[xesxes]

Hello all, we recently purchased and got running a Ganesh VMC running the Fanuc 0i-MC Controller. Just did some training on setting work and tool offsets but something doesn't seem right to me.

Currently when I zero the machine the table moves to the front/left (front being closest to you and left being your left while looking at the machine). Which tells me that X & Y zero are in the top right corner of the table.

for the moment I was instructed to set X and Y offsets in the negative value (i.e. -22.56) So now I have the tool at G54 x0 y0, Z0 is when the tool is all the way up.

Now I was instructed to bring each tool down to my part and set it's offset to my stock, and that I will have to do this for EVERY job. This is the part that seems wrong to me. This is a very time consuming process and we are a shop that runs 1 offs all the time. Also this seems that it would prevent me from running multiple parts of varying thickness at the same time. I imagine that if the work offset screen has a text box for Z this functionality must exist.

So I set the offsets for my tools to the top of my vise jaw and tried to set the G54 Z to the top as well. But if I bring my tool down the ABS position reads -22.yada. Shouldn't it read 0 or 1 if I move up an inch?

We have a Roland benchtop mill that allows me to measure the tools and set a Z0 point for each Work Offset and the tool offsets work accordingly.

sorry for the scattered thoughts, but any insight would be much appreciated.

Thank you,
Travis

[dcoupar]

You're on the right track setting tools to a standard height. To see the correct absolute position you'll have to activate the tool length offset (G43 Z1.0 H1) and if you change the G54 Z value you should probably re-activate G54.

[xesxes]

I am for sure using G43 to call the offset of the tool loaded. but I don't know what you mean by re-activate G54.

[timlkallam]

Hello Travis , For setting the X and Y axis move the table where you want X0 and Y0 to be .

Go to the offset screen highlight X under G54 key in X0 and press the measure key ,its the soft key under the screen .
Do the same for the Y axis.
now your machine is set X0 Y0 press the position key to confirm this X and Y should read 0 in absolute mode. The measure key inputs the negitive values for you .

Now for tool offsets there are 3 different ways it can be done. Heres the way I like to do it.
You want to set all the tools to the same height does'nt matter where just the same height, some were above your part .

Place a 6'' piece of scrap in your vice for a referance
Go to mdi and call up tool 1, T1 m6 cycle start .
Tool 1 is now in the spindle .
touch the tool to the top of your scrap piece
go to the tool offset page
high light tool 1
press z
under the screen press (input c)
This will input the z value for tool 1
do this for all your tools
Now all your tools are set the same but your thinking what good is this there all set about 6 inchs above the vise.

Take the scrap piece out of the vice put in the part you want to machine.
call up tool 1
G0 G43 H1 Z0
Tool 1 should stop where scrap piece was.
Go to the postion page it should say Z0
move the tool down to the workpeice your going to machine were you want Z0 to be .
Now notice the Z value on the postion screen
Go to the work offset page
highlight the Z under G54 KEY IN THE NUMBER from the position screen
and press input ( DO NOT Press input c or measure)

So every time you put in a different part to machine clear the z offset to 0 callup tool 1
GO G54 G43 H1 Z0
touch the tool to the new part
go to the position screen and enter that number in the Z offset.

Here is a another way to do it Kentech Inc. - Real World Machine Shop Software

Hope this helps

[stevo1]

Touching your tools to 1 place is the only way to go IMO. I touch them where I am doing my work. In your case it will be the vise. Put your part/fixture height in the G54-G59 and go.

What Dave is referring to is that it sounded like you did not have your offset activated when looking at your display. The display will also vary depending on your parameter settings. You can set it so your tool offset is not displayed or when pressing reset or M30, things like that will cancel your offset.

This has been discussed many times and here is a link that may help.
http://www.cnczone.com/forums/fanuc/...g_offsets.html

There are a lot of things to take into consideration. Setting up your machine has a lot of variables and a lot of people usually refer to the only way they know how and not always the most practical. Things like reference, and home positions need to be taken into account along with GL offsets, negative offset values etc. Once you have it setup properly it will be a breeze. You have a relatively newer control so you should not have to really do anything once it is setup right.

