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

[solidworks4u]

13engines, thank you! I have a way forward with BobCad and Editor Predator to make a big part of the code ready to get the tool & program to become aligned to the start point that the machine agrees with.​

The way it makes sense (because this I saw on YouTube) to me is start at the top surface of the mill table, z=0.0, I will allow for the vise height (with part included), unless this (at top of the part) is a better/preferred height to use as a start point.​

The vise will have a stop to locate a sub-base to it each time in the same place, the sub-base will have a reamed hole to "Dial In" the x & y-axis. The small reamed hole will be located off the part, so I can check the starting point with an indicator with a part in place. The small reamed hole is at a known location in relation to the part's datum points.​

I will try to attach a few pics of the screen as I attempt to set the z axis with a "pin of known length" (see the 7.150" in top of pic 74). This is after "zero return" the pics are in order. Referencing, the last number of each pic; ends in 71 is the work coordinates; pic 73 is after "zero return" for all axis; pic 74 is when I put a 7.150" tall pin on machine table, this screen is after moving all the axis from the zero return locations, so I can get close to the pin in the center of table.
I know that I am to use this 7.150" (181.615 mm) with the z axis number from "work coordinates" to set the top left spot in the "tool offset" screen, or have I mixed that up and need to go to actual position screen. You see in pic 74 "machine" (lower left on screen) is in metric, all others appear in inch (I do not know what happen). I am not clear in this part, but realize this is the area that will require to be edited often, so I need to be clear in my thinking.

I am not shore of my thinking, I need a second opinion, am I on the correct path?

Many, many thanks to you 13engines, and all the others who have been so kind to help!

 

[13engines]

Don't have too much time right this minute, but a couple things need to be corrected before you go anywhere.

First... you CAN NOT be using Metric and Imperial at the same time. It looks like you machine is set on Metric, but at some point you had Imperial going. Or vise-versa. Make sure the main System Setup Screen on your control is set to Imperial. And be sure there are no G21's in your programs. Usually near the beginning. You want G20 only. (Reverse all of that if you work in Metric)

2nd: You should not have anything in the SHIFT area. (Right above G54) Or in your G54 Z row. My understanding is you run one hand placed tool at a time. The distance your Tool is from Machine Z0 to the top of your workpiece should be set in your Tool Offset. Not there. That number you store is applied to the tool by the G43 H code call. Generally G43H1 for you.

There is no reason for you to be using the SHIFT area when running parts. If you read way back when I was describing how to use the Shift to adjust for a tool setter if you were using one. But when you get back to pushing the Green Button, there should not be anything in there.

 

[13engines]

Hi Solidworks, Re-reading your post I'll say this. Seems your X and Y location strategy is fine. The Z is another matter.

Why are you measuring a 7" pin? How are you even holding it? What on earth does that pin have to do with where the top of your work material is? But I digress... The only thing that really matters is how far from Machine Zero the Machine is, when your tool is touching the top of your work piece. The Control needs to know what that number is, so when your Program says Z0, the machine is well informed enough to place your tool perfectly on top of your part. It finds that number in the Tool Offset Table via a G43Hx call, where x is the tool number currently in the Spindle.

So how do you find that number? There are a couple of ways. Sadly even using that silly pin. I use either a 0.001" piece of shim stock, or a 4" tall dial Setting Device. I'll make life easy for you, and use the mind numbing 7.150 pin. The same strategy can be used with any other "thing" of known length.

1) Make sure your SHIFT and G54 thru G59 Z's are all 0.
2) Enter the length of your 7.150 setting device as a positive number into the SHIFT Z area.
3) With the setting device touching the top of your work material, (the place you want to call Z0) lower the tool until it touches the setting device.
4) Go to your Tool Offset screen and make the cursor active next to the tool number you're dealing with. Say T1.
5) In the same fashion that you would do Control/Alt/Delete on your computer, hit Z, EOB, INPUT. That will place the combined value of the current Machine Position, plus the length of your Setting Device into Tool Register 1. Nifty huh?
6) Go back to the Work Offset SHIFT Register and make that Z0.
7) Run your program.

Now... an alternative that isn't quite as good but may be of benefit if you have slightly shifting stock thickness is, do everything above except measure to the top of your subplate instead of the top of your current work material. Then

6a) Measure your work material thickness with a micrometer, and enter that positive measured number into your G54 Z area. Don't forget to make SHIFT Z0.
7) Run your program.

