What's new
What's new

Fanuc O M controller on a (SuperMax 2) 3 axis mill, need help with machine offsets & no BT-40 spindle rotation, because hi-speed spindle is mounted

dandrummerman21, many thanks!! I loaded your program after doing "zero return", the z axis stayed at the home (all the way up) position, both x & y-axis moved table from "zero return" positions to looks to be center/middle of the table is center of spindle. The "sample" program I used in "auto" looked correct when moving. I am not confident starting a new part, knowing the machine and tool offset are correct, please understand I will not be using the ATC and my high-spindle uses only collets and I understand I will need to touch off each time the tool is changed.​


Many thanks for any suggestions!
 
I have pic of before and after the "start button" was pushed of the "position all screen" and the "actual" & "absolute" screen location are the same, after the program has run the "machine" location has the x & y distance referenced and the "actual" & "absolute" screens only have the z axis location, all others are 0s.
 

Attachments

  • IMG_3084.JPG
    IMG_3084.JPG
    2.2 MB · Views: 4
  • IMG_3085.JPG
    IMG_3085.JPG
    2 MB · Views: 4
Was about to post and saw your successful try of dandrummer's program. As long as the coordinates you had entered into G54 represent roughly the center of your table, then all is good. The screens all look right. You must have a 4+ inch setting in your G54 Z work offsets.

Some tidbits to consider in general.

G53 is a "One Shot" call. Meaning only active in the Block containing it. The reference to G53 is not so much the EXT. Coordinate section of the Work Coordinate Screen, but rather a direct reference to Machine Zero. Recently I've come to understand that EXT. or SHIFT, according to our Resident Forum Guru angelw, is better thought of as G52. And can be acted upon in a Program by G52 Xx Yx Zx

G54 should be active when you turn the machine on. But if it is all 0's at turn on, and then you enter coordinate values into it, until you call G54 again the control will not know that you have changed anything and will act as if nothing new has happened. Also, anything resident in the EXT./SHIFT location on the first Work Offset screen will affect all Work Offsets whether you ask it to or not.
 
Last edited:
Many thanks for helping me understand my controller, as to be transparent, the G54 was set when the pics were taken to the exact values you see in the pics, x-13.062; y-6.216 & z-4.7946. As per running dandrummerman21, suggested program, why did the z axis not go to -4.7946, vs not moving at all? It is this z axis that I am stumbling over. When I try my sample program, there is a stop for manual end mill change, at this time I will "touch off" to the top of the material with a new tool (of a different tool length) to start the program again. Is this the way to approach this? If I have not thought through this correctly, say so.
 
The Position screens are pretty useless after Machine On until you actually do something. Once you made a move in Auto and called a Work Offset, they squared themselves. Honestly I wish you would give less care to what the ABS REL position displays say and concentrate on what the machine does physically. Distance To Go is your only true friend.

Trust the machine to do and go to exactly where you tell it to in every instance. It will make no mistakes when compared to what it is told to do. If you have your Offsets properly set, and you believe in what you programmed, you can rest at ease and watch it go to all the right places.
 
If I were you, I would run the machine with all Work Offsets set to Z0. Measure each new tool to the top of the material and enter what you see in the Machine Position Display Z value into T1 Tool Offset. Same place each time. Don't recall if Z/EOB/INPUT worked on your machine or not. If it does, use that. With Z0's everywhere it will give you the Tool Offset number(s) you're after.

I finished some testing on my OMC Supermax 3. It took me a minute to get it to accept the G49's and not over-travel in Z. My Tool Change Macro must have always taken care of this as for the most part it has never been a problem.The key I find is the sort of RESET nature of G28. If you want to see the difference in sending the Z axis Home between using G91 G28 Z0 and G53 Z0, try them in MDI with the head down a few inches. Using G91G28 Z0 the Z Home or Z Zero Return light will light. Using G53 the head goes to the exact same place but the Zero Return lamp doesn't light. There is more significance to this then a light bulb turning on.

