Need Help!- cant load macro on fanuc om

[positiverake]

Having trouble loading a macro program from dnc, I can load programs with no problem but with a macro it will only take the (man readables) is there a parameter to allow the control to read macro programs. the machine has the macro op. turned on, I would type it in but the key pad is limited no brackets ect. its a takisawa mill with a fanuc om. thanks

[angelw]

Originally Posted by positiverake Having trouble loading a macro program from dnc, I can load programs with no problem but with a macro it will only take the (man readables) is there a parameter to allow the control to read macro programs. the machine has the macro op. turned on, I would type it in but the key pad is limited no brackets ect. its a takisawa mill with a fanuc om. thanks

When you refer to DNC, are you drip feeding the program to the control, or do you simply mean that you are loading the program form a PC to the control’s memory?

If drip feeding, you will have trouble with most Macro statements, unless the statement is simply calling a Macro Program that is already stored in memory. For example, you can’t use a program loop in the program being fed to the machine, because once the code is executed, its discarded by the control. Accordingly, no block to loop back to.

Are you sure the control has the User Macro option? The majority of O series controls only had User Macro A. The A version used codes for all of the conditional and math functions, while the B series (the more user friendly of the two) used statements similar to that of BASIC.

If your control does have the User Macro option and if downloading the program from PC to control memory, then there should be no issue with this. I suspect that the problem may be with a filtering feature of the PC software being used for the file transfer. Its quite common to have settings available in the software to ignore certain characters.

You can determine if the control has User Macro by pressing the Offset button and then navigate through the various pages. If the control is equipped with User Macro you will see MACO as a soft key at the bottom of the screen.

Regards,

Bill

[stevo1]

Bill,
I agree. I know that some will not allow editing of the macros/man readables at the control but have not seen any that will not allow man readables

Stevo

[positiverake]

Thanks guys, yes just trying to load a program from a pc, the control alarms out with ps 004, the control has the 100-500 variables is this macro B?, im using predator software for bob cad to up/down load, the control takes the man readbles? think its coming from the pc software? must be a setting, dont know were to start?

[angelw]

Originally Posted by positiverake Thanks guys, yes just trying to load a program from a pc, the control alarms out with ps 004, the control has the 100-500 variables is this macro B?, im using predator software for bob cad to up/down load, the control takes the man readbles? think its coming from the pc software? must be a setting, dont know were to start?

When viewing the Macro Variable page, try paging Up and Down with the Page Navigation keys to see if you have other pages of variables. User Macro B series has Local Variables that start at #1, and I'm almost certain that Series A does also, but its been a long time since I visited that version.

I’m away from my office until next week and accordingly, can’t look this error code up. Please post the description associated with that error code; you will find it in error list in the Fanuc manual.

As stated in my earlier post, series A User Macro uses codes for the Macro commands, whereas Series B uses syntax similar to Basic and Pascal. See if you’re able to download a short program containing the following:

If the # and = symbols are available via the key pad, you will also be able to enter and execute #100=1 in MDI mode, but that is unlikely with the key pad you described earlier.

%
O0001
#100=1
M00
M30
%
If the program loads OK and appear as above in the control, run it. If the machine errors when you run the program, you won’t have Macro B. If no error, check the value of Macro Variable 100 in the Macro Variable registry. If its value is 1 then you have Macro B for sure.


Regards,

Bill

[positiverake]

Ill try that tomorrow, thanks

[Dan Fritz]

Is your DNC software sending EIA code? If it's sending ISO (ASCII), then the macro characters like "#" are just normal ASCII characters. If your DNC software is sending EIA, then those characters are not even defined. There are parameters in the control to define them, but chances are those parameters are not set.

The control should accept either EIA or ISO tape code. You should use ISO if you can.

[positiverake]

This is the alarm Im getting (004 ps alarm a numeral or the sighn "-" was input with out an address at the beginning of the block) ? what do you think? it wont take even the # sign from the pc. any help? the pc software is sending ISO. do you know what paramaters to change so the control can define the code anyway? or should I look at the pc side a bit deeper, sorry I never seen this problem before. like I said the control has the macro soft key and the 100-500 variables? one other thing(not to open up pandoras box) but if I hold down any key on the control and then the key with the ; / # i can get the # on the screen but it will have the 1st key before it? say I hold the M down while I press the ;/# key it will look like this on the screen M# not sure what this is all about. thanks again for the help

[Dan Fritz]

The control is not reading the program correctly. I would suspect that there is something wrong on the DNC side. You might have a typo in the program if it always stops at the same spot, but if it's happening randomly, I would suspect a mis-setting on the DNC side.

[angelw]

Originally Posted by positiverake This is the alarm Im getting (004 ps alarm a numeral or the sighn "-" was input with out an address at the beginning of the block) ? what do you think? it wont take even the # sign from the pc. any help? the pc software is sending ISO. do you know what paramaters to change so the control can define the code anyway? or should I look at the pc side a bit deeper, sorry I never seen this problem before. like I said the control has the macro soft key and the 100-500 variables? one other thing(not to open up pandoras box) but if I hold down any key on the control and then the key with the ; / # i can get the # on the screen but it will have the 1st key before it? say I hold the M down while I press the ;/# key it will look like this on the screen M# not sure what this is all about. thanks again for the help

You will find that the one key is the input for a number of characters, for example, the key that you have identified as ;/# . You don't have to hold down another key to access the other characters, just press the same key repeatedly and you will cycle through the various characters associated with that key. Once the desired character has been obtained it can be registered in the program by using the Insert key.

Write a short program containing #1=100, or #100=100 and run the program. Look for the variable you used in your program in the Macro Variable register; you should find that its value is 100.

Regards,

Bill

[angelw]

Originally Posted by positiverake This is the alarm Im getting (004 ps alarm a numeral or the sighn "-" was input with out an address at the beginning of the block) ? what do you think? it wont take even the # sign from the pc. any help? the pc software is sending ISO. do you know what paramaters to change so the control can define the code anyway? or should I look at the pc side a bit deeper, sorry I never seen this problem before. like I said the control has the macro soft key and the 100-500 variables? one other thing(not to open up pandoras box) but if I hold down any key on the control and then the key with the ; / # i can get the # on the screen but it will have the 1st key before it? say I hold the M down while I press the ;/# key it will look like this on the screen M# not sure what this is all about. thanks again for the help

You can only set the number of Stop Bits, Baud Rate, the type of External device you wish to communicate with and whether the code format is EIA or ISO. The Data Bits should be set to 2. Check on the Setting Page of your control; you will see there if the control is set to EIA or ISO.

If any data at all is able to be transfered, then its unlikely to be a cable problem, but just to be sure, the cable configuration for Xon Xoff handshaking is as follows:

Machine side---------------------------------PC Side
DB25 Male Connector----------------DB9 Female-----------DB25 Female
1-------Shield Ground-------------Not Connected--------Not Connected
2--------------------------------------2----------------------3
3--------------------------------------3----------------------2
4
| Bridged
5

6
|
8 All Bridged
|
20

7--------------------------------------5----------------------7

The settings in the PC software sould be as follows:
1. Handsahke Method = Xon Xoff (software handshaking)
2. Baud Rate = Same as Control Setting. Setting 10 at the Control is 4800 baud, so set 4800 at PC if 10 is used. Setting 11 = 9600 baud rate
3. Data Bits = 7
4. Stop Bits = 2
5. Parity Bit = Even

Regards,

Bill

[hitachibos]

to get rid of your 004 alarm you need to have "custom macro B' option custome macro A will not allow # symbols or math to be done.