[DerHammer]

I'm in a jam, for the last week I've been trouble shooting my Fanuc om linking to my PC so, I finally got fed up and bought a rs232 tester to check the cable/connecters and its fine. The controller will send out accurately to my PC but It absolutely will not receive. The tester shows data making it to the serial port on the controller, but the "ZST" keeps flashing.. nothing shows up. Again, I can send to my PC, but I cant send to my CNC, so my questions are....

Can somebody tell me whats wrong, what do I do to fix it, and how much will it cost. What are my options? Any help is greatly appreciated.

[Al_The_Man]

What cable are you using, I prefer to use the 3 wire cable with the hardware handshake jumpered out.
For 25 pin it is 4-5 6-8-20
Just 2, 3 & 7 connected.
The 9 pin end is 7-8 6-1-4
and 2,3, & 5 connected.
Al.

[Dan Fritz]

What model Fanuc control is this?

[DerHammer]

I believe its all correct, The 232 tester shows data transmitted and received correctly "pins two and three depending on direction right?".

A tech at the DNC software company I'm using was helping me trouble shoot this over the phone and he confirmed that the cable appears to be working correctly also. The Controller will send the data, but not receive, almost like half the serial port on the NC is dead. I can double check, but it seems like it shouldn't be the cable/connectors if the data comes across the pc accurately.

I decided it was the NC port because I put the tester in between the cable and the controller right at the NC port on the controller and it does show data transfer right there when I transfer the file on the pc. Its like the controller is ignoring the feed.. But then again, Your Al the man, If totally open for suggestions if you have any! =) Thanks

[DerHammer]

forgot to mention that This is a Fanuc Om controller "Gno series by general numeric" on a Webb knee mill.

and for the cable, I'm using a 25 pin jumpered as Al suggested on the NC side. On the other side where the 9 pin connector is. Its another 25 pin where I believe pins "2" and "3" are crossed from the other end for handshaking. I have this converted down to a 9 pin via an adapter I bought from the electronics store so that it mates with my com port.

I also forgot to mention that I bought a 50 ft 25 to 25 pin straight through cable and a null modem full handshake adapter, which I haven't tried yet. I just haven't bothered because the current cable seems to be transferring data correctly I'm told.

[mdparlette]

These testers are notorius for saying one thing and and the opposite is happening. Unplug it. Your rs232 port is probably OK. For the sake of simplicity, is parameter 340 set to use 310,311,312,or 313? And are these parameters set correctly? It sounds to me, since you can download to the pc, parameter 341 is set correctly. but your communication program settings aren't jiving with parameter 340's requests.
I have found that with the OM, setting the comm settings at 4800,even,7bits, none(handshaking) works best. Using parameter 313.
Amada has a precise parameter setup page on their website, if needed.
Hope I'm not to far off base in understanding your needs.
Mitch

[Dan Fritz]

Look at parameter 002, bit #2 (the THIRD bit from the right). If it's a "1", set it to "0". Also set the same bit to "0" in parameter 012

The Fanuc 0MA and 0MB had both an RS232 serial port and an ASR43 Current-loop port (the blue plastic Honda plug). The ASR current-loop port is also serial, but it's a different type of signal designed for the old TeleType machines. Not many people use the ASR port, so Fanuc discontinued it in later models.

When you send a program, data always comes out BOTH ports simultaneously. When you receive a program, the Fanuc needs to know WHICH port it's suppose to listen to. This bit of parameters 002 and 012 determines which port is used when the Fanuc reads a program. A "0" is for the RS232 port, a "1" is for the ASR current-loop port.

Parameter 002 bit #2 is effective if the "I/O" bit on your first parameter screen is set to "0", and parameter 012 bit #2 is effective when the I/O bit is set to "1". I always set 002 and 012 the same just in case somebody changes that I/O bit by mistake.

[DerHammer]

Changed the third bit of parameter 12 to 0 and "presto"! here comes the data! I can't thank you guys enough for this. I had almost accepted the fact that the board had to be replaced! Again, if you guys were local.. I would buy you dinner because you just saved me allot of money. So thank you again, hopefully I can share the karma with some other poor noob like me who's struggling.

Now on to operation. Since I can now input my code from the pc, I'm wondering how to run the programs. I set it to auto, dry run, then cycle start but nothing seems to happen. I know this is a total noob question, but if somebody can explain to me how to set the positioning up to correspond with the cad/cam model.. that would be awesome. I have this fear that I'm going to start the program and the table will run far off base because the controller doesn't actually know where I meant the part to be. If somebody could explain zeroing, home position, reference points, executing the program and which application I need to get this up and running, I would be making chips in no time!

