Programming/Using tool length

[Fudd]

I have set the tool length in the table. After a tool change T01 M6 in the next line I set the offset by H1 to use the length offset in the table for tool #1. When the machine runs this line it moves to Z 0.0. Do I need to specify a Z setting after the H word in the same line? Like N100 H1 Z0.5
It looks like that is what they show in some examples in the book. By not specifying a Z setting is the machine assuming Z0.0?

Thanks,

Scott

[nervis1]

OH man, had the same problem myself, crashed once because of it. Right after the program started the first thing it did was head for the table and bury my 1/2 roughing mill up into the holder. Luckily I hadn't set the setscrew into the flat because it was a test run...just in case. Also ran at 25% feed and rapid.

I put a z5.0 after the G43 in my post per the advice of the guys on the Onecnc board. My machine was going rapid to z0 before putting the height offset into effect. That worked fine. At least untill I use a 6" tool. I should change it to z10.0 now that I think about it.

[mtlmnchr]

How about putting your G43 on the line as follows ?

T1M6
G43H1Z5.M8

now your tool is 5 inches above your part, worse case scenario, your machine does not have enough Z stroke above part and will alarm, But no Z- crashes unless tool length is set improperly.

[Neal]

The tool length offset represents the distance from the tool tip when the tool is at tool change position and the Z zero position of your part.
If you simple apply the "H" code it will place the tool tip at Z zero of your part. I.E. the tool will touching the part. Instead program something like: N4 H1 Z.1 M8
This will place the tool .100" above the top of your part and over the lap the "pump up" time for your coolant to get flowing before the tool starts cutting.

Neal

[Fudd]

OK guys. That works. I do alot of small parts and use multiple vises with multiple parts in each. I have been using G92 to set my X and Y 0's then using g52 to offset to each part. Is this the best way to do that. By the way I am using subroutines for the milling steps. I then use g52 x0 y0 to clear before a tool change.

Thanks,

Scott

[Scott_bob]

IMO,

I don't like to use G92 at all...
Do you run your Fadal in format 1?

I prefer to use format 2 at the behavior is more predictable. For instance, I only want the CNC to do exactly as I program it to do. When in format 1, the CNC always wants to start from the set home position, so if it is not there when you start, it goes there 1st. I hate that!
Sometimes, when doing a simple operation I may just want to run one little cut then move out of the way enough to change parts, then start from there again. In format 1, the CNC will always go home 1st, this really bugs me.

I find the G54 or E1, thru G59 or E5 coordinate offsets much more accurate than using the G92.
I always prefer to have an absolute X, Y and Z position to work from relative to the machine base coordinate system (Cold Start Position).
Then if any shifting is needed I perfer to use one of the other offsets to "operate on", then when I want to go back to the original offset position I just overwrite the "operating coordinate" with the original coordinate which never changes. Also I like to always use G90, although G91 or incemental programs work fine, I think staying in absolute is just more accurate especially when using cutter compensation...

If you want an example let me know, I'll document...

Regards,

[Fudd]

I am using Format 2. I have started using the fixture offsets and do like that way better. I am always in absolute coor. I am learning the Fadal on my own and the help here is great.

Thanks,

Scott

[HuFlungDung]

Originally posted by nervis1 OH man, had the same problem myself, crashed once because of it. Right after the program started the first thing it did was head for the table and bury my 1/2 roughing mill up into the holder. Luckily I hadn't set the setscrew into the flat because it was a test run...just in case. Also ran at 25% feed and rapid. I put a z5.0 after the G43 in my post per the advice of the guys on the Onecnc board. My machine was going rapid to z0 before putting the height offset into effect. That worked fine. At least untill I use a 6" tool. I should change it to z10.0 now that I think about it.

Since reading guys advice now and then to avoid using G92, I have been slowly weaning myself off it. So now I work in G54 for a typical single part setup. But, my Shadow controller also has this problem with moving to Z0 whenever a tool length offset is called. Since I usually desire a Rapid plane of Z1, this looks (and is) dumb to see the tool moving all the way to Z0 and then back up to Z1 on its first programmed move. Instead of using a default of Z0 in the G54 offset, I use Z1 in all of my work coordinate offset tables, as a basic starting value. I always call the G54 before the tool length offset. This means when the tool length offset is executed, the movement is to Z1. not Z0. It's one way to deal with ancient controllers.