Tool Change Command

[outofsquare]

Hi Bill,

I have the control manual in front of me & it has a section with Macro in it so will read through it, I am going back to the machine shop tonight to give it another play, as the replies have given me some ideas to try.

Will check out what appears in the screen as per your suggestions

Thank heaps Bill

Tony

[outofsquare]

Thanks Bill, worked out that there was a command file missing in Macro, the manufacturer emailed me the missing program & the tool changer works, but with one problem, it knows where tool 1 in the carousel is but then if I select T2 it will go to T9 slot, its working backwards, I reference the carousel & it goes through its paces & stops at T1.

But cant seem to get the mill to simply be able to put a tool back into a slot without going and picking another up, got me stumped.

Cheers

Tony

[txcncman]

A T0 should force the machine to put a tool away and leave the spindle empty. Well, does on some machines anyway.

[outofsquare]

Hi all,

Now I have got the mill workimg perfecty in MDI mode for tool change, it will do exactly what I call up, BUT Lol, when I download NC file it will not carry out the tool change, it will skip right pass the command being T3 M06 for example, I have tried leaving the M06 out and still will not carry out the tool change, any comments or hints would ber much appreciated.

Cheers

Tony

[angelw]

Hi all,

Now I have got the mill workimg perfecty in MDI mode for tool change, it will do exactly what I call up, BUT Lol, when I download NC file it will not carry out the tool change, it will skip right pass the command being T3 M06 for example, I have tried leaving the M06 out and still will not carry out the tool change, any comments or hints would ber much appreciated.

Cheers

Tony

Hi Tony,

What command do you actually execute in MDI?
Is it, for example, T3 M06;, as one block?

Post a copy of your Tool Change Macro, and a copy of your program containing a Tool Change

Regards,

Bill

[outofsquare]

Hi Bill,

Okay here is a NC file first, and below this is what the manufaturer got me to load on my controler to get the tool changer working & having the tool changer working in the right direction instead of backwards, thanks Bill hope this is the info your looking for

%
O0000
N10 (PART - )
N20 (NOTES - NONE)
N30 G90 G00 G40 G80
N40 G91 G28 Z0
N50 (10 MM CARBIDE END MILL)
N60 T1 M06
N70 G131
N80 G00 G90 G54 X0. Y0. S8785 M03
N90 G43 Z5. H1 M08
N100 G00 X0. Y0. Z5.
N110 Z1.
N120 G01 Z-5. F158.
N130 Y100. F316.
N140 X100.
N150 Y0.
N160 X0.
N170 G00 Z5.
N180 G130
N190 M09
N200 M05
N210 (END TOOL)
N220 G00 Z50.
N230 G130
N240 G91 G28 Z0
N250 G90 M5
N260 M09
N270 M30
%

Here is what they got me to dowload on the controller

#500=#1000*1
#501=#1001*2
#502=#1002*4
#503=#1003*8
#504=#500+#501+#502+#503
G04 X0.2
M05
IF[#1015EQ1]GOTO300 ;жTָ뵱ǰߺǷ
IF[#1013EQ1]GOTO300 ;T00T11-T20ָ
M19 ;ᶨλ
G04 X0.2
G53 G90 G00 Z-96.332 ;Zᵽ
M80 ;
M82 ;ɵ
G04 X0.2
G53 G00 Z1
G4X0.2
IF[#1014EQ1]GOTO10
G12 R29 L6 Q#504 P0 ;ת
GOTO N50
N10
G12 R29 L7 Q#504 P10 ;ת
N50
G04 X0.2
G53 G00 Z-96.332 ;Zᵽ
M85 ;
G04 X0.2
M81 ;
M05
N300
M84
M99

[outofsquare]

Forgot to answer all your questions Bill, yes in MDI I input in one block T1 M06

[angelw]

Forgot to answer all your questions Bill, yes in MDI I input in one block T1 M06

Hi Tony,

Its incongruous that the Tool Change works correctly via MDI and not via a program if the Macro program is being called by an M06 or T code.

I don't know what number parameter it is in your control, but as your control is so close to a Fanuc, there should be a parameter that can be set so that the control will halt after each Macro statement block when the control is in Single Block Mode. If you can't find this parameter, place an End Of Block on a line by itself after every Macro Statement in the Tool Change Macro. An EOB is treated as an NC Word, and therefore the control will halt when in Single Block Mode.

Create a short program containing a Tool Change and run the program in Single Block Mode. When the Tool Change Macro program is called, you will be able to step through the program to determine the control flow, and why nothing seems to happen when the Tool Change is executed from within a Program. Do the same in MDI Mode to see the difference in behavior of the Macro program.

