[HalfRhoVSquared]

I must be missing something easy. Have a new-to-me VMC with Fanuc Oi-Mate-MB control.

First I set my all my tools' depths 3.000 off the table using a touch off gage and using the "offset" screen and matching the geom(h) values with the "Actual Position (Relative)" z-values.

Then using Tool 1 I manually jogged to my preferred XYZ G54 work origin and set the work offset using the "work" offsetting screen and changing the G54 values to match the machine coordinates.

That worked fine for Tool 1 to properly go to the correct XYZ G54 origin but when I change tools the XY is correct but the Z isn't.

I thought the whole point of setting tool length offset geom(h) values was so that when the tool changes it adjusts the work offset z value to match the difference. Mine doesn't seem to be doing this.

What am I missing here?

[rcs60]

on your work offset did you account for tool #1 tool offset length in G54 Z column

[the_gentlegiant]

The only position screen you should be looking at is the Machine Position screen. That's the one that never changes or gives false information no matter what you have entered anywhere else in the control. The number you see there is the number you enter into your tool height offset table. Forget about matching Actual Position or Relative or any of that. On my older OM control you can hit EOB and Z together then Input, and it will enter that value into the offset table for you automatically as long as the cursor is in the right position relative to the tool in play. Your machine may do the same. If you have in your case a 3" value entered in the "Shift" register, meaning the one right above G54 on the Work Coordinate screen, it will automatically add that (subtract a negative from a negative) and set your numbers as if you touched off on the table. Whichever method you use, you then take any tool and touch it off on your part again using your 3" block, or at least accounting for it. Take the difference between what the Machine Position screen says and what the tool height offset value says for the tool at hand, and that is the offset you need to put in either the Z position of the"Shift" register if you want to affect all Work Coordinates (G54-G59 etc) or put in in the Z position of say G54 if that's all you're using.

When using the touch off gauge, you always need to consider it's height in any transfer of measurement. If wrong your tools will either end up 3" above or below the part. Neither of which is correct, and one is crash worthy.

Hope that all made sense.

[machinehop5]

G92.1? to clear/cancel preset g92 emc2
https://smithy.com/cnc-reference-inf...offsets/page/4

[HalfRhoVSquared]

Not at shop so can't see machine but do I have to set work offset for every tool individually? So if I have 10 tools I have to go set the tool offset for each one and then have to set the work offset for each one? ( so have to set 20 things)

If so this doesn't make common sense because you should be able to go set all your tool offsets and then only have to set one work offset and it should remember all the other tool offsets and figure out where the tips of all the tools are relative to the work offset of the one tool that you had selected Whenever you set the work offset with that tool.

In short I want a simple and fast way to set the tool offsets with my 3.000 gauge and then my xyz work zero with my Heimer which is Tool 1.

I've looked all over for a video on this on YouTube etc but can't find anything for this old control.

[the_gentlegiant]

Not at shop so can't see machine but do I have to set work offset for every tool individually? So if I have 10 tools I have to go set the tool offset for each one and then have to set the work offset for each one? ( so have to set 20 things)

If so this doesn't make common sense because you should be able to go set all your tool offsets and then only have to set one work offset and it should remember all the other tool offsets and figure out where the tips of all the tools are relative to the work offset of the one tool that you had selected Whenever you set the work offset with that tool.

In short I want a simple and fast way to set the tool offsets with my 3.000 gauge and then my xyz work zero with my Heimer which is Tool 1.

I've looked all over for a video on this on YouTube etc but can't find anything for this old control.

Yes you set your offset for each tool. Read my last post carefully and you'll see I said nothing more or different then that. This tool setting all depends on how you're going to run your machine. If you're going to leave many or most of your tools loaded in the machine and change out only a few, you want to use what might be described as a Master System. In a system like that you have to have a repeatable place you can go to to measure your tools no matter what you have loaded vise or fixture wise on the table. Your 3" block sitting on the table is an example of that. If you plan on tearing down after each job (like I do, which isn't very common, but I have twenty year old tools that look like new.) you would instead use your 3" block on top of the actual work piece. This way you won't have to set any numbers in your "Shift" or G54-G59 Z areas, as all tool offsets will be referenced to the stock surface. Meaning stock surface is your current reference. CORRECTION: You will have to account for the 3"block. Otherwise your tools will al run 3" high above the part.