This is a format you can use to start each tool. You have to return the Z axis home using G91G28Z0 before starting up a new tool. That or hit the RESET button which I'm sure is not what you want to do in this situation. G53 won't set the machine up for the next bunch of moves including your manual intervention to set a new Tool Offset. The machine either over-travels or it stalled without alarm and wouldn't move.

Here's the test program I used. You can use any tool offset you want for each tool or use T1 for all. Just set the appropriate H number as needed. Note that after all the M00 (T1.x TOOL DESCRIPTION HERE) blocks, you are free to put the machine in RAPID or JOG and move it to wherever you want to find your new Tool Offset. When done and entered into the Tool Offset page, raise the head up a few inches and return to AUTO mode and hit the flashing Green Button. At first if you want to be real safe, just copy and paste the G91G28Z0 line (Already did) and put it right after the M00's. This will put the head home to start fresh for the new tool. The G90 in the Safety Line will take care of that little G90 need after a G91G28.
BELOW EDITED SINCE ORIGINAL POST: Now twice! (Removed M3)
%
O1234 (NO TOOL CHANGE TEST)

(T1.1 TOOL DESCRIPTION HERE)
G17G20G40G49G54G80G90G98

G0X0.Y0. (adjust to suit)
G43Z0.1H1

(INSERT NORMAL PROGRAMMING HERE)

G91G28Z0.M5
G90
M00 (T1.2 TOOL DESCRIPTION HERE)

G91G28Z0. (IF YOU WANT TO PLAY IT REAL SAFE AT FIRST)
G17G20G40G49G54G80G90G98

G0X0.Y0. (adjust to suit)
G43Z0.1H1

(INSERT NORMAL PROGRAMMING HERE)

G91G28Z0.M5
G90
M00 (T1.3 TOOL DESCRIPTION HERE)

G91G28Z0. (IF YOU WANT TO PLAY IT REAL SAFE AT FIRST)
G17G20G40G49G54G80G90G98

G0X0.Y0. (adjust to suit)
G43Z0.1H1

(INSERT NORMAL PROGRAMMING HERE)

G91G28Z0.M5
G90
G53Y0.
M30
%

I believe M30 will act as a RESET so G91G28 not needed, but will work. Remember to ALWAYS follow G91G28Z0 with a G90 on the very next line.
 
Last edited:
13engines, many, many thanks, you have been very generous with your time and knowledge, I am truly grateful. I will try this out on my sample program with indicator attached to the spindle. Will copy & paste your code, on a new program in BobCad and use as needed.

When I see "G0X0.Y0. (adjust to suit)" the "adjust to suit" is the (the x, & y location from home or "zero return" (from machine position screen, use this data as the source)) to pin or reamed hole that is origin to the part? This if I were to put an indicator in the spindle I could check how close the mill repeats to this location?

The "Z/EOB/INPUT" procedure to copy data, I am not completely shore of, but will test it. When the prior owner was here recently, I found what the deal was about "light bulb turning on" some of the buttons on the control panel have a small light bulb under the surface of the button that will light, I found this out when I put the question to the prior owner as why the x-axis was the only axis that would light when "zero return" was used, the answer this the only button that the small bulb was good, I have not looked to see what other bulbs are not working. It may take me sometime, there are a few things going on this week.

Many thanks
 
When I see "G0X0.Y0. (adjust to suit)" the "adjust to suit" is the (the x, & y location from home or "zero return" (from machine position screen, use this data as the source)) to pin or reamed hole that is origin to the part? This if I were to put an indicator in the spindle I could check how close the mill repeats to this location?
G0X0.Y0. is the first location you want to send your tool to. Adjust it to place the tool at the first point of interest in your program. Forget about Machine Zero Return after you've set your Work Offset. Everything you do in your program from there on out will relate directly to whatever Work Offset you have called and not Machine Zero anymore. (Not directly anyway) You've told your machine where your work piece is, so now everything you tell it from there on out refers to that location. (G54 in your case most of the time)

When testing the program, have the Program Check Screen active and watch the Distance To Go display. Stop the tool with the Feed Hold button when the tool gets close in Z to Z0.1, then ask yourself, does the distance to go value I see look about like what I see in the machine? If so, you're probably okay to hit the Green Button again. You could even run the whole thing in Single Block Mode to start. Also it wouldn't hurt to put an X and Y Feed move in the (INSERT NORMAL PROGRAMMING HERE) area. Something basic like.
G1X2. F30.
Y-2.
Just so it acts a little bit like a real program would.