To get the value, or status of a System Variable before a Macro Statement containing the variable executes, you can temporarily modify the Macro Program to read the variable value into a viewable variable such as a Local variable. For example, to get the status of Interface Signal Variable #1015 and #1013 before the Macro Statement executes, include the following code:

#1=#1015;
;
#2=#1013;
;
IF[#1015EQ1]GOTO300 ;жTָ뵱ǰߺǷ
IF[#1013EQ1]GOTO300 ;T00T11-T20ָ

In Single Block, you will be able to look up the value of #1 and #2 in the Macro Variable page before the two conditional blocks execute.

I assume that the code in Red is not actually included in the program loaded in your control?

Its an interesting Tool Change Macro. The following gets a Decimal value of a 4 bit binary number based on the Interface Signal Variable status, and then uses the number contained in #504 in
G12 R29 L7 Q#504 P10. Do you have an explanation of G12?

Regards,

Bill

#500=#1000*1
#501=#1001*2
#502=#1002*4
#503=#1003*8
#504=#500+#501+#502+#503

[Technical Ted]

Hi all,

Now I have got the mill workimg perfecty in MDI mode for tool change, it will do exactly what I call up, BUT Lol, when I download NC file it will not carry out the tool change, it will skip right pass the command being T3 M06 for example, I have tried leaving the M06 out and still will not carry out the tool change, any comments or hints would ber much appreciated.

Cheers

Tony

Sounds like the control thinks it already has T1. If you single block thru the program what tool# is the control showing before & after it runs line N60?

[outofsquare]

Just wanted to inform all who have been following my delema with tool changing command when using a NC file.

Well it turns out that the reason why the controller was responding to a tool change command in the MDI screen if I manually inputed, say T4 M06 command, was because I had the macro file in reagrds to the tool changer saved in the root directory.

But what I was doing when it came to the NC file was that I was placing the USB in the controller & then simply opened the file I wanted, & the controller would open the file & simply stated press cycle start, and this is what I was doing, the NC file would execute perfectly but without any tool change when promted (lol well not so perferctly).

Then tried somthing a little diffrent by simply opening the NC file on the USB & I saved the NC file to the root directory first & then opend the NC file from the root directory, pressed cycle start & bingo the tool change command executed when prompted, so problem ended up being that the tool change Macro was saved in the root directory, & as I was simply opening up the NC file straight of the USB it had no Macro to goto when prompted for a tool change to be carried out.

I will try saving the Macro file for the tool changer in the USB, this may then allow me to carry out a tool change if I dont actually save the NC file to my root directory.

A huge thankyou to all who posted their suggestions as putting them all togheter had ended up turning a light globe in my skull, and Bill thankyou so much for going out your way to help me yesterday, your a champion!

Cheers

Tony

[angelw]

Just wanted to inform all who have been following my delema with tool changing command when using a NC file.

Well it turns out that the reason why the controller was responding to a tool change command in the MDI screen if I manually inputed, say T4 M06 command, was because I had the macro file in reagrds to the tool changer saved in the root directory.

But what I was doing when it came to the NC file was that I was placing the USB in the controller & then simply opened the file I wanted, & the controller would open the file & simply stated press cycle start, and this is what I was doing, the NC file would execute perfectly but without any tool change when promted (lol well not so perferctly).

Then tried somthing a little diffrent by simply opening the NC file on the USB & I saved the NC file to the root directory first & then opend the NC file from the root directory, pressed cycle start & bingo the tool change command executed when prompted, so problem ended up being that the tool change Macro was saved in the root directory, & as I was simply opening up the NC file straight of the USB it had no Macro to goto when prompted for a tool change to be carried out.

I will try saving the Macro file for the tool changer in the USB, this may then allow me to carry out a tool change if I dont actually save the NC file to my root directory.

A huge thankyou to all who posted their suggestions as putting them all togheter had ended up turning a light globe in my skull, and Bill thankyou so much for going out your way to help me yesterday, your a champion!

Cheers

Tony

Your welcome Tony.

Just to expand a little on the above for those who have a similar control. Although its purported to be a clone of a Fanuc control, there are differences that aren't well documented in the Control Manual.

With a Fanuc control, Sub Programs can be called with an M code by setting the numeric value of the M code in a parameter that corresponds to a particular program number. With Tony's control, M01 through to M09 default to call a program having the program numbers 9006 through to 9009 respectively, if they exist. If they don't exist, the M code is treated as a normal M code and no alarm is raised. Because Tony was effectively running the program from a USB stick, the control would look to the Root Directory of the current drive, see no O9006 program when M06 was executed, and carry on after the M finish signal was confirmed.

Those following this thread will note that there is no M6 in the Tool Change Macro Tony Posted. This is because just about all the work for the Tool Change is done by the Macro Program. Normally M6 will be decoded in the PLC program, that is, Carousel in, Tool unclamp ect, and M codes for the various moves are often provided by the MTB so as to get the Tool Changer back home when problems occur. With this control, the M06 is broken down to all the sub M codes to carry out the various Tool Change functions in the Tool Change Macro.

Regards,

Bill