[inthezone]

I'm not sure if this is an error in my software, or my Fanuc Controller...

When I am going in for a tool change, the code issues the T command with specified tool number. I am having to manually stop the program, and turn off the spindle to change the tool. If I wasn't watching the program closely, the program would simply continue on its happy way with the wrong tool. Very dangerous.

I am used to having the program stop the machine, and turn off the spindle for a tool change, and then having to press "cycle-start" in order for it to continue.

Is this something that has to be programmed into the controller, or is it something I can issue up in my code?

[Mitsui Seiki]

Post an example of the program.It makes it easier to see what's wrong.

[Al_The_Man]

Sounds like the PMC is not programmed to recognizing the T code, normally it is done to do the change automatically or if a manual tool change machine, then a stop is issued with a message and then wait for cycle start.
If it was originally programmed for automatic tool changer then there may be a sensor malfunction etc.
Al.

[inthezone]

%
:Microscope Switch-out
(8-2-2007)
N25G00G17G40G49G80
N30G30G91Z0
N35T2M6
N40G00G54G90X18.62435Y8.1577S3000M03
N45G43H2Z-9.5
N50Z-9.5558
N55G01Z-9.6458F9.0
N60X18.80185Z-9.6605
N65X18.62435Z-9.6753
N70X18.80185Z-9.69
N75X18.62435Z-9.7047
N80X18.80185Z-9.7195
N85X18.62435Z-9.7342
N90X18.80185Z-9.749
N95X18.62435Z-9.7637
N100X18.80185Z-9.7784
N105X18.62435Z-9.7932
N110X18.80185Z-9.8079
N115X18.62435Z-9.8226
N120X18.80185Z-9.8374
N125X18.62435Z-9.8521
N130X18.80185Z-9.8669
N135X18.62435Z-9.8816
N140X18.80185Z-9.8963
N145X18.62435Z-9.9111
N150X18.80185Z-9.9258
N155X18.7186F18.0
N160G03X18.7186Y8.1577I-0.0055J0.F12.6
N165G02X18.76023Y8.1577I0.0208J0.F18.0
N170G03X18.80185Y8.1577I0.0208J0.F12.6
N175X18.80185Y8.1577I-0.0887J0.
N180G01X18.81377Y8.20651F15.0
N185G03X18.7893Y8.2504I-0.0681J-0.0092F7.5
N190X18.7893Y8.2504I-0.0762J-0.0927
N195X18.69572Y8.27644I-0.0762J-0.0927
N200X18.6521Y8.25149I0.01J-0.068
N205G01X18.6371Y8.20353F15.0
N210G00Z-9.5
N215X19.45661Y9.11689
N220Z-9.5558
N225G01Z-9.6458F5.0
N230G02X19.28586Y8.93536Z-9.6639I-0.7435J0.5283
N235G03X19.45661Y9.11689Z-9.682I-0.5728J0.7098
N240G02X19.28586Y8.93536Z-9.7002I-0.7435J0.5283
N245G03X19.45661Y9.11689Z-9.7183I-0.5728J0.7098
N250G02X19.28586Y8.93536Z-9.7364I-0.7435J0.5283
N255G03X19.45661Y9.11689Z-9.7546I-0.5728J0.7098
N260G02X19.28586Y8.93536Z-9.7727I-0.7435J0.5283
N265G03X19.45661Y9.11689Z-9.7908I-0.5728J0.7098
N270G02X18.96673Y8.76907I-0.7435J0.5283F10.0
N275X18.45947Y8.76907I-0.2536J0.0887
N280X17.96959Y9.11689I0.2536J0.8761
N285X17.68746Y9.39339I0.0821J0.3659
N290X19.73874Y9.39339I1.0256J0.2518
N295X19.45661Y9.11689I-0.3642J0.0894
N300X19.28586Y8.93536Z-9.8077I-0.7435J0.5283F5.0
N305G03X19.45661Y9.11689Z-9.8245I-0.5728J0.7098
N310G02X19.28586Y8.93536Z-9.8414I-0.7435J0.5283
N315G03X19.45661Y9.11689Z-9.8583I-0.5728J0.7098
N320G02X19.28586Y8.93536Z-9.8752I-0.7435J0.5283
N325G03X19.45661Y9.11689Z-9.892I-0.5728J0.7098
N330G02X19.28586Y8.93536Z-9.9089I-0.7435J0.5283
N335G03X19.45661Y9.11689Z-9.9258I-0.5728J0.7098
N340G02X18.96673Y8.76907I-0.7435J0.5283F10.0
N345X18.45947Y8.76907I-0.2536J0.0887
N350X17.96959Y9.11689I0.2536J0.8761
N355X17.68746Y9.39339I0.0821J0.3659
