[fomaz]

I am asking several questions since I do not have experience with Fanuc.
I have a machine center, where I am able to jog and to zero the machine. I was unable to do anything else.
My next "jump" is to try that the machine would move following some gcode in MDI mode (appers to be the most basic). I have read the manual, but I must be missing something. What did I did:

1) Power, and zero all axis
2) I went to MDI mode, and typed G00 X100
3) Pressed INPUT
4) This line was entered to the text box (as in the picture)
5) Pressed START, but nothing happens (using the interlock switch, since I did not mounted the door of the machine). I have notice that the led behind the start stays on for one brief instant, then goes off. Machine does not move.

I have read another program in machine memory, and I notice that all the lines end with ";" I do not know how to input this or to go to a new line in MDI mode. I know, those are basic questions, but I need to ask them.

I have attached a picture, that is the state before and after I press START. No alarm is displayed or anything else.

Any ideia or sugestion is very welcome.
Thank you

[stevo1]

Yes you need the end of block(EOB) “;” in the line of your code. The control looks like a 18 series. You should have a button labeled EOB.

There is no way to get to the next line. The lines will be split up based on the EOB. So just keep typing. Example is if you type at the bottom of the screen. G0X100;Y50;Z100; and when you press input it will enter the code into the control as:
G0X100;
Y50;
Z100;
And it will execute these lines one at a time.

Stevo

[Boots]

You are trying to tell the machine to move but you do not say where to move to and from where to move from. A G91 is required to move incrimentally (from where it is) and a G90 tells it to move 100 in the X from your Absolute home position.
Try this instead. G0 G91 X100;
OR if you have a work offset for G54 position then use this code.
GO G90 G54 X100 Y0;
Be sure your manual feed over rides are not shut off.

[stevo1]

No extra code is needed. G0X100 should work just fine. If you take a look through your parameter book it will tell you the settings for which codes are the default codes. Some G-code lists in the back of the manuals will tell you the same thing shaded black as the designated default code within the group.

There is no code to deactivate G90 and G91 at the same time. So if it is not programmed in the code it is whichever active/default (typically G90) is. If you go to the program check screen it will tell you which codes are active. This goes the same for the work coordinates. G54 is typically default so it is always active after reset or program end as is G90. So if these are the defaults on your control then a G0X100 will move the machine in G90 mode in relation to the setting in G54 coordinates even though you did not program them.

One thing you might want to do is put a decimal in the X100. Just in case your parameters are set up as conventional input instead of calculator input. If that is the case and you want to change it then it is parameter 3401.0 =0for conventional and =1 for calculator. I set all my machines to calculator. By the look of your CRT in the picture I ass u me that it is a 18series fanuc control and that is the parameter for that control.

Stevo

[fomaz]

Thank you for the replays,

about the line input, yes with the EOB key, now I can input lines in a good manner. About the modal mode, I am currently in G90 (in the screen we can see the current mode). Tested with the point and without the point in the coordinate, and result was the same. About the G54 it is set to X0 Y0 Z0.

Now (after the code that I have inputed) when I press start cycle, the start cycle led goes on and stays on, and I can see that the running program timer counts (in the picture 1min 37sec), it really appears that the machine is processing something. Another thing that I have notice is that the when start is pressed, the line showing currently being processed, passes from the program name "O0000" to the 1st line of code and stays there (see picture).
I do not have the feedrate in zero, I have it in 100%.
Controller is 21i-m model A.

I feel that I am close, too close
Once again any sugestion is welcome.
Filipe - Portugal

[beege]

Do you have a "Machine Lock" inhibiting axis movement? Rapid override set to 0? (not the same as "feedrate override")

[fomaz]

Rapid override set to 0?

I do not think so, but I have tested with G1 X100 F1000, and the result was the same, this is no movement, so I do not belive that rapid overdrive is set to zero, or if it is, that is not the problem for now.

About "Machine Lock". There is no key on machine about this, so I suspect that you are refering to some parameter or logic of the machine, I do not quite know were to look, but I took a picture of the diagnostic screen during the execution of the program that does not move. Were we can see that the machine is in "motion" and that interlock start lock is also true, I do not know if I should have true here or false...

Keep giving something to lookfor, that I will !

[stevo1]

This can also be caused by not having all of the axis referenced. Are you positive that you have ALL of them referenced? What kind of model/make machine is this?

I think Beege was referring to “machine lock” which is usually a hard key on the control for running a program without physical movement. I ass u med this as well but the display numbers should be moving. If you press the softkey “ALL” when you are in the program check screen it should display the distance to go. Is there a value in there?

You have no doors open correct?

Stevo

[JimBoyce]

Try this and let us know what happens

S500 M3;
M8;

[kevinl2375]

You also may need to call up a tool first..
I would try moving all axis away from there home position manually.
and then:

G0 G28 U0.0 W0.0 Y0.0 T0:
G0 G54 T0101 ( this being whatever tool you want)

[dcoupar]

You also may need to call up a tool first..
I would try moving all axis away from there home position manually.
and then:

G0 G28 U0.0 W0.0 Y0.0 T0:
G0 G54 T0101 ( this being whatever tool you want)

This looks like lathe stuff. He's got a machining center, and this will more than likely cause an alarm.

