What's new
What's new

Is starting in the middle of a program on Fanuc 0i really this f*%#king difficult?

While every program may have some differences, restarting a Fanuc on a machine that uses the T code to index the carousel can be tricky. On a Haas, M6T2 will load tool 2 into the spindle.

Completely logical.

On our old OKK M6T2 will load whatever happens to be in the magazine into the spindle and then indexes the carousel to T2. This can cause problems when restarting the machine if this fact isn't considered along with a safety block cancelling offsets, entering the correct fixture offset and so on.
 
Heidenhain lets you start anywhere anytime no matter what, kinda scary. Gotta watch out if you are using offsets or rotates
The Brother goes back and loads the previous tool, which is annoying but smart
All the ideas I have involve editing and if the OP doesn't know G code, he is going to be in trouble.
 
Is this enough?

N73 M1
N74 T1111
N75 G54
N76 M8
N77 G98
N78 G97 S760 M3
N79 G0 X0. Z0.6
N80 G0 Z0.2
N81 G83 X0. Z-0.7 F3.57
N82 G80
N83 Z0.6
N84 M9
N85 G28 U0.
N86 G28 W0.
No It's not. For one you have no tool length callout. And you should have a safety line at each tool change.
N1G17G80G40G90G49G0

Ok I'm thinking Mill. But Douglas is right. For a Lathe that is sufficient.

Even a Mid Tool restart can be done. But you should probably figure this out first.
 
No It's not. For one you have no tool length callout. And you should have a safety line at each tool change.
N1G17G80G40G90G49G0

Ok I'm thinking Mill. But Douglas is right. For a Lathe that is sufficient.

Even a Mid Tool restart can be done. But you should probably figure this out first.
I’ll have to sniff around the postprocessor and see if I can figure out how to add that
 
I put all the safety codes in a sub program and call it at the beginning of each tool.

N1 M98 P9000
T1 M6
G54...
.
.
.
N2 M98 P9000
T2 M6...

Then I commented out the stuff in the post and forced it to output M98 P9000.
 
What is your CAM system?
With any luck there is a tick box in your post dialogue box that allows you to add a "safe start" each tool or operation, that way you can just to any tool or op and it will repost the tool and work offsets as well as modal commands.
I don't think the Fanuc system is worse, I think so far you have just been very lucky with the Haas not crashing.
 
On a Haas, there is a setting for "Program Restart", which goes through the entire program until it gets to the line you want to start on, regardless of where it is. It reads all of the G00, G17, G41, D words, H words etc. so everything is in the right place before commencing the cut. IIRC, Fanuc had a "program restart" OPTION ($$$) that might do the same thing....
 
No It's not. For one you have no tool length callout. And you should have a safety line at each tool change.
N1G17G80G40G90G49G0

Ok I'm thinking Mill. But Douglas is right. For a Lathe that is sufficient.

Even a Mid Tool restart can be done. But you should probably figure this out first.
On a lathe, the T word is the tool call out for offsets, so he's safe.
 
  • Like
Reactions: VTM
The Fusion 360 post for DN mills has the option of putting in a forced tool change ahead of any operation you choose. If there's no tool to change, the machine just goes home and then back on its merry way, but importantly, it picks up a fresh set of offsets, modal setup etc.

I got bit on my DEM 4000 the other day when I tried to restart at an op with no tool change after the prior op. The restart did not pick up the Z offset. Fortunately, the toolholder was a small ER-16 what it ran into was soft aluminum at 25% rapid. Could have been a disaster.
 
While every program may have some differences, restarting a Fanuc on a machine that uses the T code to index the carousel can be tricky. On a Haas, M6T2 will load tool 2 into the spindle.

Completely logical.

On our old OKK M6T2 will load whatever happens to be in the magazine into the spindle and then indexes the carousel to T2. This can cause problems when restarting the machine if this fact isn't considered along with a safety block cancelling offsets, entering the correct fixture offset and so on.

Hello Jim,

That's a MTB's ineptness, not Fanuc. I have an old Mori with an Yasnac MX2 control that in standard form, raises an alarm if the Spindle Tool is called again in the program. Accordingly, saving a bit of time by loading the first operation tool in the spindle at the end of the program is not possible. Therefore, if any operation had to be run again, if the tool in the spindle was used in the operation that was to be repeated, the tool had to changed out of the spindle first.

I wrote a Tool Change Macro that saved the Spindle Tool in a Nonvolatile Variable (500 Series). In the Tool Change Macro the tool being called is compared with the Tool Number saved in the allocated Spindle Tool Variable and if the same, control exits the Tool Change Macro and returns to the Main Program, work perfectly. This is something that the MTB should have done within the control, for not all machines come with User Macro.

The system I have implemented in all my clients' shops, is that all tool operations that make up the whole program, can operate as stand alone programs. Its not often that the number of each tool will match the program sequence, that is, tool number one will be the first operation, tool number two the second operation and so on. Accordingly, in my opinion, its easier for an operator to remember the operation sequence, that is, first operation Spot Drill, second operation Tapping Size Drill, third operation Tap, rather than first operation T12, second operation T44, third operation T27 and so on. Therefore, I only have a Sequence number at the start of each Tool Operation, N1, N2, N3 for Op1, Op2, Op3 respectively. and if an operation has to be rerun an operation, they need only search for the Sequence Number that corresponds to the operation number.

To execute a restart part way through a particular Tool Operation, the operator first searches for Sequence Number of the operation to be restarted with the following:

1. N4 (for 4th operation)
then press the cursor down button. With a Fanuc control, this will work in either Edit, or Memory Mode.

2. With Single Block turned on, the program is stepped through until the tool has been called up and Workshift/Tool Offsets have been established.

3. Select Edit Mode and move the Curser to the block you wish to start at, ensuring that a Feed Rate has been read.

4. Select Auto Made and Press Cycle Start with the Feed Rate Override wound back to a minimum setting.

5. Check Distance To Go and once confident that the tool is proceeding to the correct location, switch out of Single Block Mode and set Feed Rate Override to its normal setting.

Regards,

Bill
 
Last edited:








 
Back
Top