When measuring tools with your block you're entering the info (possibly using EOB / Z / Input) into the tool offset screen and looking at Z only. When using your Heimer and probing for part reference, you're looking for X and Y values to enter into the Work Coordinate areas of the control like G54-G59 and not worrying about the Z just yet.

As part of your Master System, you should also have a Z offset set or written down that you obtained off the same 3" block for your Heimer. Treat it as a another tool so to speak. Then at the beginning of each job, you measure the top of the stock with your Heimer, and enter the difference between that number (Machine Coordinate Screen Z value) and the previously measured height of the Heimer on the 3" block, (obtained again on the Machine coordinate screen Z value) into your G45 Z area, and any other Work Coordinate that you're using. If you're using all 6 offsets (G54-G59) it's simpler to enter the calculated Z offset height into the "Shift" register which should be right next to G54 somewhere. Anything entered there affects all Work Coordinates. You can even use the "Shift" register to correct things in X and Y also. Say you realized that shoot... I want to move all the programming 0.005" away from the fixed jaw in all the vises you have loaded. You could enter Y-0.005 in the Shift and it would move all your offsets (G54-G59) without having to change all of them individually.

To simplify. 3" block on table.

1) Measure all tools on block. Only needs to be done once. Look at Machine Coordinate screen and enter that Z value you find there into the corresponding area of the Offset screen. T1 into T1 (H1), T2 into T2(H2) and so on. Maybe put your Heimer offset in the highest number offset you have for safe keeping. Again you may be able to use EOB / Z / Input to enter your values instead of typing them in. (See earlier post)

2) Place 3" block on your work piece Z zero surface and measure its Z height with the Heimer. Take the number you find in the Machine Coordinate Z area and add or subtract that from what you have previously set/measured for you Heimer. More then likely you'll be looking for a positive number, because it's very likely that when you're measuring on top of your work piece you're higher up then when you measured on the table. But not always.

3) That number you now have that is staring at you from the calculator screen is the number you either put into the Z area of the "Shift" or Global Work Coordinate area, or... enter it into the Z area of any and all Work Coordinate Z areas you're using on the job. Again Work Coordinates refers to G54-G59.

Tools measured once. Work height measured for each new job and calculated difference enter as in 3) above.

Last paragraph deleted. See below.

[the_gentlegiant]

In closing. Keep in mind what I said in the first post about accounting for the 3" block. Until you get used to things, it's probably better to read the numbers on the screen directly and not account for the 3". As long as you do the same thing like using the 3" block for all measurements, you should be good.

I started new here to correct the above which is incorrect. You do need to account for the 3" block. Only in the sense that you don't use it when measuring the stock surface you want to use for your reference plain. Measure directly on the stock or part surface if possible. You can use your Heimer for this, or any tool for that matter. It will be easy to see if you want to enter a positive or negative number. Slide your 3" block up to your work piece. If the block is lower then your work you will enter a positive Z number. If the block is higher then your work you will be entering a negative Z number.

Basically all you are you're doing is telling the control what the Z height difference is between the master tool reference plain (3" block on table) and the actual part surface plain. That's what the control needs to know for every new job you put on the table.

Even if you break a tool in the middle of a job. As long as you measure the replacement tool on the 3" block as you did with all your other tools and enter its new value that you find on the Machine Position page, that new tool will go right back to machining at the correct height without changing any other numbers.

That statement tells why using the Machine Position (Coordinate) screen for all measurements is so important. Those numbers under every circumstance are always the machine's position relative to the machine's Home Position set by the Machine Tool Builder. They are untouchable. This is what makes them so safe to use. Unlike Actual and Relative Position screens which can in many circumstances become meaningless due to numbers entered elsewhere. Honestly in all my years of machining I've hardly ever looked at Actual and Relative positions anyway. Unless I'm bored and want something to watch just for the hell of it.

Hope this makes sense for you and helps you get going.

[HalfRhoVSquared]

Thx so much, let me try these things when I get to my shop.

Btw, one idea I thought of- is there a Fanuc G or M command that turns on/off a tool offset mode. IOW if the command is turned on in memory it either uses tool offset or doesn't use tool offset?

[the_gentlegiant]

There are various work coordinate shifting methods you can use that are directed with G codes, but I don't normally use them as much as others might. And until you get familiar with the basics I wouldn't advise on branching out just yet. Tool height offsets are not negotiable.

