Need Help!- need help in tool measuring !!

[ahmed4040]

Dear All,

i face the following problem in measuring face mill in my TAKUMI CNC machining center

the control is Fanuc 0-imc

problem description :

when i try to measure an end mill i write in MDI the following command,

G65 P 9954 T1;

while G65 : macro call
P 9954 : is macro program number
T1 : tool number 1

till now i have no problem, the problem is in measuring face mill tools which have multi insert.

when i write in MDI the previous command, the inserts of the face mill does not touch the "tool length measuring device" .

i must stop the machine during measuring cycle and move X axis by Manual Pulse generator to make the inser touch the "tool length measuring device"

i need the command by which i can measure the face mill tools with an automatic cycle.

is the problem clear ??

if any one can help me it will be very good.

Note : attached here the macro program if any one want to check it

[stevo1]

I add the shift in the macro program for tools that need to be offset. Do you keep your tool radius in the control for these types of tools? I set mine in the offset radius column. Now depending on how your tool touch pad is set up or how much clearance you have on the sides will dictate which direction you want to shift the axis the radius of the tool. Mine works best coming Y negative the radius of the tool.

Your position to the offset pad is done in program 9954 so this is where we will add a variable to adjust that amount. Lets use #537 to capture your tool radius and wear. I don’t have a Oi manual with me at the moment so I am not 100% positive if it uses the same variables as my machine for radius(#2400 and wear(#2600). Lets also say that you have a 1.5” radius tool.


O9954(AUTOTOOLVER2.1)
#537=#[2400+#20]+#[2600+#20]---will gather the radius and wear of the tool being called. (#537=1.5)
#595=#4001
#596=#4003
G91G28Z0
M05
M09
IF[#20EQ#0]GOTO26
#27=FIX[#20](TOOL)
#594=1
T[#27]
G91G28Z0
N1
G90G80G40
#4=#5021-#5041(XABSPOS)
#5=#5022-#5042(YABSPOS)
#6=#5023-#5043(ZABSPOS)
M35
#600=250.(MAXTOOLLENGTH)
#601=60.
#28=#521+#600-#6
G0X[#523-#4]Y[#524-#5]
IF[#537EQ0]GOTO2----will skip the Y movement if no radius is set
G91Y-#537----incremental move the radius of the tool
#3006=1(ALIGN TOOTH TO PROBE)---not needed but will stop and give a message so you can rotate tool if needed
N2G90---back to absolute
G31Z#28F3000
IF[ABS[#5063-#28]GT.05]GOTO24
#28=#521+#601-#6
...
...

Now I don’t know what all of your other variables are set to or what program 9899 does from program 9954 so you have to make sure this does not affect any other aspects of the program.

I add the #3006=1 message because not all of our tools will align a tooth to the touch probe. Once aligned just push cycle start. If you find they always align then you can build the #534 into your Y[#524-#5] line and remove everything else. That way it will move if it reads a radius and will stay 0 if it does not.

Stevo

[GPena]

This is usually a machine tool buider issue, why don't you try to contact them, I had something similar with a Chevelir VMC and they solved the problem quickly.

GP.

[ahmed4040]

i could not know the variable number responsible for tool radius and wear.

my control is fanuc 0imc

anyone can help me !!

[stevo1]

I am not sure if I am 100% correct but digging through some old notes try #13000 for the geometry and #12000 for the wear if #2400 & #2600 do not work for you.

#537=#[13000+#20]+#[12000+#20]

Stevo

Edit: I see that if the number of available offsets is less then 200 then you should be able to use the #2001 thru #2400.

[ahmed4040]

thanks Stevo for your care

but

what is #20 for ??

thanks

[stevo1]

Ok #20 is your T value when you program a G65P9954T1 (now #20=1). Now we can plug this into the equation replacing the #20. #537=#[13000+1]+#[12000+1]. Which is actually #537=#13001+#12001

The way the variables work is #13001 is for tool 1, #13002 is for tool 2 etc. So the above equation will get the tool radius of #13001 and add it with the wear of #12001 for a total radius of tool 1. Now if you program G65P9954T7 then #20=7 and is used in the equation to gather the info from those variables pertaining to tool 7.

This way you are always gathering the data of the acutal tool you are offsetting.

Does that make more sense to you?

Stevo

[ahmed4040]

yes Stevo,

i'm now understand what do you mean.

and also if you have all macro description for fanuc 0imc(Local, System and common), kindly send it to me

my email is : ahmedibrahem@hotmail.com

i will try this steps and tell you the news.

also please add me in your messenger in order to easy chatting (if you want of course)

any way i appreciate your effort a lot

thank you very much

[ahmed4040]

sorry forgot one question,

for #537 shall i use this variable or i can use another one ?? such #538 or any other one ??

thank you

[stevo1]

#537 or #538 ou can use any variable that you want to. You just have to make sure that it is not being used with some other program.

As to the list of variables most of them should be in your operator/programming manual. The tool variables are listed under the custom macro section. Do you have your manuals?

As to the specifics of your input/ouput variables #1000's and #1100's most of these are set up and will vary based on the MTB. You should have a MTB manual that specifies what each on is.

Stevo

[ahmed4040]

Stevo,

i have the operator manual and i know it's supposed that it contain variable list

but unfortunately, the most of variable is not listed in details.

i will try to get this manual. also i will search for #537 to see if it's belong any other operation

thanks a lot for your great help

[stevo1]

If it is the Fanuc manual it is not going to give great detail into the meaning of your system variables. This manual usually just describes the tool, workoffsets things like that. The MTB manual should give you more details of these. I apologize I don’t have a lot of data on the Oi control.

Stevo

Edit: If you find that #537 is being used for something you can use any of #500-#999 if you have that many activated. You also have #100-#199 if you want to use them.