picking up a long nc program where it "left-off"

[Diedesigner]

Hi all,

When running a long program as in finishing a die or mold, if you lose a cutter for whatever reason, how do you pick up your milling cycle where it "left-off"?

Have any of you dealt with this sort of problem?

 

Thanks,

Chris

[chris m]

That depends greatly on what type of machine and control you have; do you have a specific one in mind?

 

C

[Tony]

DieDesigner

There is a Free Mastercam Highspeed/High feed

seminar At Chicago machine tool in Elk Grove.

March 13th and again on the 14th. (1 hour long)

You have to register. 1 847 364 4700.

 

And now back to are regularly scheduled programming....How to figure out where you were and Chop your program to that point

[Diedesigner]

Chris M:

I have two controls/machine types in mind; Fanuc16mi/Okuma & Howa vmc, and a Fadal vmc. I don't know much about the Fadal.

 

Tony:

Thanks for the info -- I will try to make it.

[chris m]

My condolences on the Okuma & Howa.

 

The Fanuc controls can be tricky for this type of thing, I'm sure some of the mold guys like Jay, James, or Scott Bond will be of more help here.

 

I don't have much familiarity with the Fadal control; does it have a "restart" feature? We have several Okumas which have a restart feature that allows you to pick up a program on any line you want; very nice.

 

Sorry I'm not too much help here

 

C

[Dan Bedore]

what i do is copy the whole line of code where i want to restart then i do a find using that data. there should only be one line of code that matches, if there are more then you will need to check lines of code before and after to determine which line is the correct line. or you could edit the code at the machine i mean add a * or something to the line of code you want to start on and save the program that way. then search for that * then you can delete all the code between that symbol and your initial g and m codes. then you will have to add some x, y, and Z moves to safely get you into position to restart. i try to restart on a line that has a x,y, and z move in it. then i copy the x and y numbers from my restart line ahead of the line i want to restart on. that usually is a safe move if the cutter is all the way up on the z. don,t forget to add your G1 fxxx and turn your feed rate or % way down so you come into the part slow at first. I don't always have great success with this because i might be a little off on my tool setup.

[TheePres]

On Fadals it's peace of cake, use the AU command.

As in au,725..this will rapid to XY of 724 block then feed down to 724 'Z' level and do normal feed to 725.

In Fanuc I do search for previous Rapid out, note block number. Then start tool in single block, after has picked up tool offset move selector to manual then edit..manual again..then back to edit, now do search for noted block number or sometimes to the next XY block (dont page down-use N??? arrow down key), place back in auto and your set to go. On occasion you will need to edit program to insert feedrate or "D" for cutter-comp.

[chris m]

I'm glad we're not the only ones doing that with Fanucs...

 

Since Fanuc has such a business making CNCs, why do they have the least user-friendly features imaginable?

 

C

[jdempsey]

On the fadal you do have the option of jogging the tool away from the part and returning to the same point while the program is running by hitting slide hold and jog. You also can start in the middle of a program by putting the cursor at the line that you want to start at and going to the edit screen, press auto, choose option 3 search for modals and start at cursor line. HTH

[Zero]

Don't know about the controls you're using...but you could edit your gcode to start from the closest z retract to where you left off and run it. Make sure you start at the closest z retract or you could crash your part.

 

[ 02-25-2003, 01:01 PM: Message edited by: Zero ]

[jadaro]

I agree with the latter,

 

However if you were NOT in the middle of a really long toolpath, you can post all the remaining toolpaths from the operation menue.

To select the remaining ones that you want to post, slect one, then aditional ones by clicking on them while holding down the Control button (similar to slecting multiple files in the file manager).

 

Then click the post button, this will post all the selected paths as if they were their own program.

 

Retain the same height offsets, etc, origin also.

 

You will likeyly have to restart the toolpath it was working on while the cutter broke etc.

 

[ 02-25-2003, 03:53 PM: Message edited by: jadaro ]

[Mark H]

As far as editing the G code and deleting everthing above it, make sure you watch your G17, G18 and G19 in your arc moves. (Some posts dont output a G17 for each and every G2 or G3) Also watch any cutter comp.

 

[ 02-25-2003, 03:25 PM: Message edited by: Mark H ]

[Brendan P]

When using a fanuc control,I would do what Zero mentioned.But I would add a little code to the program to get me to where I want to start back up.

After the tool reads the G43 Z.1 line,I would then

put in the next line M99 P2000 all by itself.

(The "p"# can be any number you choose,as long as you are not already using it).

Then on the line that I want to pick back up on,

I put an N2000 (this # has to be the same # as

you used as the "P" #).

 

Most of the time you will have to assign a feed

to the line you want to start back on too or

you may get an alarm.

In essence the M99 is just a return code,and all

it is doing is returning it foward in the program

just where you want it.

 

Hope this helps

[resjun]

mazak does it realy cool while the machine is running cutter blows a gasket just push manual button then tpc button then use the mpg handle move away from the part change insert push memory again and it goes in the reverse direction

[Finecut]

And in Haas its make sure parmeter 36 is on. Go into edit and highlite the place you want to start, hit the memory button, hit start.

piece of cake!

Finecut

[toolman321]

This happens frequently in my work (mold building). Rarely does it occur while the machine is being watched, so using the jog/resume type of features is rarely an option.

 

Determining at what point the program should be restarted can be done several ways. One can measure using calipers or other measuring tools to find a safe location to resume cutting. Some times I will jog the machine over the area and note the coordinates where the cut was interrupted.

 

It is then a matter of editing the g-code. Any text editor will allow you to search and find the desired coordinates. Once they are found, it is only necessary to delete code after the preparatory codes at the top of the program up to the point you want to resume cutting, while paying attention to ensure that:

 

1. The tool and offsets are called out

2. The spindle is started

3. X, Y and Z moves are present, in the correct order

4. There is a feedrate called out in the first feed move

 

This can all be done in less than 5 minutes, for the most part.

 

Dave