Restarting a Drip Feed via RS232

[Rocko1]

I was curious about a setting on my Haas. We currently will drip feed via a rs232 cable to our 98 VF3 for programs larger than the 1 meg on our control and have not had a issue yet on 4meg or smaller files yet. What am wondering is if we break a tool or some other mishap half way through the program, can we just replace the tool and offset the replacement tool and have it in the spindle. Making sure it is recognized as the current tool in the spindle of course. Then edit the program code deleting all the lines up to a point before the breakage and start drip feeding and restarting from there. I typically on our milltronics will of course find a nice x y and z retract code line and start there for gouging safety for when the machine moves to restart. Is this the proper method with a Haas also?
Also I notice my machine has the setting #36 PROGRAM RESTART as ON. Will this cause me a problem doing the above or does it only affect programs residing on the machines memory. Thanks

[gar]

071025-1513 EST USA

Rocko1:

I have not tried PROGRAM RESTART on a drip feed, and therefore I do not know if it will function or have problems.

Your approach of removing un-needed code would be my suggested method. What your need to do here is include all your startup code at the beginning of the shortened file. I might do a dummy tool change to any tool that was not the one your are going to use. Do nothing with this dummy tool. Then select the working tool that will be used at the restart point and all its parameters. Probably leave in some of the code just before your actual needed restart point.

The restarting point must be determined by any special problems like moving into an undercut.

.

[gar]

071025-1832 EST USA

Rocko1:

I am now at the shop and looking in the HAAS manual and I can not find any means that would allow you to do Program Restart in DNC mode.

Besides correct setup of setting 36 you have to scroll (move) the CURSOR to your start point. It is pretty clear that you can not do this in drip mode. I can find no indication of a special code to be inserted into the program, or a means to specify a specific line number for the Restart Point.

.

[uperez]

If you have a communication software like multi-dnc, you can restart anywhere in the program in dnc mode. All you have to do is create a safe start block where your start up codes are written (you can copy/paste your program heading) then just specify which block number to jump after sending the safe start block, no special settings on the machine just run it like your regular routine. You'll just have to be sure of the plane selection you're using but if your post processor outputs plane selection in every tool change then you'll have no problem. I used to run programs so long that it runs for more than 3 days and loops the block number from 1 to 12000 nearly 4 times. The only problem I had is when I restarted with a tool that uses G18 plane and since the previous tool uses the same plane, the post processor neither cancel it off to G17 nor re-call G18 on that tool, the plane selection in my program heading is G17 so it made a chamfer instead of a radius. The dang part costs $10,000 and my boss sure had a go with all of us in the shop and programming department.

[Rocko1]

Thanks to all on the info.