[Chais82]

I have these very simple rings i need to machine. All that is required is to bore the id and cutoff. Im using a 10" long pc and gonna cut as many .5" pcs I can get out of it. My question is can anyone help me figure out how to move Z grid in the program? So every time it finishes a pc all the tools will move in the required amount on z until I hit my amount of pcs then stop. This is something I could program on my Okuma lathes. But fanuc seems to be different. Thanks in advance guys!

[fizzissist]

I did this on a Fanuc 6T-B machine in '83. Wrote a macro to do a part, shift the Z, do another part, shift the Z, do another part, shift the Z.... After the 6th part, the machine would reset and go home. Load another bar and hit the green button.

It's not that hard to do (it was my first macro!) and a great exercise in learning how to write and implement macros.

[Chais82]

Ive dealt with macros years ago, but very briefly. I also didnt write them then. Ive just worked with them in previously written programs. i guess my next question would be where can I find info on how to write a macro? I do write all my program mostly without mastercam. I do have a lot of experience writing programs. Just not macro's. Any help would be appreciated!

In the mean time I will do some research and try to figure this out myself. Im just on a time constraint. Thanks in advance!!!

[txcncman]

In your case, you may not need a macro. I would be tempted to write all of the cutting moves in incremental mode as subprograms for each tool. Then in the main program position the tools at the appropriate start point. You might also consider what tool you will use for machining. A specialized groove tool that is capable of turning might be in order. Then the entire process runs from the one single tool. I have used Iscar tools for this in the past.

Upload a part print or sketch and maybe someone can help you actually construct the needed programs or macros.

[fizzissist]

In your case, you may not need a macro. I would be tempted to write all of the cutting moves in incremental mode as subprograms for each tool. Then in the main program position the tools at the appropriate start point. You might also consider what tool you will use for machining. A specialized groove tool that is capable of turning might be in order. Then the entire process runs from the one single tool. I have used Iscar tools for this in the past.

Upload a part print or sketch and maybe someone can help you actually construct the needed programs or macros.

What he said.

..Your machine should have a manual for the control, and it should contain the syntax and accepted command structure and calls for macros, if the control will do macros.

[Chais82]

In your case, you may not need a macro. I would be tempted to write all of the cutting moves in incremental mode as subprograms for each tool. Then in the main program position the tools at the appropriate start point. You might also consider what tool you will use for machining. A specialized groove tool that is capable of turning might be in order. Then the entire process runs from the one single tool. I have used Iscar tools for this in the past.

Upload a part print or sketch and maybe someone can help you actually construct the needed programs or macros.

like I said extremely easy part. Its 3.25" OD 304 SS with a .188 wall thickness. All im doing is turning the id to 3.01 +.005 -.000 and cutting them off at 1/2". There is no OD turn required. The length is a fractional number so they don't have to be perfect. Maybe just a face on the first part to clean the marks done by the saw. after that it would be just bore and cutoff till I get 10pcs. I also went with a 8" tube instead of 10" because i was getting to much chatter. The jaws take up about 1.5" to hold the 8" tube. So I can get about 10pcs a tube.

I love your idea to write subprograms. But Unless I do 10 different offsets for bore and cutoff, Im still in the same situation. How can I get the program to move Z0.0 in for each part? I'm having a mental block right now. So im sorry for the noob questions. Thanks txcncman and everyone else for your help.

[txcncman]

Does your control have G10 settings command?

Does your machine have multiple work zero offsetting (G54, G55, G56, etc.)?

Does you machine have macro capability?

[Chais82]

Does your control have G10 settings command?

Does your machine have multiple work zero offsetting (G54, G55, G56, etc.)?

Does you machine have macro capability?

It does have G10 but I just dont understand how its saying to write it. I get an alarm when I try. I added a pic of the page in the book on how... http://instagr.am/p/RGCn7DHaol/

Thanks Again!!

[txcncman]

You still will need to write your program to cut one ring and set it as a sub program.

G10 L2 P1 Z-zz.zzz should be the correct sintax. Z will equal the distance from machine home zero to part work zero, the same as G54. The way it would be implemented is in the main program:

%
Oxxxx (Main)
G10 L2 P1 Z-zz.zzz
M98 Ppppp
G10 L2 P1 Z-zz.zzz
M98 Ppppp
G10 L2 P1 Z-zz.zzz
M98 Ppppp
G10 L2 P1 Z-zz.zzz
M98 Ppppp
M30
%

Should cut 4 rings. First Z above would be front of material minus clean up amount. Subsequent Z's would be first Z minus part length, minus part off tool length, minus clean up amount.

