Parameter Setting For Tool Length Value

MacDaddy · Feb 12, 2018

I think I know everything but in case I don't - somewhere in my convoluted mind I am sure that when G43 and an H value are programmed, somewhere in the parameters it inputs the length value of the associated tool so calculations can be made for movements.
Is this a correct - and would anyone no the parameter number? I have looked through a couple of manuals I have but no luck.
My dilemma is I use 3 tools to do machining on parts on a Mori Seiki with a pallet change system.
Each tool does 2 parts and then times out and moves on to the next - all not relevant.
At the end of the cycle before tool changing I have a sub program to verify tool length on a Blum laser and if it is off because of chipping or breakage then the machine alarms out.
The sub program needs the tool 'H' value to conduct its measuring cycle.
I need to either find the parameter value so I can put in H#5200 (example) so it will use whichever tool is in - or i will need to right a macro and use 3 sub programs for the different tools - which then I will probably need to find the variable for the 'T' value.
As an aside in case anyone has similar machine - to call up the tools with an M06 I use T9901 (01 is the group it selects from in the tool management) and where G43 is I need to put H9999.
I tried putting H9999 in the sub program but it says "Variable out of Range".
Any help appreciated.

sinha · Feb 12, 2018

Did you try H99?
Is it Fanuc?
Check what you have in variable #4111.

huskermcdoogle · Feb 12, 2018

Depending on integration, there isn't necessarily a readily available variable to read the current length from.

Well when using tool life like that there are many ways to skin that cat. I have seen Mori's setup to take the current tool H HW D DW values and populate them into offset register 99 ( or whatever number you want to set it as) upon tool change (regardless of group code and normal tool management), then everything in the program uses H99 or D99, as they will have the current spindle tool values in them. This is another layer you could add to what are already doing. I don't know how the blum laser macros are setup, but are you looking to put the current length value in as an agruement for H, or are you looking to know which H register to read.

Anyway if this is a Fanuc, #8409 is the current tool H compensation number selected by tool life, at which point you can use that to read the length in the table by using #2200 or #11000 variables (compensation memory C parameter 6000 bit 3 = 0) So your H code in the macro call to measure the length would read H#[2200+#8409]. The 2200 is the base variable for length geometry, this might be different on your machine if it has a mits control or a different offset system is being used..

Hope that helps point you in the right direction.

Get us some info on what machine model and control you have and we can drill it down a little further if you still need help.

MacDaddy · Feb 12, 2018

huskermcdoogle said:
Depending on integration, there isn't necessarily a readily available variable to read the current length from.

Well when using tool life like that there are many ways to skin that cat. I have seen Mori's setup to take the current tool H HW D DW values and populate them into offset register 99 ( or whatever number you want to set it as) upon tool change (regardless of group code and normal tool management), then everything in the program uses H99 or D99, as they will have the current spindle tool values in them. This is another layer you could add to what are already doing. I don't know how the blum laser macros are setup, but are you looking to put the current length value in as an agruement for H, or are you looking to know which H register to read.

Anyway if this is a Fanuc, #8409 is the current tool H compensation number selected by tool life, at which point you can use that to read the length in the table by using #2200 or #11000 variables (compensation memory C parameter 6000 bit 3 = 0) So your H code in the macro call to measure the length would read H#[2200+#8409]. The 2200 is the base variable for length geometry, this might be different on your machine if it has a mits control or a different offset system is being used..

Hope that helps point you in the right direction.

Get us some info on what machine model and control you have and we can drill it down a little further if you still need help.

Excellent info. i will check into this when I get a sec.
Machine Mori Seiki NMV3000
Control MSX-711IV
The drives are Fanuc which is why I assumed the control was Fanuc based as well - plus other variables like #5221, 5222, 5223 etc to set G54 xyzbc positions

huskermcdoogle · Feb 12, 2018

Well up until now you gave us no indication it was a fanuc. Now that we know what we know, what I described should do exactly as you need. All of that info is in the Fanuc Operators Manual, if you don't have one, request one.

Search

Largest Manufacturing Technology Community on the Web

Search

Parameter Setting For Tool Length Value

MacDaddy

Plastic

sinha

Titanium

huskermcdoogle

Stainless

MacDaddy

Plastic

huskermcdoogle

Stainless

Similar threads