[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 : [email protected]

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.

[ahmed4040]

Stevo,

i wil try to get the MTB manual, thanks anyway.

but i need to know the parameter which make the variable # 13000 appear.

i can show till # 999, i need to show #13000 to be sure that the value which i will put it in the offset table will be the same in #13000

thanks

[stevo1]

I am not 100% about the Oi control but I don’t think that you can view the #13000. Someone please correct me if I am wrong.

You can however get the value of #13000. If all you are trying to do is determine that these are the proper variables for the tool radius and wear all you have to do is program them into another variable that you can view. The way these settings go are:

#13001=tool 1
#13002=toot 2
Etc.

Now put a value in the offset page tool radius. Something odd like 1.4567. Now MDI program #100=#13001, go look at the value of #100 if it is set to 1.4567 then these are the proper variables. Also do the #12001. If these are not the ones try #2401 and #2601 as I had given before.

Stevo

[ahmed4040]

Dear Stevo,

thanks a lot for this idea

i have write in offset table in geometry page a value for tool raduis (25) mm

then

i have typed in MDI :

#100 = #13001;

so the value of #100 = 25
then repeated the same idea with #12001

i think you are right, we can not preview #13001 directly.

i will try the modified program you sent me the update you with the news.

thank you very much for your help

[ahmed4040]

Dear Stevo,

the problem have been solved :banana: (thank you), but i made a small edit in your modification.

my touch sensor diameter's is 20mm, so i don't want it to shift with tool less than or equal 20mm, i have made this by using IF #537 LE 20 GOTO N2.

and it working.

Now, if i want to make the spindle orient by a certain angle to measure each face mill insert... is it possible ??

i mean if i have 5 inserts face mill i will have to orient the spindle by 72 degree to measure each insert alone

thank you

[sinha_nsit]

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

This issue bothered me a lot a few months back when I saw different statements at different sources. Then I read somewhere that #13000 would be for geometry and #12000 for wear when parameter 6000#3 is 0. The geometry and wear offset numbers get interchanged when this parameter is set to 1.

[stevo1]

Ahmed,
i don't have anything with me right now. i am out of the country and this is the first chance i had to get back to the zone. i do not beieve that there is any way to orientate the spindle to a certian tooth unless your spindle can idex to a particular degree. IIRC most of the tools that you put in the spindle should line up at least 1 tooth at 12,3,6,or 9 o'clock so it would just be a matter of shifting your machine in the proper direction.

As i said i will take a look when i get back on Monday.

Stevo

[stevo1]

Ahmed,
No you will not be able to measure all of your inserts unless you set up the macro to stop after the first measurement then you manually rotate to the next tooth and repeat. But the only thing you can do with that is take the longest tooth and set that as your offset. There is no need to do this. Your face mill should run accurate from tooth to tooth so it should not matter what tooth you touch off. If you do have a problem then you need to check your machine or contact your tool rep for new or different tooling.

Stevo

[ahmed4040]

Dear Stevo,

welcome back to the zone

first of all than you very much for your great help, it really was helpful.

for spindle orientation problem, you are right, i will not be able to orient this face mill inserts automatically, it will be only manually.

again i would like to thank you very much for your care.

have a nice day