Need Help!- Fanuc custom Macro Question????

[ixoxi999]

The following is my Custom Macro program of my Takeda Drilling Center Fanuc 10m:

O9000(ATC CUSTOM MACRO)
#3003=1
IF[#1012EQ1]GOTO8
IF[#1013EQ1]GOTO8
IF[#1014EQ1]GOTO8
#101=#4003
#102=#4002
IF[#500NE0]GOTO1
WHILE[#1015EQ1]DO1
#3000=1(TOOL CLAMP ALARM)
END1
IF[#149NE0]GOTO1
#3000=2(T CODE ERROR/T0...T0)
N1IF[#500NE#149]GOTO2
#3003=0

M99
N2G80G49G40
IF[#149LE36]GOTO3
#3000=3(T CODE OVER DATA)
N3
IF[#1015NE0]GOTO4
T1
M90
M19
T2
N4G91G28Z0
T1
M19
IF[#500EQ0]GOTO5
G53G90G00X#[#500+500]Y0
G23
G53Z-95.45Y80.0
G53Y150.2
M91
#500=#149
#1=BCD[#149]
#1132=#1132OR63
#1132=#1132AND#1
#1115=1
G91G28Z0M92
IF[#149GT0]GOTO6
G28Y0M93
T2
G22
G#101
G#102
G61
#3003=0
#1115=0

M99
N5G91G28Y0
N6G23
G53G90G00X#[#149+500]Y150.2
T1
M91
N7G53Y150.2
G53Z-80.0M92
G53Z-95.45
M93
M90
G53Y80.0
T2
#500=#149
#1=BCD[#149]
#1132=#1132OR63
#1132=#1132AND#1
#1115=1
G91G28Z0Y0
G22
G#101
G#102
G61
N8#3003=0
#1115=0

M99

The tooling are placed along the x-axis. If I want to change the tool. The x-axis will move to the tool and clamp it into the spindle head.

If I want to change the tool, I command "Txx"(xx = tool number such as T01 is tool no. 1). And the program will excecute automatically.

My problem is I try to increase my memory by installing new ram into the motherboard. But I need to clear out all the memories including "Custom Macro Variable".

In the program, I can run it all, Clamp and Unclamp tooling and etc, the functions except,
"moving x-axis"
IF[#500EQ0]GOTO5
G53G90G00X#[#500+500]Y0
The program don't know the value of #500 Variable.
N6G23
G53G90G00X#[#149+500]Y150.2
The program don't know where to collect the value of #149 Variable. I think this is the tool number.

I don't know this Macro Program is Macro B or not.
What can I do to excecute the x-axis moving to the right position to get the tooling.

Thanks guy for your help.

[angelw]

Set bit number 5 of parameter 0319 to 1. This will allow single step of every macro statement and therefore enable you to check the value of the Macro variables and the flow of the program in single block.

Variable #500 is a Common variable that retains it's value when power off. Check the value of #500 before you try a tool change. I haven't checked the logic of the program thoroughly, but #500 may have had a value preset by the OEM, and if you cleared the memory and didn't record the value, then this may be part of your problem. #500 needs to have a value other than Zero to get past the first error trap.

[ixoxi999]

Thank alot for your help man.
I can solve the problem.

[sinha_nsit]

Null variables:
Except for EQ and NE, a null variable is treated as 0 in arithmetic and conditional expressions.

[ggborgen]

Gentlemen,
In ixoxi999s macro it has this statement:
#1=BCD[#149]
My question is what is BCD? Thank You

[sinha_nsit]

BCD[_] changes its argument to BCD representation, interprets it in binary and outputs that value.
Let us say #149 contains 10 (in BCD[#149]).
BCD representation of 10 is 0001 0000.
The binary interpretation of 00010000 is 16.
So, 16 is output. Thus, BCD[10] = 16.

BCD and BIN functions are used in association with system variables for input/output interface signals.

For more information, read the attachment.