I thought we went over this once before but maybe not. When you get your tool touching the top of your workpiece where you want to call Z0. bring up your Offset screen, set the Cursor to T1, then in a manner similar to Control/Alt/Delete on a computer, hit EOB/Z/INPUT. EOB/Z should place the Z value of the Machine Position Display into the Buffer Area at the bottom left of your screen. INPUT will enter that info into T1 for you. If it doesn't, write down exactly what you see in the Machine Position Display and INPUT the value into T1 manually. (it will be a negative number)

If the Control Panel Buttons are anything like mine, (colored and rectangular) the light bulbs are easy enough to replace and still very common to locate. To replace, carefully pry off the cover, then using a rubber hose or cap of the right diameter as a puller, press it over the bulb and then pull it out. (Friction Fit)

Got to go. Slave to a lathe again for another 3 days.
 
Last edited:
13engines, thank you for all the help. I have gone back to the beginning as to test the difference between G91 G28 Z0; and G53 Z0 in MDI mode do the following:

13engines,s example from post 47; "If you want to see the difference in sending the Z axis Home between using G91 G28 Z0 and G53 Z0, try them in MDI with the head down a few inches. Using G91G28 Z0 the Z Home or Z Zero Return light will light."

When I was in MDI mode the area at the bottom of screen on the right side as per manual should say [RSTR] & my screen does not say that (see pic) at the bottom on left you can see my input, keyed in the G91 G28 Z0, used Input & nothing happen, no motion, nothing. The mill had "zero return" with z axis down a few inches.

I first tried to copy and paste 13engines,s code from post 47, but found some conflicts, my internet computer is Linux, my BobCad PC is Window 10. It will allow saving & run from USB drive (will not allow saving to hard drive in win10), so just clumsy, I will just key in a copy of 13engines,s example and work with it. After editing this file to add a simple sample program, the alarm was the 07 alarm (improper use of a "." period was the alarm), noting happen, no motion just the alarm 07.

Many thanks, suggestions welcomed.
 

Attachments

  • IMG_3090.JPG
    IMG_3090.JPG
    2.1 MB · Views: 4
Not able to respond in depth now. But after keying something in via MDI, each line has to end with an EOB and then hit INSERT. Then the Output Start Button. Your command line should end up at the top of the page after O0000

Copy and paste my code into a text file. Then open that in your Predetor Software and copy to the machine.

EDIT IN: I don't see any improper periods in my code sample.
 
Last edited:
Those miniature bulbs under the switch cover only have the 33/24V stamped on them, but I have not found a source yet or something close to looking like the base, a small piece of Tygon tube is what I found that fit. I have good lights on the +X, +Y, & +Z switches, will replace old bulbs when I find new ones.

When I used the MDI mode this time ending with EOB, then Input, then <start>; nothing happen, the axis were off their "home" position by several inches. I tried both G91 G28 Z0 and G53 Z0, after entering "EOB" there was a " ; " add to end of line, when "Input" was pushed, no movement but the line (G91 G28 Z0 and / or G53 Z0) disappeared.

13engines, thanks!
 
13engines, thanks! The G91 G28 Z0; EOB; INSERT, press <start> all worked as hoped, z axis went to zero return, all the way up, nothing else moved and the Z axis light was ON. When I tried the G53 Z0, nothing happens, not motion, no light. Both methods should have worked, correct.
As to defend my thinking as to why I was using INPUT with the MDI mode, I can only point to the manual, please see pic.
I will be working using your g-code with a simple shape in BobCad/Predator Editor to find what the secret handshake is, but will be checking in for any suggestions.