Don't forget that this is a computer and is completely lost until you tell it something. It will always need to know how long your tools are and where your work is situated in the Work Envelope. No getting around that. If you start using cutter compensation it will also want to know the diameter of your tools, but that's another story.

Make sure to see if that EOB / Z / Input thing works for you. It will save a ton of button pushing. I used my OM machine for years before I learned about it.

You do it sort of like control - alt on a computer. Roll from EOB to Z. You'll see the number (extracted from the Machine Coordinate) go into the buffer area on the screen, then hit Input and it will enter the number wherever the curser is at. If you're doing say tool 8, make sure your offset screen is showing and the curser is at T8 setting area before hitting Input. Helps eliminate button pushing errors and really speeds things up. Note that on my mid 90's OMC, this only works for tool offsets and not work offsets.

While I'm on this subject I'll go a little further. I hope this doesn't make things more confusing. If it does just forget about it for now.

If you have a number in the Z area of the "Shift' register I've been talking about, anything there will be added or subtracted form the number that appears in the buffer when doing the EOB/Z/Input thing I've also been talking about. Here's how I use that functionality.

I have a 4" tall setting device. I use it to measure my tools on the actual part surface I programmed to in Z. As I said earlier I don't use a Master System so am setting my tools directly to the current work piece. So with my tool setter sitting on my part, I put 4.0" in the Z line of the SHIFT register. This 4 inches gets automatically added to my tool length offset number I'm inputting, so for all practical purposes, the machine thinks I'm touching off on the part surface, where in actuality I'm touching off on the tool setter surface 4" above the part. Before starting to machine I have to remove this 4" from the SHIFT register or all my tools will stop 4" above the part. You can verify what's happening by looking at the Machine Position compared to what was just input into the tool length offset. In this case they will be exactly 4" difference. There are a lot of tricks you can do with a device like this. Nothing better then lying to a computer to get it to do what you want it to. :-)

[machinehop5]

Can you post a sample Program Format that you are trying to use?
Here is one from the net...its MM but, you should get the Idea of the Format for call Tool Offsets with G43 H1


this might help too
https://www.slideshare.net/MaheshNam...amming-milling

DJ

[the_gentlegiant]

HI Machinehop5,

That cheat sheet you posted is similar to what I see in post processor output. A lot of wasted space and unnecessary division of tasks. It also has a potentially dangerous thing at the end with G28. G28 is usually called in G91 Incremental Positioning Mode, but the author of that sheet didn't return the machine to Absolute Positioning Mode (G90) immediately after the G28 which leaves the machine in a potentially dangerous state. Besides, it's best to use G53Z0 to send the machine home at the end of the program. In my 20 years of programming I've entered G28 about twice. Never use it. The tool changer needs G28 but it is included in the Tool Change Macro, so there is no need to program it. The cheat sheet also uses line numbers which are a complete waste of time and memory. The only time you actually need a line number is if you have a special program line you need to go to a lot. You could put an N1 there which would make it easy to search to. The only other time you need line numbers is if you want to return to the main program from a subroutine at a certain line number in the main program. You'll need one there. Simple enough to add one as needed instead of on all lines.

TYPICAL SEQUENCE:

1) Call and label tool
2) Set up machine in safe configuration with no cycles/offsets or anything accidentally left over from previous programming. G54 Work Coordinate is buried in there but gets changed as needed.
3) Line space to add clarity to program when being viewed. Allows lines 1 and 2 to create a sort of tool header that is easy to spot while speed scrolling through the program.
4) Move machine to first position with head still at tool change position.
5) Activate tool offset while moving to clearance or Initial plain. Set Spindle Speed/Rotation Direction and start spindle. Call next tool to ready position. (This is only applicable to swing arm tool changers.)
6) Coolant on when machine is near the work. I do it here on a separate line so if I'm single blocking I can have this moment to adjust nozzles.
7) Start Machining
8) Coolant off
9) Use G53Z0Y0 to send spindle home to get it out of the way while also bringing table full forward so operator can reload vises or fixtures etc.