Hope that all makes sense. I believe you said you have a Fanuc O machine.. The Z,EOB,INPUT should work on them. Does on mine.

 

[solidworks4u]

13engines, thank you for your time and knowledge, you have been kind, bless you!​

If you believe the disagreement in the "metric vs. imperial" will make this an ongoing issue, I will start fresh to try not to allow this to happen again? Please tell me what you're thinking.

What needs to happen to get the metric vs. imperial on the same page, is starting fresh, using the USB to mill devise to input parameters and diagnostic data I believe.​

The 7.150 pin (round stock 7/8" dia x 7.150") was the 1st piece of material that I found to face off & measure accurately, it stands up by its self. I kind of rock-it & twist when close, as I lower the z axis, this process I saw on YouTube video.

I can follow the logic in "touch off" top of material and call that Z=0.

When you say: "1) Make sure your SHIFT and G54 thru G59 Z's are all 0." the word shift is the tool offset screen, correct?

13engines, this is way too cool/Nifty & great to know!!​

"5) In the same fashion that you would do Control/Alt/Delete on your computer, hit Z, EOB, INPUT. That will place the combined value of the current Machine Position, plus the length of your Setting Device into Tool Register 1. Nifty huh?"​

Before I have anything in the spindle, I plan to temporarily tape a penile to the spindle with approx the length of the hi-speed spindle to see how that looks and get some confidence.
I plan to try the 1st approach, not the one that allows for (slightly shifting stock thickness) until I have more confidence in myself. The varying stock issue is real, just too many things to think clearly about now.

Many thanks, I have plenty to keep busy with! Much, much more if the "metric vs. imperial" issue needs to go away, and I need to start fresh.

 

[dandrummerman21]

If you make parameter 63 bit 0 = 1 (xxxxxxx1) then the machine coordinates will show as inches, since that's what you have the machine set to.

 

[solidworks4u]

dandrummerman21, many thanks!! I will check what I got at parameter 63.0 (did I get that correct?) make shore to go to 1.​

Many thanks!

 

[13engines]

​

If you believe the disagreement in the "metric vs. imperial" will make this an ongoing issue, I will start fresh to try not to allow this to happen again? Please tell me what you're thinking.

What needs to happen to get the metric vs. imperial on the same page, is starting fresh, using the USB to mill devise to input parameters and diagnostic data I believe.​

Just go to your Parameter Setting 1 page and make sure it's set on inch. I tried to take a pic but it wouldn't work. You can also do what Dandrummer said. Your USB device is mostly for transferring programs and running DNC. I suppose you can use it for changing parameters, but I think most folks do that at the control. You go to your Parameter 2 page and set PWE (Parameter Write Enable) to 1 (ignore the alarm) You can Page Down a few times to 63. Then enter exactly what is there except for the last digit on the right make 1. After that, go back to Settings Page 2 and put PWE to 0. Then hit RESET. If you still have an alarm you have to shut the control off and turn it back on again to clear it.

When you say: "1) Make sure your SHIFT and G54 thru G59 Z's are all 0." the word shift is the tool offset screen, correct?

No... Work Offset Screen right above G54

It would do you some good to download a Fanuc O Operations manual for the Model of O control you have. This will help you find all the different screens you might need.

 

[Vancbiker]

If you make parameter 63 bit 0 = 1 (xxxxxxx1) then the machine coordinates will show as inches, since that's what you have the machine set to.

This does not work on A or B versions of the 0 series controls. Machine Position display on those versions will always be in the units of the ballscrew pitch.

 

[13engines]

This does not work on A or B versions of the 0 series controls. Machine Position display on those versions will always be in the units of the ballscrew pitch.

What the... so how does one set their tool offsets when the most important numbers on the screen are metric? And does Z/EOB/INPUT even work? If so does it do any auto translating? What version does the OP have. Did he say?

 

[solidworks4u]

Many, many thanks, to each of you guys for helping me through this.

I have a computer, downstairs by the mill that I was not logged in, so can't leave a message there, and I needed to verify the version I have. Mine is a PLC: B1 Revision 4.; this was info the machine builder requested early in our conversations and where I went to verify this.

dandrummerman21, THANKS!! This worked just like that, my 63 parameter is now 00001001, this made the "all position screen" all went to inches. I have removed the z values in the G54 to G59.​

I have not pondered the most recent messages other than add this info: PLC: B1 Revision 4. This I hope helps to understand what I am working on, if not please say so if this is not the correct info and I will look again.