[Chais82]

You still will need to write your program to cut one ring and set it as a sub program.

G10 L2 P1 Z-zz.zzz should be the correct sintax. Z will equal the distance from machine home zero to part work zero, the same as G54. The way it would be implemented is in the main program:

%
Oxxxx (Main)
G10 L2 P1 Z-zz.zzz
M98 Ppppp
G10 L2 P1 Z-zz.zzz
M98 Ppppp
G10 L2 P1 Z-zz.zzz
M98 Ppppp
G10 L2 P1 Z-zz.zzz
M98 Ppppp
M30
%

Should cut 4 rings. First Z above would be front of material minus clean up amount. Subsequent Z's would be first Z minus part length, minus part off tool length, minus clean up amount.

I really do appreciate your help!! I will give it a try now and report back when done.

[Chais82]

You still will need to write your program to cut one ring and set it as a sub program.

G10 L2 P1 Z-zz.zzz should be the correct sintax. Z will equal the distance from machine home zero to part work zero, the same as G54. The way it would be implemented is in the main program:

%
Oxxxx (Main)
G10 L2 P1 Z-zz.zzz
M98 Ppppp
G10 L2 P1 Z-zz.zzz
M98 Ppppp
G10 L2 P1 Z-zz.zzz
M98 Ppppp
G10 L2 P1 Z-zz.zzz
M98 Ppppp
M30
%

Should cut 4 rings. First Z above would be front of material minus clean up amount. Subsequent Z's would be first Z minus part length, minus part off tool length, minus clean up amount.

So I tried real quick to just write the "G10 L2 P1 Z-zz.zzz" in MDI as "G10 L2 P1 Z-0.25;" Just to see if the g10 works. But I get a 010 alarm(improper G code) Must be something im not understanding. Thanks again!

[txcncman]

I do not think your lathe has this option enabled.

If you have G54-G59, you can still sign the part zero offset outside of the sub program:

%
Oxxxx (Main)
G54
M98 Ppppp
G55
M98 Ppppp
G56
M98 Ppppp
G57
M98 Ppppp
M30
%

Then you will need to input the appropriate values in the work offset table. Make sure you do not call a work offset within the sub program. Do it externally.

[Chais82]

I do not think your lathe has this option enabled.

If you have G54-G59, you can still sign the part zero offset outside of the sub program:

%
Oxxxx (Main)
G54
M98 Ppppp
G55
M98 Ppppp
G56
M98 Ppppp
G57
M98 Ppppp
M30
%

Then you will need to input the appropriate values in the work offset table. Make sure you do not call a work offset within the sub program. Do it externally.

So This isnt something I can turn on in the parameters? Im just trying to avoid using g54 g55 g56 and so on because that limits the amount of parts I can make without making a real sloppy program. You've been a real big help. Im very great full!

[fizzissist]

Regardless of control capabilities.... There is one simple way to fix this...

Open up Notepad and write the program to bore and cut off one part. Cut and paste that repeatedly, equal to the number of parts you want to make per blank.

Insert a comment line in between each to make editing easier, then go into each portion and edit the Z values appropriately. There's your program, done in Notepad.

Another way around is to create the part in Mastercam, and post the code. Shift the part, and rewrite/re-post the code as a different part (#2, for example). Shift it again, and again, re-posting each time. Then copy and paste those different parts into the first one, simply editing the transitions so you don't have any pauses, tool changes, whatever.

You don't need macros, subroutines, calls, or special control options. You're just doing it the hard way.

In the alternative, you could pay txcncman to do it for you! (slightly shameless plug)

[txcncman]

Regardless of control capabilities.... There is one simple way to fix this...

Open up Notepad and write the program to bore and cut off one part. Cut and paste that repeatedly, equal to the number of parts you want to make per blank.

Insert a comment line in between each to make editing easier, then go into each portion and edit the Z values appropriately. There's your program, done in Notepad.

Another way around is to create the part in Mastercam, and post the code. Shift the part, and rewrite/re-post the code as a different part (#2, for example). Shift it again, and again, re-posting each time. Then copy and paste those different parts into the first one, simply editing the transitions so you don't have any pauses, tool changes, whatever.

You don't need macros, subroutines, calls, or special control options. You're just doing it the hard way.

In the alternative, you could pay txcncman to do it for you! (slightly shameless plug)

LOL. Thanks. He could just post his work here and get help for free.

[Chais82]

Regardless of control capabilities.... There is one simple way to fix this...