N360X19.73874Y9.39339I1.0256J0.2518
N365X19.45661Y9.11689I-0.3642J0.0894
N370G00Z-9.5
N375X19.6331Y6.6702
N380Z-9.5558
N385G01Z-9.6458F5.0
N390G02X19.59934Y6.42327Z-9.6639I-0.92J0.
N395G03X19.6331Y6.6702Z-9.682I-0.8862J0.2469
N400G02X19.59934Y6.42327Z-9.7002I-0.92J0.
N405G03X19.6331Y6.6702Z-9.7183I-0.8862J0.2469
N410G02X19.59934Y6.42327Z-9.7364I-0.92J0.
N415G03X19.6331Y6.6702Z-9.7546I-0.8862J0.2469
N420G02X19.59934Y6.42327Z-9.7727I-0.92J0.
N425G03X19.6331Y6.6702Z-9.7908I-0.8862J0.2469
N430G02X19.6331Y6.6702I-0.92J0.F10.0
N435X19.59934Y6.42327Z-9.8077I-0.92J0.F5.0
N440G03X19.6331Y6.6702Z-9.8245I-0.8862J0.2469
N445G02X19.59934Y6.42327Z-9.8414I-0.92J0.
N450G03X19.6331Y6.6702Z-9.8583I-0.8862J0.2469
N455G02X19.59934Y6.42327Z-9.8752I-0.92J0.
N460G03X19.6331Y6.6702Z-9.892I-0.8862J0.2469
N465G02X19.59934Y6.42327Z-9.9089I-0.92J0.
N470G03X19.6331Y6.6702Z-9.9258I-0.8862J0.2469
N475G02X19.6331Y6.6702I-0.92J0.F10.0
N480G00Z-9.5
N485G30G91Z0M09
N490G49G90
N495M01
N500T5M06
N505G00G54X18.7131Y9.6452S401M03
N510G43H5Z-9.5
N515Z-9.5558
N520G01Z-9.6458F1.4
N525X19.4631Z-9.7758
N530X18.7131Z-9.9058
N535X19.5192F2.8
N540G02X17.907Y9.6452I-0.8061J0.
N545G00Z-9.5
N550G30G91Z0M09
N555G49G90
N560M01
N565T3M06
N570G00G54X18.7131Y8.1577S305M03
N575G43H3Z-9.5
N580Z-9.5558
N585G85R-9.5558Z-9.9758F9.1
N590G80
N595Z-9.5
N600G30G91Z0M09
N605G49G90
N610M01
N615T2M06
N620G00G54X18.36282Y11.1684S3000M03
N625G43H2Z-9.5
N630Z-9.5558
N635G01Z-9.6458F5.0
N640X18.60789Y11.11895Z-9.6639
N645X18.36282Y11.1684Z-9.682
N650X18.60789Y11.11895Z-9.7002
N655X18.36282Y11.1684Z-9.7183
N660X18.60789Y11.11895Z-9.7364
N665X18.36282Y11.1684Z-9.7546
N670X18.60789Y11.11895Z-9.7727
N675X18.36282Y11.1684Z-9.7908
N680X18.72586Y11.09514F10.0
N685G02X20.1631Y9.6452I-0.0128J-1.4499
N690G01Y6.6702
N695G02X18.72586Y5.22026I-1.45J0.
N700G01X18.36282Y5.147
N705X18.60789Y5.19645Z-9.8077F5.0
N710X18.36282Y5.147Z-9.8245
N715X18.60789Y5.19645Z-9.8414
N720X18.36282Y5.147Z-9.8583
N725X18.60789Y5.19645Z-9.8752
N730X18.36282Y5.147Z-9.892
N735X18.60789Y5.19645Z-9.9089
N740X18.36282Y5.147Z-9.9258
N745X18.72586Y5.22026F10.0
N750G03X20.1631Y6.6702I-0.0128J1.4499
N755G01Y9.6452
N760G03X18.72586Y11.09514I-1.45J0.
N765G01X18.36282Y11.1684
N770G00Z-9.5
N775G54S2500
N780F4.2
N785X18.0881Y5.36181
N790Z-9.5558
N795G01Z-9.6458F4.2
N800G02X17.8729Y5.48844Z-9.6639I0.625J1.3084
N805G03X18.0881Y5.36181Z-9.682I0.8402J1.1818
N810G02X17.8729Y5.48844Z-9.7002I0.625J1.3084
N815G03X18.0881Y5.36181Z-9.7183I0.8402J1.1818
N820G02X17.8729Y5.48844Z-9.7364I0.625J1.3084
N825G03X18.0881Y5.36181Z-9.7545I0.8402J1.1818
N830G02X17.8729Y5.48844Z-9.7727I0.625J1.3084
N835G03X18.0881Y5.36181Z-9.7908I0.8402J1.1818
N840G02X17.2631Y6.6702I0.625J1.3084F8.4
N845G01Y9.6452
N850G02X18.0881Y10.95359I1.45J0.
N855G03X17.8729Y10.82696Z-9.8077I0.625J-1.3084F4.2
N860G02X18.0881Y10.95359Z-9.8245I0.8402J-1.1818
N865G03X17.8729Y10.82696Z-9.8414I0.625J-1.3084
N870G02X18.0881Y10.95359Z-9.8583I0.8402J-1.1818
N875G03X17.8729Y10.82696Z-9.8752I0.625J-1.3084
N880G02X18.0881Y10.95359Z-9.892I0.8402J-1.1818
N885G03X17.8729Y10.82696Z-9.9089I0.625J-1.3084
N890G02X18.0881Y10.95359Z-9.9258I0.8402J-1.1818
N895G03X17.2631Y9.6452I0.625J-1.3084F8.4
N900G01Y6.6702
N905G03X18.0881Y5.36181I1.45J0.
N910G00Z-9.5
N915G0G91G28Z0M09
N920G49G90
N925M30
%