Many thanks!
 

Attachments

  • MDIfromManual.JPG
    MDIfromManual.JPG
    1.5 MB · Views: 5
Wow... everything about that page is incorrect. That is not the MDI screen as I've ever seen it, and INPUT is not the correct key to place something active in MDI. INSERT is. You might want to get a later version of that manual. They make a lot of fixes over the years and publish updated editions. The number at the end after the / is the Edition number of any Fanuc manual.

If you were already at Z zero after doing G91G28Z0 and the light was on, and without moving anything tried G53Z0 and nothing moved and the light went off, then everything happened as it should. One point is... why would there be any movement when the Z axis was already at Z0 and you told it to go to Z0 again???
BTW, don't forget to do a G90 EOB INSERT after doing a G91. You can even do it at the same time after G91G28Z0 by creating a 2nd line of code before hitting the Green button.

What I was trying to say in my instructions was to move the head down before each try. You would have had to moved the axis back down a few inches before trying G53Z0. Anyway... the fact that the light went off shows there is a difference. In normal use the machine will know the difference and act accordingly.

If you're having trouble getting your computer to transfer files to and from the machine, try purchasing dnc4u out of Great Britain. Very good program for transferring and DNC work. Been using it for years.Nice UI and loaded with helpful tidbits.
 
The manuals are dated on the front to 1988, but on the back (lower right) the Maintenance manual is dated Aug 1992 the Operator's manual (this is where the page came from in post #54) is dated April 1985, so 10yrs. older than the mill.

Using MDI G53 Z0, when the head is several inches from home, this command does nothing. From the same z position and use the G91G28Z0 and the z axis, move to home and the light comes on.

Is it possible the way the post processor is written that the z axis data only needs to be in a single location? Referencing post 47 this part:
"G43Z0.1H1" only put in G54, not tool offset also?

Could it be that the "tool offset" (this is the same value (this value comes from the "machine position" screen) as the z axis in "machine position") and G54; I am suggesting it only needs to be in tool offset or G54, but not both as inputs, seems like the z axis is where I get too much negative z axis?

Or do I need to be real careful to not use the "handle" to change positions, so the mill will not lose its position after the program is running? Is this an issue to use "handle" and know the mill will not lose its location?

I am using the very beginning & end of 13engines,s example from post 47, with a 4 sided small part programmed in the middle. This will start and run until the end of the small part and then z axis goes up to the home position and y-axis comes to the operator, just like I hoped. The orientation in x & y look to be acceptable (close to where you would think they should be) the z axis not so much. I am trying to do 1 line at a time and editing the file and reload to tease out the issue.

The DNC device I have does work well now, and programs are easy to copy.

13engines, many thanks, I welcome any suggestion.
 
The manuals are dated on the front to 1988, but on the back (lower right) the Maintenance manual is dated Aug 1992 the Operator's manual (this is where the page came from in post #54) is dated April 1985, so 10yrs. older than the mill.
Not completely about the manual date. The Manual Part Number Edition number after the backslash. Something like B-61404E/05 (OMC Operations Manual)
Using MDI G53 Z0, when the head is several inches from home, this command does nothing. From the same z position and use the G91G28Z0 and the z axis, move to home and the light comes on.
Weird, G53 works on mine in the same situation. Might be a parameter or maybe just different models or Firmware. Did you go back to G90 first before trying G53? That might make it not work. I see Vancbiker has the answer to this.
Is it possible the way the post processor is written that the z axis data only needs to be in a single location? Referencing post 47 this part:
"G43Z0.1H1" only put in G54, not tool offset also?
As I said, run your Work Offsets (G54-G59) at Z0. Set each tool as it is brought to bare in the Tool Offset page. (H) Your Post Processor only needs to call G54 once for the whole program as long as another Work Offset is not called. And a G43Z0.1H1 for each new tool is all that is needed to let the machine know what's up. (As long as you've chosen to use T1 for everything) All the other programming spit out by the Post has to do with creating your part, including all Z moves etc.