[Al_The_Man]

Sounds like you are jumping in the deep end, I would suggest you get a good book like Computer Numerical Control Programming by Michael Shaw and Joseph Pusztai.
You need to know about G54 to G59 - Work Coordinate shift. and Tool offsets, among a few other things.
Be wary that dry run will run rapid around the part without the spindle running, so make sure you do not have tools in or take other precautions.
When testing a program, use the feed rate over ride to slow the feed right down and check the distance to go, on the screen, some feed rate O.R. will go right down to zero, depending on how the OEM set it up.
Al.

[DerHammer]

Hi Al,

your right about the deep end of the pool thing, its a good thing I can swim right =). I am learning fast though. I do know what tool offsets are, but I have no idea how to manage/input a tool table in the controller. I was trying to play with it earlier, no tools in the end mill holder, feed rate turned down like you suggested but I couldn't get any movement whatsoever when trying to run the program. This was with auto mode/ dry run lit up.. I got no response out of the cycle start. Any suggestions? is this because my tool table isn't set up in the controller? Why is my controller ignoring me? =)

[Al_The_Man]

You need to find out what is in the cycle start string, like air pressure, door switches etc.
The other thing is to turn the ladder on if it is not showing, as this is a marvelous tool when trying to find out what is (not) happening.
It is Parameter 0060 #2 set to one.
This controls the machine functions like spindle, tool changers, all the operator panel switches etc.
The feed hold is not on is it?
Al.

[DerHammer]

what do you mean by #2 in parameter 60? are you talking about the byte thats third from the right ..aka "byte 2?"

I looked for a feed hold button but never found one, there are a few blank buttons without labels, but as far as I know they don't do anything especially because they don't look worn and none of their lights are lit up anyways. the face is actually in pretty good shape.

As far as the cycle start string, your going to haft to elaborate there. I have no idea what your talking about on this particular point but I'm presuming that this somehow relates to an early line in the program? Is that right? please elaborate here

[Al_The_Man]

As far as the cycle start string, your going to haft to elaborate there. I have no idea what your talking about on this particular point but I'm presuming that this somehow relates to an early line in the program?

This is a general idea as to how your machine operates, the CNC side of the system look after operating the servo's and running the CNC part program, which you have already found out how to enter, there is another process(or) called the PMC or PLC Ladder, which is a program that is written by the MTB that controls all the other machine external operations, i.e. makes sure the M,S & T codes are carried out, and any other external housekeeping duties.
Both these processors can comunicate with each other.
This also includes how the operator panel functions are conditioned and used, for example, before the PMC passes a cycle start over to the CNC side, it may ensure that the air pressure switch is on and the doors are closed.
Now normally, all you should have to do is write the part program, download it and switch to memory and press cycle start.
But with operating a CNC machine there are also times when alarms or operator messages appear or, as in your case, nothing seems to happen.
This is where the diagnostic in the form of the PMC ladder comes in.
What this does is display the logic circuitry that the MTB/OEM wrote in the form that is used in electrical print schematics.
When you display it it shows the functions in the form of normally open/normally closed contacts that are on or made when highlighted, if the rung or 'string' is complete the output 'relay coil' will be highlighted.
In the case of the cycle start, there is a 'coil' that is actually a register bit that is passed over to the CNC side telling the CNC to Cycle Start.
I know this may seem a bit overwhelming, but if you master it it helps trouble shooting and can prevent expensive service calls.
If your machine does not display the ladder, it can usually be turned on by setting parameter 0060 bit 2 to a 1 this is bit xxxxx1xx (the bits start at 0 to 7).
It will help a great deal if you have the annotated ladder listing in the documentation.
Al.

[DerHammer]

Hi Al,

this rabbit hole keeps getting deeper =), but its interesting. When you say "switch to memory" after downloading, what exactly do you mean by this because I may not have done this step before if it is one. Ill also check out parameter 60 too!

[Dan Fritz]

Al_The_Man is referring to the safety conditions that are necessary to permit the machine to cycle start. Most machines have one or more things that can prevent cycle start for safety reasons. For example, if you have low air pressure, low hydraulic pressure, low way lube level, etc. the machine may not cycle start until you satisfy that requirement. By looking at the "ladder", display on the control, you might be able to see what's holding you up.

On the machine interface, there is a signal called "STLK" (Start Lock). If this signal is on, the machine just won't cycle start. Some machine tool builders program the ladder logic for the machine interface so that a whole bunch of different things might turn on the STLK signal, preventing you from starting in AUTO mode.

Generally, if you press CYCLE START and nothing happens at all (no cycle start light comes on), that means that one of these safety conditions is not met. If the cycle start light comes on and stays on (but nothing happens), that's a different matter. You may have your feerate override set to 0%, or you may have something in your program that can't "finish out" like a tool change or a spindle-on command, etc.