Sinha

[stevo1]

Originally Posted by ixoxi999 Thank alot for your help man. I can solve the problem.

So what was the solution to the problem?? It may help others with similar problems.

With a quick glance at your code it appears that #500 is to be set to the current tool that is in the spindle. With this being cleared it got mugged up on you. Was that the solution?

Stevo

[triphataaa]

#500: the current tool in the spindle (1, 2, 3,...36)
#501: The position of the tool 1 (A)
#502: The position of the tool 2 (A+B); B:distance between two tool
#503: The position of the tool 3 (A+2B)
#504: The position of the tool 4 (A+3B)
...
...
#536:The position of the tool 36 (A+35B)
triphat-tp co., ltd; triphat.com@gmail.com

O9000(ATC CUSTOM MACRO)
#3003=1
IF[#1012EQ1]GOTO8
IF[#1013EQ1]GOTO8
IF[#1014EQ1]GOTO8
#101=#4003
#102=#4002
IF[#500NE0]GOTO1
WHILE[#1015EQ1]DO1
#3000=1(TOOL CLAMP ALARM)
END1
IF[#149NE0]GOTO1
#3000=2(T CODE ERROR/T0...T0)
N1IF[#500NE#149]GOTO2
#3003=0

M99
N2G80G49G40
IF[#149LE36]GOTO3
#3000=3(T CODE OVER DATA)
N3
IF[#1015NE0]GOTO4
T1
M90
M19
T2
N4G91G28Z0
T1
M19
IF[#500EQ0]GOTO5
G53G90G00X#[#500+500]Y0
G23
G53Z-95.45Y80.0
G53Y150.2
M91
#500=#149
#1=BCD[#149]
#1132=#1132OR63
#1132=#1132AND#1
#1115=1
G91G28Z0M92
IF[#149GT0]GOTO6
G28Y0M93
T2
G22
G#101
G#102
G61
#3003=0
#1115=0

M99
N5G91G28Y0
N6G23
G53G90G00X#[#149+500]Y150.2
T1
M91
N7G53Y150.2
G53Z-80.0M92
G53Z-95.45
M93
M90
G53Y80.0
T2
#500=#149
#1=BCD[#149]
#1132=#1132OR63
#1132=#1132AND#1
#1115=1
G91G28Z0Y0
G22
G#101
G#102
G61
N8#3003=0
#1115=0

M99

The tooling are placed along the x-axis. If I want to change the tool. The x-axis will move to the tool and clamp it into the spindle head.

If I want to change the tool, I command "Txx"(xx = tool number such as T01 is tool no. 1). And the program will excecute automatically.

My problem is I try to increase my memory by installing new ram into the motherboard. But I need to clear out all the memories including "Custom Macro Variable".

In the program, I can run it all, Clamp and Unclamp tooling and etc, the functions except,
"moving x-axis"
IF[#500EQ0]GOTO5
G53G90G00X#[#500+500]Y0
The program don't know the value of #500 Variable.
N6G23
G53G90G00X#[#149+500]Y150.2
The program don't know where to collect the value of #149 Variable. I think this is the tool number.

I don't know this Macro Program is Macro B or not.
What can I do to excecute the x-axis moving to the right position to get the tooling.

Thanks guy for your help.[/QUOTE]

[stevo1]

Your program states that #500 is suppose to be the current tool in the spindle so set #500 via MDI equal to the current tool in the spindle.

#149 is probably being set via T() command thru a parameter setting which also calls program 9000. Make sure you have that parameter set. It is different depending on which model Fanuc control you are using. Since you did not tell us which control you are using we cannot tell you which parameter to set. You can also test this by programming a T() command and then checking parameter #149 and it should be set to your modal T().

FYI it is macroB that it is coded to.

It will also help in the future to start a new thread related to your problem instead of posting in one that is over a year old and not related at all to your issue.

Stevo

[fordav11]

AND post that new thread in the Macro forum
Parametric Programing - CNCzone.com-The Largest Machinist Community on the net!