[fahed]

I am using a CNC Lathe with a bar feeder attachment and the cycle time for a part is 1minute 33 seconds, My problem is its a mass production and when I place M30 at the end of the program I have to press "CYCLE START" after a component falls off, I loose some time there since time is very important,

If I replace M30 with M99, the program runs over and over again after parting, but the problem here is when I press the "POS" button on the controller, Part Count = 0, Cycle time = How much time the machine has run after I hit the "CYCLE START",

I need the program to run without hitting the cycle start button over and over again and see how many parts have fallen and also the cycle time for each part not the whole session.

[Ashish B]

I doubt that you cannot get individual cycle time, because cycle time counter is restarted only when u command M30 & as in your case u command M99...So can't get the individual cycle time.

For the Part Count, follow the instructions -



Before pressing cycle start, turn the Part Counter to 0


In your program command,


#xxxx = #xxxx+1;
M99;

(Where xxxx is the Parameter number which traces the Part Count...)

(Consult your Machine Dealer to know about the parameter which stores PART COUNT).

[fahed]

I use a Galaxy Midas 0 machine, In the Parameters I could see in Help of the mahcine its shows 6700~, But when I used 6700, I get a error, illegal parameter used.

[Ashish B]

U have to ask to machine dealer...Or do post a new thread asking about parameter number which traces part count in forum of


"Paramteric programming".


But i suggest to ask to machine dealer...

Ash

According to my knowledge, the program mentioned is right...

Ash

[beege]

I use macro variables as a part counter. How you would use it depends upon what control you are using. Mine is a Fanuc 10TF. At the end of the program, just before the M99, I have a "#549=#549+1. I can adjust that number while in MDI mode if necessary, like when first setting up a job,I can adjust to zero, or subtract bad cycles. Do you know which control you have, and whether you have Macro B installed?

[fahed]

I use a "FANUC 0i mate-TC", Could you help me in detail how do you set that parameter in MDI mode. I have never used the MDI mode.

[Ashish B]

Simply Program the following code in MDI.


#xxxx = 0,

(where xxxx is Parameter which traces the Part count

[dertsap]

If I replace M30 with M99, the program runs over and over again after parting, but the problem here is when I press the "POS" button on the controller, Part Count = 0, Cycle time = How much time the machine has run after I hit the "CYCLE START",

.

setup so that your main program is a sub routine then loop it to the number of parts/bar

[fahed]

I called up the dealer, He gave me this code "M90" before m99, & this worked, Thanks all for your help.

[Ashish B]

Hey what's M90 ??

[fahed]

My Machine dealer says its a code to add 1 to the part counter, so if I put M90 10 times in my program, I would a part count of 10, Can you tell me what is Macro B and what is the advantage of it.

Thanks in Advance.

[beege]

M90 is a machine-builder added in feature not available on most makes of machines unless they too want to build in that M code. They would add it to the PLC side of the control. Don't expect to be able to use it on other makes of tools.

Macro B is a programming tool that allows you to have changeable parameters within your program. If you have a family of parts, for example, with different bore sizes, one program could be written that would suffice for all, with a simple change in the macro variable table that would modify what the program would do. There are conditional branch commands, calculating functions, I/O testing (if you know the address for that I/O). Counting is one of the simpler things you can do with Macro B. You could also set up the macro to stop the machine (M30) when a certain number of parts is reached. Powerful tool.

[Ashish B]

I am confused...Can u tell me what's the defination of M90 code. I am bit surpised that such code (of increasing Part count) do exist.




Macro programming is a gr8 tool. U can yourself create new canned cycles & u can really fulfill array of wonderful applications....But u need to have through knowledge of it before using. It is complicated to learn.

G-code programming is simple to learn & easy but to learn macro programming is really a tough task.

Ash

[fahed]

Beege & Ashish,

I appreciate all the effort you put into to help in this issue, As you suggest I would try and get some books on Macro Programming,

Best of Luck
Fahed

[Ashish B]

I wanted a M90 Code description. Can u please help

[fahed]

The dealer say its a code given for part count in Galaxy CNC machines, Did you try it too, What were the results ??

[PixMan]

This is very simple: That M90 is a custom M-code created by the machine builder. If you REALLY want to know what's in it, you can find out by unlocking the "parameter write enable" then look at the "9000 series" program written for the M90. To identify the program, find the M90 listed in the paramaters up around 6050-6059 (I think.)