I was not able to get the "Z/EOB/INPUT" to work for me, but I only tried 1 time, took pic, but camera is downstairs with the mill. Because the number did not autofill, I measured with tape measure the approx height of my 7.150 pin + 4.5" (part on paraells in vise, height), to top of part and keyed that in.

Many thanks!

 

[Vancbiker]

What the... so how does one set their tool offsets when the most important numbers on the screen are metric? And does Z/EOB/INPUT even work? If so does it do any auto translating? What version does the OP have. Did he say?

On my 0MB equipped Makino, Z/EOB/INPUT works but the values come from the Relative display so one has to be sure to zero that display after performing the initial zero return when powering up the machine.

 

[13engines]

On my 0MB equipped Makino, Z/EOB/INPUT works but the values come from the Relative display so one has to be sure to zero that display after performing the initial zero return when powering up the machine.

You know on my OMC, in maybe the 15 odd years I've owned it, I've never once touched the Relative Display. I never look at it and barely ever the Absolute either. So honestly all these years it could have been using the Relative, as I think it's Zeroed out when you turn on the machine. I'll have to experiment some time. It does accept anything I put into the Shift Display to compensate for my 4" Tool Setter. That much I know.

 

[solidworks4u]

Today for the 1st time I have had the yellow 360* light, strobe the shop, that the program was at the end!! Many thanks!!
This program had a pocket command, was too long for a sample program. My new sample program, real basic square profile with corner radius 2 places, a z axis offset/step, small quick in BobCad. In BobCad at the beginning when you use "stock wizard" one of the next screens has on the right side of the screen has vertical arrows at different heights as to where the tool is in relation to the part in this software. This critical amount of motion (from the mill tool set-up) that we are talking about needs to be included in this software? I believe so, it seems to me the rapid travel would be here, or is it that I have told the top of the part and that is all that is necessary for the z axis location?
In addition, for the x & y-axis, I will need to tell where the start point is (for all axis) in relation to the place where the mill stops after using "zero return". My hope is that I will do this only 1 time (every time if the vice or vice stop is moved) but the z axis I will need to do each time the tool is changed.
I will need to include a "pause" when the end mill is changed from ruffing to finish tool.
I am thinking about other parts of the program, that I will need to add to the part program that is generated when pocket command is used, an example is to get the tool in the correct place, to start to cut the part the 1st time, on the 1st part.
The "Relative display" when I ponder this screen, it should make sense if I have got my set-up and off-sets correct?
Many thanks for all the suggestions, I am very grateful.

 

[13engines]

Today for the 1st time I have had the yellow 360* light, strobe the shop, that the program was at the end!! Many thanks!!
This program had a pocket command, was too long for a sample program. My new sample program, real basic square profile with corner radius 2 places, a z axis offset/step, small quick in BobCad. In BobCad at the beginning when you use "stock wizard" one of the next screens has on the right side of the screen has vertical arrows at different heights as to where the tool is in relation to the part in this software. This critical amount of motion (from the mill tool set-up) that we are talking about needs to be included in this software? I believe so, it seems to me the rapid travel would be here, or is it that I have told the top of the part and that is all that is necessary for the z axis location?
In addition, for the x & y-axis, I will need to tell where the start point is (for all axis) in relation to the place where the mill stops after using "zero return". My hope is that I will do this only 1 time (every time if the vice or vice stop is moved) but the z axis I will need to do each time the tool is changed.
I will need to include a "pause" when the end mill is changed from ruffing to finish tool.
I am thinking about other parts of the program, that I will need to add to the part program that is generated when pocket command is used, an example is to get the tool in the correct place, to start to cut the part the 1st time, on the 1st part.
The "Relative display" when I ponder this screen, it should make sense if I have got my set-up and off-sets correct?
Many thanks for all the suggestions, I am very grateful.

Your Zero Return is only of consequence the first time you do it after turning the machine on for the day. You can also use it to easily send your Z or Y axis home manually. This gets the head out of the way and brings the table full forward for reloading. Another way to do that is to add this code at the end of your program.
G53Z0M5
G53Y0
M30

Your post is a little hard to follow, but I'll give you this. As long as you position your part in BobCad so that the same corner or point of interest on your part is the same (in all axis) as that which you're going to use when the part is in the machine, everything will come out fine. No other adjustments needed. The height above the work that the tool moves at in between cuts is called the Clearance Plane. There is likely a setting in BobCad to put that where you want. Z0.1 is a common height. Use more or less as you see fit.