[Mitsui Seiki]

N470G03X19.6331Y6.6702Z-9.9258I-0.8862J0.2469
N475G02X19.6331Y6.6702I-0.92J0.F10.0
N480G00Z-9.5
N485G30G91Z0M09
N490G49G90
N495M01
N500T5M06
N505G00G54X18.7131Y9.6452S401M03
N510G43H5Z-9.5
N515Z-9.5558

So when it reach the part of the program marked red ,it just continues with the tool it has in the spindle?

[inthezone]

This bridgeport series II is manual tool change only. Lemme guess, programming the PMC to stop the spindle and program during a tool change is a pain?

[inthezone]

Mitsui Seiki, yeah it just continues, no pause or anything!

[Mitsui Seiki]

The M06 is usually a subprogram(macro),depending on what Fanuc control you have, that includes spindle stop/spindle orientation.Do you still have that?

[Mitsui Seiki]

Use "Optional stop" and run tool change using "Single block" and see what happens.

[Al_The_Man]

M,S,T codes are typically written in the PMC ladder, it is up to the MTB or OEM to include them, especially if the machine has a tool changer.
Al.

[CNCRim]

I guess you should check Optional Stop see if it is on or maybe the switch is loose, it is sound funny....... but maybe that's all it need and check machine parameter.

[codyst]

This bridgeport series II is manual tool change only. Lemme guess, programming the PMC to stop the spindle and program during a tool change is a pain?

You could do it a couple of different ways. 1. Create a macro as mitsui suggested, where when M6 is fired you can bring it into position for a tool change stop spindle and orient(if needed) and then issue an M0(as long as the parameters aren't set to reset/rewind off of an M0). And you may also have to re initalize any work coordinate offsets you are using depending on the parameter settings.

