1. ## Parametric programming question.

Is there away in parametric programing to have the control ask the operator a question, have the operator input answer then pass that to the program as a variable?

Example.

Display this on the control. "What is the part number"
The operator then enters part number. "0469"
So that after that input variable #1 will be 0469

2. What control would you like this to happen on?

3. its a fanuc ot.

4. What you're asking can't be done on an OT, as is, since the operator would have to keypress over to the screen for variable input, cursor down to the proper variable, type the value and then press [INPUT].

• You could have your operator put the program number into a predetermined offset. Then have the program stop and display that number before it ran, and ask if that is correct, if it is the operator could just hit cycle start to contniue, if not stop and change it.

• Yeah since most of the operators have zero manufacturing experience. I can't go the parameter route I was thinking of some thing like this.

%
O0001
(Enter part number here)
#1=0469

Then use if then statements to set up the rest of the program based off that number. I think I can train the operator to drop to edit and just alter that one line. Now the only issue I have is figuring out a way to get the operator to remember to adjust the work shift on the few parts we have to. This program is to streamline a part family we have.

• Ok, stay with me here this is kind of hard to explain. What I'm saying is this, say you have five different programs and a fanuc control. First figure out what the variable is for say H1 ( the very first length offset ) I don't know what it is off the top of my head but it should be in your manual, we will say it is #2500 for know. Then write a main program with some logic like this in it.

IF [#2500EQ100] GO 100 (100 IS YOUR FIRST PART, PC 100)
IF [#2500EQ150] GO 150 (PC 150)
IF [#2500EQ200] GO 200 (PC 200)
IF [#2500EQ250] GO 250 (PC 250)
IF [#2500EQ300] GO 300 (PC 300)

N100 M98 PO100
AND SO ON, you can use what ever your part numbers are so it is not confusing. This way all your operator will need is to go to the offset page and fill in the first value. Then put a check, Like i mentioned in my other post, that will remind the operator to check the value. This may sound confusing, but I think it would be pretty simple to run, just one value to set.

• Ok I see what your saying. That would work better than them going into edit mode. I'll have to look that varible up in my manual. Now what this program will be for is making different types of nipples out of schedule 40 pipe. There are threads of different lengths in the part family. Some of the longer threads lengths we have to hang the part further out of the chuck. We use the workshift to do this. Can I put a check in the program to see if they adjusted the workshift, if the part number they entered requires it. If they haven't it throws an alarm?

• 070930-1131 EST USA

chrisryn:

I have no real experience with Fanuc, but I have with HAAS and it is similar.

Assuming you have MACROS, then consider:

A main O# program for each part, and one surbroutine for your part program. The operator picks the main program desired, then hits START.

Example:

%
O0100
(part numb 91308-07-251)
M00
G65 P1000 and your parameters that define the part
M30
%

%
O0101
(part numb 91308-08-263)
M00
G65 P1000 and your parameters that define the part
M30
%

%
O0102
(part numb 91308-11-373)
M00
G65 P1000 and your parameters that define the part
M30
%

%
O1000
G54 (Or whatever coordinate system you want.)

(Start up stuff.)

(Your cutting program.) (Uses the passed parameters to define the part.)

M99
%

Consider G52 as a means to offset from your base G5x coordinate system. The value for G52 can be passed in as one of the parameters.

.

• What control are you working with? I don't know if you can have it alarm out if they don't change the work shift, but you can have it stop and tell them to check. Is it the same amount of shift every time for each part, if it is you can preload those shifts in the sub programs and have the control call it up when the program runs.

• Its a fanuc 0T. All of our tool geometry is from the face of the chuck. We use the work shift to shift the program zero(datum) to were the end of the part will be. So depending on the length of the threads is were the work shift will be. So I guess yes would be the answer to your question. If there making 3" long threads the work shift will be the same every time they make 3" threads.

• 071001-0633 EST USA

chrisryn:

Set your tools however you want. Then adjust G54 Z so that when G54 is active that Z=0 is the face of the chuck. From your description I believe this is your current method. Now if you want your working coordinate system to have Z=0 at 3" away from the chuck face, then insert the instruction
G52 Z 3.0
After this instruction and until changed your working coordinate system is changed by the content of the G52 registers.

In Fanuc at power on, program start, and various other changes of operating mode the G52 regsisters are all zeroed.

The G52 values are added to whatever the current active G5x is. However, you may need a sign reversal in the G52 Z command. Experiment to determine the sign to use in the G52 Z command, and do it with G54 set away from the face of the chuck.

You can put the offset value in the G52 command with a variable. Such as
G52 Z #500
Prior to the G52 you can insert a test on #500 that would prevent being closer than some desired value from the face of the chuck.

.

• Page 1 of 2 12 Last