Fanuc 0i VMC - Set tool length automatically clears H+D wear parameter

[Newbeeee™]

Hi All,

On our VMC's, when we set a tool length (input C), it automatically clears the H wear value (which we like ).

But it doesn't clear the D wear (which we don't like).

So if we set the next job up and forget to manually clear the wear value, the part is wrong.

So does anyone know a parameter that automatically clears H+D wear values when setting the tool length?

Cheers

[Guest CNC Apps Guy 1]

Hi All,

On our VMC's, when we set a tool length (input C), it automatically clears the H wear value (which we like ).

But it doesn't clear the D wear (which we don't like).

So if we set the next job up and forget to manually clear the wear value, the part is wrong.

So does anyone know a parameter that automatically clears H+D wear values when setting the tool length?

Cheers

 

#10000(or #2000)+Tool Number = 0 (H Wear) Look for a line that contains

#11000(or #2200)+Tool Number = 0 (H Geometry)

#12000+Tool Number = 0 (D Wear)

#13000+Tool Number = 0 (D Geometry)

 

This will clear the offending offset completely (geometry and wear). There's not a single magic parameter that clears it AFAIK. You're going ot have to go into the MACRO call and find the line that references and clears them and add another line that clears the D stuff.

 

 

HTH

[Newbeeee™]

James,

We're setting the tool length manually onto a clock (DTI).

We're not using probing so there is no macro, or am I miss-understanding you?

 

I went through the big yellow book and couldn't find anything, but I suppose the question could be 'why have length offset clear diameter register?' because they are separate things. So I don't think there is a parameter, but I have our MTB looking at it...

Thanks

[Guest CNC Apps Guy 1]

Ahhhh. RIF (for me). AFAIK ther is no parameter that clears the D when you r press the INP. C.

 

I was thinking Tool Measurement System (laser/touch). SOrry.

[Newbeeee™]

Thanks for the reply

[Manuel0822]

As long as you do remove all tools from setup to setup, you can always hit the soft key under the screen for clear all, I think I remember you would press the right soft arrow once or twice once you are on the tool offsets screen and then it will show you the key Im talking about.Once you clear them all up you should be fine to start setting up the new tools offsets.

[Newbeeee™]

Thanks Manuel,

Yep - just seen that. Never even noticed it's there.

It works as you said - just have to remember to do it now LOL.

Cheers

[Matthew]

In the past I had a macro I would use to set the tool height. I would bring the tool down to the top of a '123' block, then go to program 08000 and press the start button. This would input the machine Z value plus 2.0" (a variable that was previously set and could be changed) into the height offset for that tool. This would effectively set the tool to the top of the table. Then it would retract the machine to the home position. I'm sure a macro like this could also be used to clear the D value at the same time.

 

Matt.

[huskermcdoogle]

In the past I had a macro I would use to set the tool height. I would bring the tool down to the top of a '123' block, then go to program 08000 and press the start button. This would input the machine Z value plus 2.0" (a variable that was previously set and could be changed) into the height offset for that tool. This would effectively set the tool to the top of the table. Then it would retract the machine to the home position. I'm sure a macro like this could also be used to clear the D value at the same time.

 

Matt.

 

 

I do something similar to this with the probe for picking up .5" dowel holes on fixtures on the fms. Move the probe to the dowel hole sitting flush with the face. Then the machine will probe the face next the hole followed by probing the hole and setting it to G54 for me to write down and G10 into a program.

[Tim Johnson]

Here's what we do to clear offsets...

 

%
O9026(M501 -- TOOL OFFSET REMOVAL PROGRAM)
(PARAMETER 6086)

(A = FIRST TOOL TO REMOVE, DEFAULTS TO 6)
(B = LAST TOOL TO REMOVE, DEFAULTS TO 200)

IF[#1EQ#0]THEN#1=6
IF[#2EQ#0]THEN#2=200

WHILE[#1LE#2]DO1
#3=10000+#1
#4=11000+#1
#5=12000+#1
#6=13000+#1
IF[#1EQ4]GOTO1
#[#3]=88.8888
#[#4]=0
#[#5]=0
#[#6]=0
N1
#1=#1+1
END1
M30
%

 

Note: the 88.8888 length eliminates the potential crash if a tool length is missed.

[Hitachi]

You can just add the command to the program #12001=0 etc. doesn't matter if you are using a probe or not