Open up Notepad and write the program to bore and cut off one part. Cut and paste that repeatedly, equal to the number of parts you want to make per blank.

Insert a comment line in between each to make editing easier, then go into each portion and edit the Z values appropriately. There's your program, done in Notepad.

Another way around is to create the part in Mastercam, and post the code. Shift the part, and rewrite/re-post the code as a different part (#2, for example). Shift it again, and again, re-posting each time. Then copy and paste those different parts into the first one, simply editing the transitions so you don't have any pauses, tool changes, whatever.

You don't need macros, subroutines, calls, or special control options. You're just doing it the hard way.

In the alternative, you could pay txcncman to do it for you! (slightly shameless plug)

I appreciate your advise. This is the way I did it. Which is copy and paste in notepad and changing each z appropriately. Unfortunately as I stated before this is a fanuc 10T control. It's old. Therefore wont hold a program at that size.
I'm not looking for anyone to do it for me (even though I pretty much am asking for that) I need to learn this type of thing for the future. I have a new lead position in lathe dept. I'm responsible for everything except operate (program, setups, ordering, keeping all tools in stock etc). I've only been machining for just under 7 years. I've been running my dept. now for the last year and a half. We are under a new owner and the company is growing fast. I'm looking to learn this type of thing on my own for obviouse reasons. I will figure it out. Just trying to suck as much info as I can out of you guys. . The problem with my generation is the old timers don't like to give you any info. The only reason I know what I do know is the few people I have worked with were willing to teach me because of my ability to to the job. What i will do is ask the inlaws what they think. Between the two of them they have 40+ years experience. I just hate going to them. Thanks txcncman and fizzissist for your help.

[txcncman]

The old timers don't like to give out info, because when they do, they get replaced with some young guy that is willing to work for less money. It is a matter of survival for most of them. Also there is the idea of working for your knowledge. (Think school of hard knocks.) These old guys took their knocks. Why do they need to make it easy on you? What do they get out of it? In the days of apprenticeships, apprentices earned their knowledge by doing all the dirty work that the old guys don't want to do. Did you spend your time cleaning up some old guy's work bench? Organizing tools? Resharpening drills? Sweeping floors and cleaning out chip pans? If you were doing all these things, those old guys should have been sharing their knowledge with you. If they didn't, their fault.

What is the max file size you can load into your machine?

Upload the code you have so far and let's see if it can be condensed.

[Chais82]

The old timers don't like to give out info, because when they do, they get replaced with some young guy that is willing to work for less money. It is a matter of survival for most of them. Also there is the idea of working for your knowledge. (Think school of hard knocks.) These old guys took their knocks. Why do they need to make it easy on you? What do they get out of it? In the days of apprenticeships, apprentices earned their knowledge by doing all the dirty work that the old guys don't want to do. Did you spend your time cleaning up some old guy's work bench? Organizing tools? Resharpening drills? Sweeping floors and cleaning out chip pans? If you were doing all these things, those old guys should have been sharing their knowledge with you. If they didn't, their fault.

What is the max file size you can load into your machine?

Upload the code you have so far and let's see if it can be condensed.

I understand this about the old school machinist. And I have much respect!!! I did have to earn my position. And I was always givin respect in return. They have showed me the same respect. I meant no disrespect. But I have to disagree with the thinking here. My feeling is because people don't help one another is the reason there aren't enough skilled workers to do the job. The machining world is a lot different from back in the day too. And most old school don't know the new CNC part of it all(atleast in my experience). But that's political and I don't do politics lol. Ill be able to get the program loaded by shortening it. Was just trying to pick your brain. I thank you so much for your help! Lots of respect here for you two!

[Chais82]

For the record, I didn't get my job by replacing a guy for less. I earned where I am. And am very proud of it. I do not expect a hand out. And I'd be the first to help anyone who needs it. So I forgot sometimes others don't feel this way. I hope I don't come off as an *ss. Thanks again for taking the time to help.

[txcncman]

I understand this about the old school machinist. And I have much respect!!! I did have to earn my position. And I was always givin respect in return. They have showed me the same respect. I meant no disrespect. But I have to disagree with the thinking here. My feeling is because people don't help one another is the reason there aren't enough skilled workers to do the job. The machining world is a lot different from back in the day too. And most old school don't know the new CNC part of it all(atleast in my experience). But that's political and I don't do politics lol. Ill be able to get the program loaded by shortening it. Was just trying to pick your brain. I thank you so much for your help! Lots of respect here for you two!

You are correct about employees not working as a team. I did not mean to imply that you have done anything wrong. All of the questions were rhetorical from the view point of "the old guys".