**
Oi-mc control?? No tool probe??

Stevo

[sinha_nsit]

If you have only a few thicknesses to handle, you can use G54, G55, etc. for each thickness. Six plus 48 additional (as option) WCS are available.
To simplify coordinate setting, you can use a macro which places the WCS datum at the current tool position. Just jog the tool to the desired zero position and run the macro. The process can also be automated with probes.

Sinha

[xesxes]

Tim:
I have tried your method and everything looked good up to running the program. I would "reactivate" G54 and bring the tool down to z1 and looked great. but then when I ran the program it wanted to cut a few inches down from the machine Z0. I even tried adding G54's to the G43 commands.

Stevo:
Thank you for clarifying that. I wish i could lock the display to G54 or G55 etc. The probe wasn't offered with the machine. We bought the machine used as a bank repo. But I am working on getting a quote for one. Alternatively we are tossing around the idea of a micrometer on a fixed height block.

We have our second day of training today, this time with a person that is supposed to be more versed with the controller. Hopefully he will be able to help as well, and maybe even show me how to setup the graphics screens!

Thanks for the help guys, hopefully I can get this wrapped around my head.

[manolo23]

in setting the wcs x0 y0, and z0, this steps i hope this will help you ... when you turn on the machine automaticaly the WCS is G54 ...it was set on the machine they called it modal it will only change when you call another WCS like 55 to 59
when you set the x0 y0 just put your tool to the location you want and put the cursor on G54... type x0 or y0 then press measure ...for multiple tools leave the z on 0. of G54 , then call your t# and set every tool at tool geometry H1 for t1 so on ....when you program
ex.
T1 M6,
G0 G43 H1 Z1

dont rely on ABS position on screen it will change everytime you change your coordinate on WCS refer to machine coordinate..

[stevo1]

dont rely on ABS position on screen it will change everytime you change your coordinate on WCS refer to machine coordinate..

Wouldn't you want to know what the position is relative to the active work coordinate which is displayed in the ABS position?

Stevo

[gbowne1]

I have been using my 15M machine a lot lately..

But all along, I have been using G54, the standard.

I also do not heavily rely on the ABS position reading, but I ALWAYS look at it and I record it in my job notes.

My T1 is a 3/8" CAT40 end mill holder, standard length.

I do not have a Renishaw probe.. yet! My work area is my Kurt D675 and generally I do not have parts thicker than 0.250", so I try not to go more than 0.312" or .218", although I have some table and vise fixtures that I use too.

I do generally use one place to start any location of reference

So.. I do a quick MDI of T1 M6. Cycle Start. Then the standard G0 G43 H1 Z0 (or sometimes 1). I have used the top of my vise jaws, on either side but generally rely on my fixed jaw. So as that I don't drill or mill into the jaws or the bed of the vise, I'm always careful to set that work area up so it stays out of that area with length offsets, etc. G55 goes to my work/part surface. I know where my G53 is too. I don't think I ever put a G90 in there either, but I couldn't tell you right off.

Is there any rule to where to place G90 or when to put it in?

G10 is an oddball to me too.. same with G91.. or G92? I was always told to be careful with G10.

I checked my Z length a while back and it's pretty accurate. An old FANUC guy here told me to check it with a reference block and indicator in a collet or chuck or a 1-2-3 block, but I had used a 1-2-3 block.
I found it within .00025"

I have a lot of programs that use G83 that I originally wrote on my 11M.

I generally use some wear offsets for changing setups with the same tools.

Toolpath is verified with CGTech Vericut 6.1/6.2

I sometimes work with two vises next to each other which clamp on piece of stock or fixture.

Any ideas here?

[sinha_nsit]

...
Is there any rule to where to place G90 or when to put it in?
...

I would discuss a general rule, for those who are not aware of it:
(with reference to Fanuc 0iM control)
The G-codes have been categorized into different "groups," based on the similarity in their functionality. For example, on a machining center,
G00, G01, G02, G03, G33 belong to group-1.
G17, G18, G19 belong to group-2.
G90, G91 belong to group-3.
...
G68, G69 belong to group-16.

There is a group-0 also which contains "non-modal" codes such as G04. These codes are one-shot codes, and need to be explicitly commanded wherever needed.

At any time, one G-code from each group remains active (except group-0 codes). If you do not explicitly specify one, the default code is used.
These are modal codes, and remain active until some other G-code from the same group is commanded.

