Newbie- Work and Tool Offsets Question

[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]

Originally Posted by manolo23 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]

Originally Posted by gbowne1 ... 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)