Some machines have safety interlocks on the door switches, so you have to close the doors before it will start (some shops jumper out these switches because they are so anoying). You may have a chuck open/close switch that must be in the "Close" position, you may have almost anything safety related wired into this circuit. If this machine's been sitting idle for a while, I'd check the way lube level first. Also try to index the tool turret by giving it some T-commands in MDI mode and pressing CYCLE START to see if that works. If the entering a 1-block command of any kind in MDI and then pressing CYCLE START results in movement, then the cycle start button is working, but the safety interlock just won't let you start in AUTO mode.

[DerHammer]

yeah, The cycle start light does come on.. but theres no movement. like mentioned previously, I am new to this and the program I loaded might be tad bit long for my first program to start with "basic profiling on a rectangle, but has alot of step downs for multiple passes".

When I brought home the machine, I actually ran one of the programs still in memory from the previous owner and it did worked "set off the stroke limit alarm" but I did get some movement. Being a nub I cleared them to free up the memory and now wish I had not, because it would of helped trouble shoot this. When I first loaded the code, it did give me a unreadable g-code alarm, in which I reset, changed an early program line which looked odd and tried to rerun it. No alarm this time, but no movement either. The cycle start light does stay illuminated though if this is a helpful clue.

In the mean time, I'm going to try recreate a part to post with just one pass and hopefully I might have better luck. Am I correct to assume that my procedure was correct then? "auto mode, dry/or test run, then cycle start?

[Dan Fritz]

If you can make the machine stop with the cycle start light on, press the DGNOS button and look at diagnostic #700. One or more of the digits will be "1", indicating what the control is waiting for:

Bit 0 (far right bit): Control is waiting to finish an M, S, or T command
Bit 1: The control is executing an axis motion command
Bit 2: A dwell is being executed (G04)
Bit 3: Servos are not in position, control thinks a move has not been finished
Bit 4: Feedrate override is at 0%
Bit 5: Interlock signal STLK is on.
Bit 6: Control is waiting for spindle to come up to speed. (or down to speed)

[DerHammer]

Just came in from the garage. I created another small part program, this one much shorter but got the same error as before. The controller is giving a ps 010 alarm whenever I try to run it. My book says that this is a "unreadable G-code alarm".

I am using the correct post processor supplied from my cam software but don't know g-code myself, so I have no whats off if at all.
I am using rhino with madcam. Any thoughts? In the mean time ill check out that parameter too.

[Al_The_Man]

Unless you post the program here, you could reduce the program to find out the offending code.
Is it a Fanuc 0 post processor?
Al.

[DerHammer]

Good idea, why didn't I think of that =)

anyways, heres the program I created. This basic part was generated from a cad drawing in rhino/madcam and of course, with the fanuc OM post included with the cam plug in. This should be a small rectangle. anything look fishy for an om?

%
O1
G40 G55 G80 G90
M06 T1
S4000 F30 M03
G43 H1
F20000
G1X3.131Y2.234
Z0.625
G1Z1.000 F30
X3.128Y2.233F30
X3.100Y2.200Z0.833
X3.090Y2.172Z0.750
X3.090Y2.143Z0.667
X3.097Y2.120Z0.583
X3.103Y2.103Z0.500
X3.134Y2.055
X3.145Y2.000
Y0.000
X3.134Y-0.055
X3.103Y-0.103
X3.055Y-0.134
X3.000Y-0.145
X0.000
X-0.055Y-0.134
X-0.103Y-0.103
X-0.134Y-0.055
X-0.145Y0.000
Y2.000
X-0.134Y2.055
X-0.103Y2.103
X-0.055Y2.134
X0.000Y2.145
X3.000
X3.055Y2.134
X3.103Y2.103
X3.120Y2.097
X3.143Y2.090
X3.172Y2.090
X3.200Y2.100
X3.220Y2.114
X3.234Y2.131
F20000
G1Z0.645
F20000
G1X3.131Y2.234
G1Z0.500 F30
X3.128Y2.233F30
X3.100Y2.200Z0.333
X3.090Y2.172Z0.250
X3.090Y2.143Z0.167
X3.097Y2.120Z0.083
X3.103Y2.103Z0.000
X3.134Y2.055
X3.145Y2.000
Y0.000
X3.134Y-0.055
X3.103Y-0.103
X3.055Y-0.134
X3.000Y-0.145
X0.000
X-0.055Y-0.134
X-0.103Y-0.103
X-0.134Y-0.055
X-0.145Y0.000
Y2.000
X-0.134Y2.055
X-0.103Y2.103
X-0.055Y2.134
X0.000Y2.145
X3.000
X3.055Y2.134
X3.103Y2.103
X3.120Y2.097
X3.143Y2.090
X3.172Y2.090
X3.200Y2.100
X3.220Y2.114
X3.234Y2.131
F20000
G1Z0.625
M09
M30