You can have as many G-codes as you want in a single block, with the restriction that two codes from the same group should not be commanded in one block (if you do that, the code appearing later is used, and the previous one is ignored).

CNC machines use word-address format, so order of G-codes in a block is not important. Thus, G01 G90 is equivalent to G90 G01.
In fact, this applies to all addresses, with a few exceptions. For example, all arguments of G65 should appear to the right of G65. But the arguments of G65 can have any order. Therefore, one should generally avoid playing with the order; place a word at its "logical" place.

You can have G90 anywhere, just do not pair it with G91 in the same block. Even if G90 is the last word in a block, that block would use G90 mode. G90 is also the default code of group-3.

There are a few G-codes which cannot be used with G91: G53, G92
If you specify G53 in G91 mode, G53 would be ignored.

This is what I interpreted from Fanuc manuals. Comments/corrections, if any, are welcome. The learning process must continue. Nobody knows everything.

Sinha

[Jake E.]

We use an Elbo Controlli Pre-setter to set our tools, but before we go it, we would set our tool length off of a flat surface (i.e. center jaw of a vise) with a 1.000"block. This would give us a tool length of -5.000 to -15.000 etc. Our Z of the part is then calculated from the top of the 1.0" block. If the top of the surface the block was sitting on, then G54 Z0 would be -1.000, where as if the Z0 was.625 below the flat surface, then the G54 Z0 woudl be -1.625, etc.

Right now, our tools are in positive lengths based off of the Pre-setter, and our Z is caluclated by, again touching off on a flat surface with a 1.000" block, but then adding the absolute value of the length of the tool, the 1.0 block and the machine position of Z ( 5.3945 (tool length) + 1.000 + 24.3568 = 30.7513) then putting the negative value of that number in for G54 Z (Z-30.7513).

our initial lines of a program would be:

T1 (Call up Tool #1)
M6(Change Tools)
G0 G90 G54 X???Y??? S2500 M3 (Rapid Mode, Absolute Mode, G54 Offsets, positioning in G54, Set Spindle Speed, activate spindle)
G43 H1 Z1. T2 M8 (Activate Tool Length, Set Tool Legnth to H1, Move to G54 Z1. (compensating for tool), call up T#2(prep move), turn on coolant)
Z.1 (move to .1" from Z0 - done to ensure proper tool positioning)
G1Z-.125F150. (feed to Z-.125 at 150 inches per minute)
X???F20.(begin cutting operation, based on geometry at set feedrate from tool).



As for the G10, we use a subprogram to write our preset tool engths and offsets into the control. The lines vary form machine to machine, but here is an example:

(PALLET #1)
(1ST OP @ B0)
G10G90L2P1X-9.3111Y-15.6495Z-18.8807B0(G54)
(2ND OP @ B0)
G10G90L2P2X-13.9782Y-3.0614Z-19.8623B0(G55)
(2ND OP @ B90)


(TOOL OFFSETS)
G10G90P001R8.4401( 3/16 ENDMILL ROUGH )
G10G90P002R8.8516( 3/16 ENDMILL FINISHER )


Some Fanuc Controllers we use the following:

#7001=-27.3264(G54.1P1X)
#7002=-22.5268(G54.1P1Y)
#7003=-21.9375(G54.1P1Z)

(TOOLLENGTHS)
#2007=6.1862(5/64ENDMILL) (T#7)
#2008=3.5519(1/4ONSRUDCUTTER) (T#8)

[christinandavid]

Hi xesxes,

I too was taught on the Haas the negative tool length method and also to set relative to each setup. What a pain, eh?

The logical way:

1. Get yourself a standard gauge length tool for use as a reference. You could just use the back end of an end mill in a collet chuck as a reference tool - but a proper one will be a known dimension to the taper gauge line.

2. Make sure this tool can reach your machine bed should you ever want to set the bed as Z zero.

3. Make a nice block/pillar for setting tool lengths on. This can be fixed in the corner of the bed. Dedicate a work offset to this block, XY zero being the tool setting position.

4. To set Z zero to the 'setting block' work offset, touch the top with the known standard length and note 'machine' position in Z.