I don't have my Fanuc manual for the 16i/160i/18i/180i/21i/210i here at home, it's in my toolbox at dad's shop. I'll be heading over there later today so I'll look up the paramter range for custom M-codes and their associated "9000" programs. Basically, a given parameter number is permanently associated with a "9000" program, you assign and M-code value to it, and write the 9000-series program you want. No different than creating a custom G-code. If you go to that range of parameters and look (no need to unlock the PWE to look BTW), you should see "90" next to one of the parameters. When I get my book, I can tell you which 9000-series program it runs. It'll be something like 9016, 9017, 9018 etc.

[PixMan]

OK, for you that have Fanuc 16i/16iS/160i/160iS, 18i/18iS/180i/180iS, and/or 21i/21iS/210i/210iS controls and want to know about parameters for user variables, custom G codes and custom M codes:

#6036 = Number of custom macro variables common to paths (100-199)
#6037 = Number of custom macro variables common to paths (500-599)

#6050 = G code that calls the custom macro of program number 9010
#6051 = G code that calls the custom macro of program number 9011
#6052 = G code that calls the custom macro of program number 9012
#6053 = G code that calls the custom macro of program number 9013
#6054 = G code that calls the custom macro of program number 9014
#6055 = G code that calls the custom macro of program number 9015
#6056 = G code that calls the custom macro of program number 9016
#6057 = G code that calls the custom macro of program number 9017
#6058 = G code that calls the custom macro of program number 9018
#6059 = G code that calls the custom macro of program number 9019

#6071 = M code that calls the custom macro of program number 9001
#6072 = M code that calls the custom macro of program number 9002
#6073 = M code that calls the custom macro of program number 9003
#6074 = M code that calls the custom macro of program number 9004
#6075 = M code that calls the custom macro of program number 9005
#6076 = M code that calls the custom macro of program number 9006
#6077 = M code that calls the custom macro of program number 9007
#6078 = M code that calls the custom macro of program number 9008
#6079 = M code that calls the custom macro of program number 9009

#6080 = M code that calls the custom macro of program number 9020
#6081 = M code that calls the custom macro of program number 9021
#6082 = M code that calls the custom macro of program number 9022
#6083 = M code that calls the custom macro of program number 9023
#6084 = M code that calls the custom macro of program number 9024
#6085 = M code that calls the custom macro of program number 9025
#6086 = M code that calls the custom macro of program number 9026
#6087 = M code that calls the custom macro of program number 9027
#6088 = M code that calls the custom macro of program number 9028
#6089 = M code that calls the custom macro of program number 9029

Look at those parameters and take note of which ones have numbers entered, and write down those that interest you. Now to see what commands any one of them actually executes, go to MDI mode. Find the "Settings" page, usually by hitting the "offset" button 2 or 3 times (depending upon if your machine shows both geometry and wear offsets or not.)

There will be one bit marked as "Parameter Write Enable". Change it from "0" to "1". An alarm will immediately come up, don't worry about it...yet. It won't reset as long as the "PWE" is unlocked.

BE CAREFUL! Enabling the "PWE" allows all kinds of bad things to happen if you accidentally change a previously-locked parameter or program while in this mode.

Now go to the "parameters" page by pressing the "system" key. Type in "3202" and search for it. Cursor over to Bit 4 (the 4th one over from the RIGHT.) It shold be labeled as "NE9". Change it from "0" to "1".

Next, go back to the settings page and change the "PWE" back to "0". Reset the alarm. Now is when you need to be extra careful not to change anything!

Select EDIT mode. You should now be able to see and edit the "9000 series" of programs. With the notes you wrote down about which 9000 series program you want to see code for, such that "M90" or any other G code or M code you don't recognize as standard Fanuc, you can call up that program as you would any other and see everything.

If you edit ANY machine manufacturer-written 9000 series program while "NE9" is unlocked, you risk both crashes and part programs that won't work. If you are very familiar with programming, you can use this information to create your own custom G and M codes. This can be very useful.

When you're done looking, be sure to go back to the "PWE" and enable it again. Go back to parameter 3202.4 and change the NE9 back to "0", reset the PWE to "0" and all should be good in this world again.

You're welcome.