[James L]

Just as you may or may not have to put a decimal after X100, you may also have to put in in the feedrate. On my machines a feedrate without a decimal will run but it takes forever. Try F20. or something. If your machines behaves like mine f20. will move many times faster than f1000 without the decimal. Also, have you tried jogging your machine to a random location and type G28X0.Y0.; and run that?

[fomaz]

Just to tell to everbody that I will try all solutions from all posts today after I have the workshop closed and will inform on the results. I would like to say thank you to all that are trying to help.
Filipe

[fomaz]

I have managed to have more progress, now I can G0 !! but not G1. In order of reply, and bassicaly the order of the tests I made, where it goes:

stevo1: I am sure that I have all 3 axis referenced. I press zero axis, the machine moves from current position to zero position. All green leds (zero leds) appear on axis X,Y,Z. Pressing the ALL, I can see that the distance to go is present and correct. The door is closed. For double checking, when door is open I cannot jog, with door closed I can jog, so I belive it is not a door issue. Machine is a vertical machine center, Kira VT40A.

JimBoyce: Trying to go with the spindle it works! Nice to see something working. Spindle rotates ok, so the program runs. Thanks !

kevinl2375: I did not used the code you typed, but I have tryed to issue a G0 X100 T0 after I homed the machine (I think it is simillar to what you meant). Result was the same, this is, no movement. Next I tryed:
S200 M3;
G28 X0;

Pressed start, and machine turned spindle and moved! This was very nice, but no more, it goes to zero, nothing more, even if I had more code.

James L: G28X0.Y0. This runs both axis to the home position. (better !!)


Honestly i do not know what I have made, I tryed so many things on the MDI, but now I am able to move the machine in fast mode (G0). I do not need to home the machine. The command that works are like G0 X100.; If I type G0 X100; machine goes to X0.1.

Now the odd thing; G1 this happens the same than before: No movement, no error. Machine just stands. I have tryed:

G0 X100. ; (This is OK - now)
G1 X200. F200. ; (This makes the counter of the machine running forever and does not move)

Note that if I home the machine using "home axis" or using "G28 X0 Y0 Z0" in code the result is the same. In G1 no movement... I am starting to like better all my Mach3 machines.
Filipe


One again thank you all,
Filipe

[stevo1]

Filipe,
Ok you are making progress. If you do not like having to insert the decimal X100. then change the parameter I gave you earlier so it is in calculator method. I like it this way because if a decimal is forgotten in say a 5” clearance move and it only goes .5!!!

As to the G1 it could be that either you need to have the spindle rotating or you could be in G95(feed per rev) and the spindle is not going. Try this.

M3S200
G94(feed per min.)
G1X100.F200.
M30

Stevo

[fomaz]

stevo

You are right. I need the spindle rotating! Machine will only move with spindle rotating even if I have a G94 code. Do not undestand quite well why, but I will go to the parameters one by one trying to see what is going on. But it is a relif knowing that the machine will eventually work... When bought it was not clear that it will. Also the parameter 3401 now is in calculator mode (better for me).

Thank you all for the suport. I will now try to create a program and save it, and after that will try to transfer code with a PC. What software is needed on the PC side to transfer code to the machine? Any sugestion?

Filipe

[sinha_nsit]

stevo

... Machine will only move with spindle rotating even if I have a G94 code ...

... difficult to believe! Are you sure it is like this only.

PCMCIA flash memory card is a convenient way for transferring programs to/from CNC.

[fomaz]

Where goes 2 pictures showing just what I have said before. It will only move with the spindle ON. Can this be related to the ladder logic? This machine was on a factory doing quite large series of pieces (I think only part of each piece). I recall to see on part count 5000 as the target value.

About the PCMCIA, if this is the most commun used method I will used it to. But a serial communication would also be fine.

[sinha_nsit]

... Can this be related to the ladder logic? ...

I believe so.

Once, on an emulated Fanuc, I needed to plot a 2D toolpath. I attached a spring loaded pen to the spindle, placed a paper on the machine bed, modified offset setting, and executed the program without M03. This would not be possible on your machine.

[stevo1]

Filipe,
That is weird that the spindle needs to be rotating. This is only in G1 mode correct? You don’t need it on for G0 moves do you? Yes it is probably related to way the ladder was written. I have never come across this before. It is not a crazy idea though. I suppose what would you need to be feeding on if the spindle is not rotating.

With your machine the PCMCIA card is convenient as Sinha suggested. However I think the most common is using the RS232 port. I have all my machines set up to the network thru RS232. There are a few things that you need to do to get this working. There is free software out there for communication or you can use the HyperTerminal on your computer. Do a search here it should come up with something. If you want to spend money I have had good success with Dostek software(contact info below). You could also PM Dan Fritz. He is the DNC guru here and has his own software and is always willing to lend a hand.

Dostek Incorporated
238 Westheights Drive
Kitchener, Ontario
Canada N2N 1j9
Tel (519) 742-5721
Fax (519) 741-8669
www.dostek.com
Ask for Doug Struthers

Good luck,
Stevo