5. The 'machine' Z coordinate you are now at minus the reference tool length can be entered as your Z work offset value for the 'setting block'. Basically if there were no tool offsets loaded (G49) and you were working in the 'setting block' work offset and told the machine to go to Z zero, the spindle nose would want to move down to the top of the block.

6. You can put a command in MDI with feed override on zero and check this using 'distance to go' value. If the 'tool setting' work offset was G59 the command would be: - G0 G90 G59 G49 Z0. The figure in 'distance to go' will be a negative amount.

Reset the control once you have confirmed this figure tallies with the figure in your tool table.

7. You can now touch on with each tool and use the same command to check the lengths. Always putting positive values into table.

When you set up a job, touch on the desired Z origin with the reference tool and do step 5, entering figure into appropriate work offset (G54-G58). If you need to reset a tool mid-batch, remember to recall your 'setting' work offset. A good thing to do would be to set up a little 'tool setting' G or M code macro program which calls up the work offset and moved to XY zero automatically, and cancels tool offsets, ready for setting.


Obviously there are subtle variations on this method (using the 'reference' coordinates is another, probably even easier, way), and as you learn the control you will find your preferred method, but it's great to be able to stick a rule next to a tool in the spindle and quickly check it to the tool table, and everything making sense. Also useful to know if you ever get a tool setter that subsequently gets smashed up...

Set all your machines up using the same reference tool and you can easily swap tools between machines, knowing the lengths will tally up.

DP

[stevo1]

Greg,
I am not quite sure what you are asking for. It appears that you have a good handle on setting up your machine and tools.

As to the G91, G10, G92.
G90 is absolute programming and G91 is incremental. If you had G54 set and you programmed G90X1.Y1. your machine would move 1” in X and Y from your G54 position. Once your tool is there and if you programmed it again your machine will not move because it is already in position. Now if you were to program a G91X1.Y1. your machine would move incrementally from the previous position. Now your machine would be sitting X2.Y2. from your G54 spot.

G10 is for data setting. It can be used for setting many things via program. If you wanted to change your G54 values on the fly while running you can do so with the G10 code. G10L2P1X1.5Y2.0 would change your G54 values to X1.5 and Y2.0. The L2 tells the control which registry to look in (L2 is for workcoordinates). P1 tells it which workcoordinate to change. P1 is for G54. If you did P2 it would change your G55 instead of the G54. This is not the only use. You can use the G10 to change your tool offsets and even NC parameters in the control.

G92 on a machining center is for shifting your position. I am not even going to explain it (unless you want me to). If you have workcoordinates then I personally see no reason to use it. I never liked G92 nor G50 on lathes. Back in the day before workcoordinates and tool offsets G50 was all we had.

Alright boys let me have it on the G92 G50 :boxing:

Stevo

[stevo1]

but it's great to be able to stick a rule next to a tool in the spindle and quickly check it to the tool table, and everything making sense.

I could not agree more. That is why I never set up a MT with large negative offsets.

Stevo

[manolo23]

Wouldn't you want to know what the position is relative to the active work coordinate which is displayed in the ABS position?

Stevo

i stand corrected ,what i mean is dont rely heavily on ABS position. ..this is the common mistake when i was new on the machine i put the value on ABS in the WCS coordinate ....when starting a new set up its not reliable to look on ABS ...i just use it for quick checking....i attentively watch the distance to go... or i zeroed the relative as well and compared both...

[stevo1]

I kind of figured that’s what you meant but I did not want to ass u me. Yes putting the ABS values in your WCS can reek havoc. Machine position is the best way to go.

Stevo

[gbowne1]

Greg,
I am not quite sure what you are asking for. It appears that you have a good handle on setting up your machine and tools.

Well, stevo. I was hoping I haven't been doing it all wrong on my 15MA. Thanks for the validaton on that point. The person who set up my control gave it the G54. I do not have G54.1 though. I also do have G55 as well as using G53.

What I'm asking for is, because I now have to train 3 - 4 operators I want to make sure I have everything right and am not doing the wrong things. I'd really like some sort of white paper, beyond the manuals, on how to do this on my 15MA including a couple of examples. I need something I can hand them when I do my training session with them on how to set the tool lenght offset and the G53, G54 and G55 with some examples.