EDIT IN: The Post programming expects that all offsets are valid and is not concerned about them other then calling them into play. The post is not trying to set anything new or replace anything. Only call it into being present and operative.
Could it be that the "tool offset" (this is the same value (this value comes from the "machine position" screen) as the z axis in "machine position") and G54; I am suggesting it only needs to be in tool offset or G54, but not both as inputs, seems like the z axis is where I get too much negative z axis?
Yes the Z- value is needed in one place only. The Tool Offset Page.
Or do I need to be real careful to not use the "handle" to change positions, so the mill will not lose its position after the program is running? Is this an issue to use "handle" and know the mill will not lose its location?
You should be able to use the Handle all you want between tools, as long as you follow my earlier Program example. The green button light should never go out while you're measuring a new tool and entering in the new Tool Offset value. Meaning no hitting RESET. The current value in the Tool Offset will not effect what you see in the Machine Display while measuring a new tool. So the number you use for your new tool will be exactly what you see there. ie... roughly the same as previous but different.
I am using the very beginning & end of 13engines,s example from post 47, with a 4 sided small part programmed in the middle. This will start and run until the end of the small part and then z axis goes up to the home position and y-axis comes to the operator, just like I hoped. The orientation in x & y look to be acceptable (close to where you would think they should be) the z axis not so much. I am trying to do 1 line at a time and editing the file and reload to tease out the issue.
Not sure what the issue is as seen from here.

Sorry I'm somewhat distracted trying to keep a lathe moving. Think I get things right.
 
Last edited:
Pretty sure that manual is for a 0ma or 0mb, also relatively sure that in MDI, you would hit the INPUT button to insert crap.

Been a while since I messed with one, but we had a 0ta that we recently scrapped that I would occasionally have to help someone out with, that I had to remember to insert a command was the input button, not insert.

Your machine is probably a 0mc based on the age of the mill per your comment.
 
Gentlemen, at last a proven matching set of, parameters, diagnostic and O9020 ATC Macro, needless to say I have been busy. This would not of been successful without a great deal of excellent help from many people, including on this very forum, in addition to YCM's machine tool builder's Advanced Service Engineer, who was a true blessing. The ATC and other systems work as designed with this update, finally.

I am seeking a 2nd opinion, I have referenced 13engines's post 47 that this is the appropriate g-code to use after a M00 stop (this tool stop needs to allow for use, all axis to "touch off", to set next tool height).

This is from 13engines's post 47.
"G91G28Z0.
G17G20G40G49G54G80G90G98"

The attached pic is the screen of DNC4U software to "Drip Feed" a program that was created in BobCad, (I was unable to figure out the Predator Editor's "DNC send". The pic shows the 2 screens in the DNC4U software, (1 screen on the left, just above the "(1 MM ENDMILL in GREEN)" at the top you can see Line N4432 with M00 (in RED) command) and on the right side of the screen is the same line of code in the DNC4U software that allows the input of g-code commands on the far right side of that screen, that are suggested to restart the program from the M00 command. It will save these commands for next time, so I need the information that's required but no more than necessary. I am trying to get a templent or something to pattern from, and so I have confidence from the start.

Referencing 13engines's post 47; the g-code enclosed in the " " is this acceptable to put on the far right side of the DNC4U screen?

When this tool change happens, this is the finish cut on a pocket that was rough out earlier in the program. I plan to "touch off" on the top of the part (that was how the roughing pass was located), this may require to move all 3 axes. I will record the final Z axis location and manually key that as the new tool length for the finish cut.

Many thanks in advance for suggestions!
 

Attachments

  • DNC4U with Restart.png
    DNC4U with Restart.png
    1.8 MB · Views: 6








 
Back
Top