O9006 (M6 Sub);
G91G28Z0;
M5;
M19;
M00;
M99;

Or..2. As you mentioned edit the ladder logic to stop the spindle and program. This should be a relatively easy edit if you're comfortable with getting in and making changes. If you're not comfortable with it and decide to go this route send me a PM and I'd be glad to help.

[Switcher]

Some code, etc...

M5 (Spindle Stop)
M9 (Coolant Off)

(Might want to add a small amount of Dwell Time here)

Change Tool,etc...

M8 (Coolant On)
M3 (Spindle CW)

Some code, etc...

M3 - Spindle CW

M4 - Spindle CCW

M5 - Spindle Stop

M6 - Load Tool

M8 - Coolant On

M9 - Coolant Off

[dpuch]

Your problems is that typically machines without tool changers do not include the M06 in the ladder. Check your M code list to be sure.

You could do it a couple of different ways.

Codyst gave a great way to handle it, making the sub/macro and assigning it to M6 is my prefered way to handle it. Aditionally you can put that code in your programs instead of using the M6 as a macro/sub if that isn't supported. I also like to add intalizing tool length comp in my M6 macros, the example only stops the spindle for you.

Dale

[dpuch]

Also take a look at my previous post Sample Fanuc Tool change macro

Another post you might get something from A sample tool change macro

[inthezone]

Dale,

I am not quite sure how to look at my "M Code List" to check whether M06 is included in the ladder. What is the M Code list, and where is it located? I have lots of reference material on my controller, including the parameter manual but I am not quite sure what you mean.

If M6 is in fact not included in the ladder, I am guessing that I have to program a macro.

I looked at your post about a tool change macro for fanuc controllers because I have a Fanuc O-M controller on my bridgeport. That looks like what I probably need to do. In your post you mention that you have to "set parameter 6046 = 6" on your specific controller. My controller will obviously be different.

In my parameter manual there is this line:

-- 0040#5 ) TMCR 1 A T code is processed as the code of the tool function/code for calling 09000.

So I am guessing that I would have to set parameter 0040 = 5, and then write my tool change macro in program O9000.

Problem is I am not sure how to set parameter 0040 equal to 5.

In my parameter list,

NO. DATA
0040 00000000

Looking at the data, I can see that there are 8 zeros so I am assuming that this is an 8 bit system, and that setting 0040 = 5 would be like so:

NO. DATA
0040 00000101

But I am making a lot of assumptions here. I am not even sure if I am supposed to set it to 5.. anyone know whats going on here?

[dpuch]

For the M code list. Whoever put the control onto the machine should have provided some list of G and M codes that they enabled for the machine. Somewhere in the documentation they should list what is available for you to use.



For the macros stuff I'll suggest you read up on the macro programming section of your fanuc control. I'll try to give you the information it looks like your missing, but it will not be a thorough as the manual.


First lets clear up the parameter 0040#5
What they are talking about is parameter 40 bit 5 There are 8 bits in parameters like that. 0 thru 7 starting at the RIGHT and each bit can be a 0 or 1 This is called binary, and each bit is a virtual on/off switch for the control.

So the bit positions are:
76543210

You would need to set the on in the 5th position to 1 to turn that position on, or 0 to turn it off. LEAVE all the other bits as they were.

If 40 was 10010010 then you would change it to 10110010
There are of course parameters that aren't binary and take a normal number.


Now That said setting 40#5 to 1 will turn on using program 9000 whenever a T command is used. This is similar to using M6 as a macro, and in your case can be used in place of it if you want. You will not need a M6 at in in that case. In your main program you would only specify T7 without an M6 to change to tool 7

Regardless of the method of calling the tool change code, you still have to work out what you want it to do. Despite all the talk about macros and such, you should first make the machine do what you wish with code right in the program, then move that code to the macro to make it easier to use.

---------------------------
So lets take a few steps back and start with the basics. I think in an effort to make your life easier, the suggestions of making the tool change a macro has made it harder. At a tool change you want to move the spindle to a safe point, stop the spindle and coolant, and stop the program so a manual tool change can be performed. codyst gave you a sub program that will do all that. In your program posted before replace your tool changes (M01 tool number and M06) with

G91G28Z0;
M5;
M19;
M00;

You shouldn't NEED anything more. Make sure that works for what you want. If so, perhaps just leave it at that.