A good code to use for stopping the machine so you can change the tool would be M00. This is a Mandatory Stop. Meaning it doesn't need any buttons pushed on the control for it to work. M01 if used, needs the Optional Stop Button on to work.

 

[solidworks4u]

It has been a busy week, after reaching out to the BobCad forum searching for the best way around, so the spindle would not need or require input to stay in the OFF position, the suggestion was a modified post processor that included a way to stop (M00) for tool change and allow "touch off" (to allow for z difference) when end mills are changed in the collet.
I have studied "machine offset" & "tool offset" in YouTube videos, most are a later model controller that my Fanuc O M, this model uses the "CAN" soft button in the "Relative" (DRO) screen to "zero out" (0.0) each axis (x, y, & z) as for the "start point" in relation to the part, I think, correct me if I am wrong. The "tool offset" all are 0.0; the "machine offset" all read zero, including z=0.0. Is this correct, I am not shore, there are several ways to do this, I need the easy w/o ATC requirements?? I have not given up on the fixed length pin (in my case 7.150") and input this as a "machine offset" value, if I get this correct it will set z=0.0 at the top of the table, correct, is this ideal for my application?
I am in need of firming up the method I am going to use to set "machine offset" & "tool offset"; being that every time the end mill is removed from the collet I will need to "touch off" so do I need to use "tool offset"?
From the small amount I have run, the table around, w/o anything bolted to the spindle, or to the table (so it can't hit anything) it looks to me that after the "touch off" this allows for the new z axis value w/o setting anything in "machine offset" & "tool offset" screens? Or do I need to study and look harder? Are their numbers in a certain screen that need to be input in to another screen?
It would be nice to have the ability to watch the DRO and have a way to check a z height distance with a scale (manually) to know I am the correct height to take a cut before "start cycle". This would provide a check to see if all is good and correct. I know there are more than 1 way to use or set up the "machine offset" & "tool offset" data, being I will never use ATC need something easy for beginner.

Many thanks.

 

[13engines]

Hi solidworks4u, You still seem to be struggling with the basic comprehension of what your setup tasks are. This is a lot. Take your time with it.

Let me ask... have you even once done everything in order like I showed in post #23? If not, please do it. If the Z/EOB/INPUT thing doesn't work on your machine, just input it in manually.

Let me try to explain what you're trying to do in setting up the machine to run a job.
When you Zero Return your machine each time you turn it on, stop and look at it for a minute. Let me say here that Position wise, your machine is pretty dumb. Where it's sitting right now at the Zero Return Position, is the only thing the machine knows for certain. Machine Coordinate X0.Y0.Z0. That's the full extent of it's Position knowledge all on its own. It knows nothing else.

In this Home Position, if you happened to have a perfectly long tool in the spindle, and could perfectly set your workpiece reference corner under that tool, you know, the reference point or corner you programmed to in BobCAD, and the tool perfectly touched the top of your material, you'd be ready to go without setting any offsets of any kind as in having everything zeroed. Wouldn't that be a dream? But it just so happens that that never happens. Nor is it even possible in a real sense.

In as such, your job is to tell the dumb machine where you decided to put things on the table, in reference to the only thing it knows on its own... Machine Home. You do this by locating the reference point on your workiece in 2D X/Y space with any number of locating devices available. This point in space may coincide with a point on your workholding, but not necessarily so. Then your job is to tell the machine where that place is. And where is the only and most reliable place to find that number that the machine needs to know? On the POS screen under MACHINE. And again... look nowhere else! See your center & right picture in post #21. It's there in both. You take what you see there and enter it into a Work Offset of your choosing. Generally people start with G54. See Pic on left in Post #21. Hit Mode OFFSET, then soft key WORK, then cursor to G54 X and enter via the Numeric Keypad, X- xx.xxxx, and the same with Y. Note that all your OFFSET numbers will ALWAYS be NEGATIVE.

That was X and Y, now Z. Do everything in post #23 for Z.

