axis brake (clamp) on. You must put a M43 before the C move. If you are cutting using the C axis to feed I would put this at the begining of the program. If you are just indexing I would put M43 before the move and M44 after so it clamps again (making it more rigid). Those M numbers may vary depending on your actual machine setup so look in the M code list for your machine operating manual. Or if it is a fusion or matrix go to an EIA program screen and click on the help meun (at the top of the screen) then M code for a list.

[vxss57]

This is my Eia/iso program layout

g91 g00 m212 c7.2
m210 m99

With this I get an overload error just before indexing.
m212 is c axis unclamp
m210 is c axis clamp
Do i need to have any other mcodes (such as braking) for this to work.
Thanks bildoo you have been great help

[vxss57]

Got it to work finally, got some help and played around with positioning of m codes, thanks bildoo once again

[bildoo]

I was just about to reply to you to put the M212 before the move line. Is that what you had to do?

[vxss57]

I was just about to reply to you to put the M212 before the move line. Is that what you had to do?

thats right
M212
G91 G00
C7.2
M210 M99