I do look at the [ABS] and the machine coord's, etc. I have not programmed in metric. I always watch the "Dist. to Go" page. I just always like to verify things are exactly where they are supposed to be at. And yes, manolo23, doing some comparisons are nice between the modes.

Nobody knows everything, yes, but it should be better understood or described.

Will G00 work for G0? I have always used G0.

Usually, like I described, when in [EDIT] or testing in MDI or writing programs like these I usually do these things" I do all of the machine prep in the first few lines before I start any axis/axes movement, i.e. changing tools, turning on coolant, setting spindle speed, activiating spindle, spindle direction, turning on rapids and setting [ABS] or [REL] or [INC] modes. The other lines are used for the axis/axes positioning, plus adding the comments to help the operator and/or programmer understand what we're doing.

I keep all of my vise fixtures standard thicknesses and size so there is little to no variation. I usually will do any locating on pins. That is a 3/4" plate 1018 and sometimes a 4000 series steel (4130, 4140, 4340). I have a fixture reference point in that I use

I never really had a chance to use G10. But I knew that it had to use the L2 and P1 values.

On some occasions, I do also two parts with two vises. One part is running while I'm clamping or setting up the next part on the other vise. That may not be the safest or coolest thing to do but it works. While it's running the 2nd part on the 2nd vise, I unclamp the 1st finished part from the 1st vise and reload the 1st vise with new material whilest it's running the 2nd part. I never found a really good way to do that.

When I am in a G83, I generally know the length from the gage line to the tip of the chuck plus the length of the tool which I record on a setup sheet. I generally use HSS jobber length in my 14N and generally clamp to the end of the unground portion of the shank.

I never used the bed as a reference for the spindle nose/face, except for the machine home or ref. returnv or the tool change position..

Since I do not have a table/bed height that changes, I usually always work in XY.. not XZ or YZ.

I don't have a presetter either. So I use the gages I have.

[stevo1]

On the 15 series control yes G0 will work instead of G00. All the G-codes should be this way. You also don’t need trailing 0’s G0X5.000—X5. works just as well. This is not true on every control. I have seen where G00 is needed.

It sounds like you have it down pretty good. Where do you touch off your tools now? And why must you record them on a setup sheet when you have a tool offset page? How many tools do you have in the magazine? If you have the measure function on the control you can use that as well. What I would suggest is touching all of your tools off the work surface (vise face) or the table just in case you need to do an offset when there is a part in the vise.

If you offset your tools on the table face then you will need to put the vise+part height in the G54. If you use the vise top then you only need to put the part height in G54. One trick to this if you touch all your tools off the table would be put your vise height in the common work offset leave it that way you only need to put your part height in G54.

If you are going to be having new guys at the machine a setup sheet as you are going for is a good thing. Just don’t over complicate it. The 15series control is a pretty powerful control. Use it to do the work and the thinking. Also if you have a big enough magazine leave the tools in and touched off and just make a nice laminated tool list. I could really go on and on about things you can do to make it easier like having a S&F program if you are going to have designated tools in the magazine that way you don’t have to hard code the S&F.

Stevo

[gbowne1]

Stevo,

Yeah, I use setup sheets to record basically everything an operator needs to know and any pertinent information about each job.

I do have a sheet on which tooling lenth offests is recorded just so there is no confusion, incase things are changed or lost.

My ATC has plenty of tools. I keep one of each standard size CAT40 end mill holdesr, three collet chucks (ER16, ER32 and TG100) and two jacobs taper drill chuck arbors, one with my Albrecht, the other with my 14N. I have room for a couple morse taper arbors for taper shank drills. I use a lot of 3/8" and 1/2" end mills in jobs. I do lots of work which is .003" or better.

I do have the measure function. I dont know a whole lot about its use.

Where do I touch off? Yeah, it's the top of the vise jaws. I generally keep X0,Y0 of the vise on one fixed corner. I do not take the vise off very often these days, but often have another vise set up next to it.

Now I am used to the 11M and the 6M, but the 15MA is the one I am still learning. Mine is almost set up like the 150MA, in fact I could set up the 150 with the other cards I collected off eBay for it. I love the 14" color monitor.

I am thinking about using Fixture offsets like G52. I do a lot of double part fixtures, I like to be able to keep track of all my standard fixture locations. I was hoping I didn't have to sneak into using G92. I do tons of G83 peck drilling.