Now your machine knows where things are located. Other then your actual cutting program, that's all the machine needs to know. Near the beginning of your Program and before any axis movement, you will enter G54 somewhere. The machine will look there for what you're wanting it to know about where your work is sitting. When your tool loads and heads for the work, it should find in your program a G43 with a matching H code with it. EDIT HERE: Now the machine knows where to look for how far you had to move the Z axis away from Home, in order for your tool to touch the Z0. Reference plane on your part. In other words, your Tool Offset. (Z- Distance from Home)

In short... the only thing you're doing with all Offsets is telling the machine how for from Home it should do the requested work. That's all. Don't confuse yourself and attach any other grandiose meaning to it. Simple basic location form Home. Nothing more.

EDIT HERE: That's also why messing around with the Relative Display and Zeroing it out at some position is wasted work. The machine doesn't care about some arbitrary position you decided you wanted to Zero out to. Even after touching the tool to the top of your 7.15 rod. Zero Relative there and then what? What usable number can you find at that point and where? Well... there isn't one. Yet if you look at your Machine Position Display and add -7.15" to what it says, (Make more negative) that is the Tool Offset number the machine wants to know. (This technique is described using SHIFT in post 23) (End Edit.)

As far as watching Position displays. Don't get hung up on that either. I've machined thousands of jobs without ever bothering to look at position displays as in Absolute and Relative. The most important Position display to be concerned with is the Distance to Go display found on the CHECK Screen. (In Auto or Memory Mode) If you Initial Position most if not all your tools in your programs at say a common height of Z0.1 for example, and you watch the Distance To Go Display as your tool approaches the work, you will find it easy enough to see if you have things set right. If you Feed Hold the tool roughly say an inch above the work and the Distance To Go says Z-6.5 still left to go, you'll know you have something screwed up. If it looks about right, put Single Block on, hit the Green Button once more, and let the tool finish it's move in Z. Then it will be easy enough to eyeball whether the tool looks like its roughly a shallow 1/8th inch above the part or not. If so you're good to go.

I really need to get back to work. Hope this helps.

 

[solidworks4u]

Gentlemen, today the prior owner & I were at the machine trying to set "G54" to cut a simple program. After observing the mill, the prior owner stated that the "actual position" would not "zero out" when starting the program. As I understand what was described that the (upper right corner of position screen) "actual position" should be zero at the beginning of starting a program, and it is not 0.0. His thinking is that G92 is active and not allowing the data in the G54 "machine offset" screen to be accessed and that a parameter needs tweaking. I pray someone has some knowledge about this or can point me in the correct direction. Prior to today's visit by the old owner, I have been pondering, reading and viewing anything I thought may help me understand my problem better.

Many thanks in advance for any thoughts that may help.

 

[13engines]

Gentlemen, today the prior owner & I were at the machine trying to set "G54" to cut a simple program. After observing the mill, the prior owner stated that the "actual position" would not "zero out" when starting the program. As I understand what was described that the (upper right corner of position screen) "actual position" should be zero at the beginning of starting a program, and it is not 0.0.

The last part of this post is vague and can mean a dozen different things depending on point of view. Honestly, most programs start with the Z axis at the Tool Change Position and the Table forward so the Operator can reload material. Then there is the fact that few if any programs start with a Tool being brought to X0.Y0.Z0. I ask, what exactly is meant here?

Regardless... there is no "zeroing out" of the Actual Position Display. Only the Relative will do that. The only time the Actual Position Display will show Z zero, is after a tool is called and initiated using G43, and then brought all the way down to the work and touches the Z zero part Reference Surface that the job was set up for. (Combination of Work and Tool Offsets.) The X and Y will Zero when a tool is at the X and Y reference point that was set up for the part being machined.

 

[solidworks4u]

13engines, I asked the prior owner to describe what he did when at the mill, last Friday, this is his response.
After the vise was indicated X and Y zero, went to the offset screen under g54 entered the appropriate numbers let's say X -15.5 Y-7.00 Z-20.0, but the machine does not pick up the offsets and keeps using g53 machine coordinates. We tried using the same numbers in all g54-59 still the same thing. I also went to the MDI screen and entered in g54, but the machine is still looking at the g53 coordinates. What parameters control this?

Many thanks, in advance.

 

[dandrummerman21]

Does it function in AUTO mode with a registered program?

I wouldn't be using MDI for anything related to going to a work coordinate.

Make a program like this:

O1234
G90G80G40
G54
G0X0Y0
M30

What does that do?