T9M6 (LETTER G DRILL)
G17G20G40G49G54G80G90G98

G0X5.7873Y2.283
G43Z0.1H9S2927M3T7
M8
G98G81Z-0.4R-0.035F18.
X0.2127Y-0.19
G80
M9

T7M6 (1/4 END MILL)
G17G20G40G49G54G80G90G98

G0X0.1977Y-0.19
G43Z0.1H7S5450M3T8
M8
Z-0.3
G1Z-0.4F8.
X5.7873F21.6
G41Y-0.32D7
X5.7973F5.8
***Blah-Blah-Blah***
G3X0.0727Y2.283I0.J-0.14F5.8
X0.2027Y2.153I0.13J0.
G1X0.2127F54.
G40Y2.283
G0Z0.1
M9

T8M6 (NO 35 DRILL)
G17G20G40G49G54G80G90G98

G0X0.2Y2.3455
G43Z-0.035H8S5500M3T15
M8
G99G81Z-0.558R-0.35F22.
G91X0.2K28
G80
M9
G0Z0.1
G53Z0.Y0.
M30

Hope this helps.

[machinehop5]

That cheat sheet you posted is similar to what I see in post processor output. A lot of wasted space and unnecessary division of tasks. It also has a potentially dangerous thing at the end with G28. G28 is usually called in G91 Incremental Positioning Mode, but the author of that sheet didn't return the machine to Absolute Positioning Mode (G90) immediately after the G28 which leaves the machine in a potentially dangerous state. Besides, it's best to use G53Z0 to send the machine home at the end of the program.

Agreed. Very sloppy programming example...Line 5 was my point. Of coarse if there were no Line numbers we would not know where we are talking about in the program. Got to save space right?

[the_gentlegiant]

Of coarse if there were no Line numbers we would not know where we are talking about in the program. Got to save space right?

99.999% of the time I'm not discussing programs with another person. Especially online. So not knowing line numbers is a mute point. If I were talking to a fellow worker we would likely be talking about how we're running a certain tool more then a specific line in a program. I will admit that I tend to work alone, so in large companies maybe line numbers have more meaning. I wouldn't know.

But hey... this is the Fanuc forum. Anyone who knows anything about a Fanuc Controls knows memory is hard to come buy. Ixnaying line numbers is what method to fight that. :-)

[machinehop5]

N10 T9M6 (LETTER G DRILL)
N20 G17G20G40G49G54G80G90G98

N30 G0X5.7873Y2.283
N40 G43Z0.1H9S2927M3T7
N50 M8
N60 G98G81Z-0.4R-0.035F18.
N70 X0.2127Y-0.19
N80 G80
N90 M9

N100 T7M6 (1/4 END MILL)
N110 G17G20G40G49G54G80G90G98

N120 G0X0.1977Y-0.19
N130 G43Z0.1H7S5450M3T8
N140 M8
N150 Z-0.3
N160 G1Z-0.4F8.
N170 X5.7873F21.6
N180 G41Y-0.32D7
N190 X5.7973F5.8
N200 ***Blah-Blah-Blah***
N210 G3X0.0727Y2.283I0.J-0.14F5.8
N220 X0.2027Y2.153I0.13J0.
N230 G1X0.2127F54.
N240 G40Y2.283
N250 G0Z0.1
N260 M9

N270 T8M6 (NO 35 DRILL)
N280 G17G20G40G49G54G80G90G98

N290 G0X0.2Y2.3455
N300 G43Z-0.035H8S5500M3T15
N310 M8
N320 G99G81Z-0.558R-0.35F22.
N330 G91X0.2K28
N340 G80
N350 M9
N360 G0Z0.1
N370 G53Z0.Y0.
N380 M30

That is a good example program you posted....Just in case you need Line numbers to help HalfRhoVSquared with their problem I added the sequence numbering.
I'll butt out ...and move on. You guys will figure it out. Good Luck on the adventure
DJ

[the_gentlegiant]

Fancy numbers you got there. : -)

I just noticed that I forgot to return to Absolute Mode after the Incremental repeat cycle in the last drill. Bad-bad-bad. Looks like we need a N345 G90. Damn.

Ahh... I just noticed why. I didn't copy over the complete cycle. Had some more holes that followed including the missing G90. Oh well.

BTW - Nobody owns this space on the www or this thread. You're as welcome as anyone to chime in any way you see fit. Can't speak for the OP, but I certainly gots no problems.

[HalfRhoVSquared]

Thanks for all the advice, especially gentlegiant for your lengthy responses. I finally got it figured out I think As you pointed out I think the "relative" numbers were messing me up so I started using just the machine coordinates and that helped.

The guy that sold me the machine had a few videos and one of them he said that he always writes in the following, even when making a simple EOB command input to move the machine somewhere: G0 G90 G54. I know what each of these does and they're all modal commands. When I go to the program screen it lists a bunch of commands that are in the modal memory. My question- if these three commands are already in modal memory then why do I need to write them again? Of course I will put them in to be safe when I write a program offline because I won't know what's already in the machine, but did he recommend this when you're working real time in front of the screen just because it's a good habit or is there another reason?

Another thing he said was that when you put in a zero you need to put in a period after it. Like "G0X0.Y0." rather than "G0X0Y0". I tried both ways and it works. On my CNC router I can even go G0XY and it works without putting any zero in at all (the Fanuc doesn't work this way though). Is there a reason to put the dot in or is that again just good practice?

Now I'm working on trying to get the Titan DNC I bought to drip feed to my Fanuc. One video I watched recommended setting the baud rate to 19,200 for speed and better 3d toolpaths. Any tips on changing the parameters in the Fanuc control. This one scares me since I don't want to mess anything up.

And any tips on how to save the parameters I have to the Titan DNC before I start changing them? Apparently the DNC will upload them. Again, I don't want to erase my parameters! <yikes>

Thanks again so much- this forum is great!

[the_gentlegiant]

In MDI there is no technical need to always reloading Modal commands. It's just whatever you feel comfortable with. The sample programming I gave you earlier has a lengthy safety header that also loads things that are likely on already, but those first five or so lines and spaces up to the M8 or drill routine header are either entered automatically at the head of my programs, or copy and pasted as I'm writing them. I program semi-manually so lots of copy and paste. You could easily incorporate the tool header into your post processor. Anyway... back to my point. You might be surprised at all the things that may happen between one tool change and another. An interruption. A quick jump to do something else. Some MDI or manual work. You just never know. That header ensures that no matter what was going on before that tool starts to work, the machine is in a known, practical and safe state to start from. But no I would never enter all that manually.

0 is the only time you can let a dot go. But it is good practice to always include it. About the only time I ever leave it out is when sending the machine home with G53 moves like G53Z0Y0. Even then out of habit, I many time include the periods.

I also always include 0 before a coordinate. Like X0.403 - I think it makes it much easier to read and gives the right visual space. Lone periods can easily get lost or go unseen. Maybe it's my previous 30 years in the printing industry where I saw a lot of Typography and had to consider how words or numbers looked on the page. I don't know.

Fanuc controls like 4800 and 9600 speeds. Your machine has an input buffer that stores a certain amount of code. I really doubt you're going to drain the buffer with your tool paths even at those speeds. You could try the speed right above 9600 and see how that goes. You're right it's a parameter change. Download the Parameter and Operations Manual for your control off the www. In one or both of them will be the instructions on how to back up your parameters and how to change them. It's very easy, but each control can be slightly different. Plus you really should have these manuals and learn where to go for needed information. Don't forget you read the 8 bit Bytes from right to left. Many time parameters are written like 1004.6 - This means bit 6 of parameter 1004. Bit 6 is the next to last position on the left. Bit 0 is first on the right. 76543210 - like that. So setting bit six to 1 would look like 01000000.

Parameter changes should only be done with a definite purpose in mind. You must know before hand exactly what you're changing. In short, you never ever "play" with parameters. Keep very clear records any time you change them.

Here is a great website with a bunch of stuff that will likely help you over the years. Dig around and you'll find a wealth of information.

CNC Machine Tool Help | Learn CNC | CNC Programming | Learn cnc | CNC Training information and CNC articles

Good luck. Fun isn't it?

[the_gentlegiant]

accidental double post

[HalfRhoVSquared]

Getting better at running my machine. One thing I haven't figured out though... after I zero all axis then I can rotate the umbrella toolchanger one tool at a time by pushing the button. This lets me unload tools by hand without having to do a toolchange. I do this to take them out and clean/dry/oil them so they don't rust inside the collet mating surface.

But as soon as I move my Z axis I can't index the toolchanger anymore unless I re-origin all the axis. Is there a command to go to Z home or somewhere that will allow my toolchanger to be indexed manually again?

[the_gentlegiant]

There are a couple ways. I like the first one as it is safer. Though it may or may not turn on your Z Home light.

Try

G53Z0.


If that doesn't work try

G91G28Z0.
G90