[CBNDude]

Has anyone ran a Fanuc controller with Manual Guide i ? If so can you please tell me what you liked and disliked about it. Was it easier, harder, quicker, slower , etc. to program. And type of machine. All opinions welcome please.. Thanks

[Ozemale6t9]

On lathes, I love it. On mills I think it is virtually useless.

For turning (especially mill-turn), it really simplifies programming. I have had customers who have never had anything to do with programming get up and running and confident within days of machine installation. Plus there is the added advantage of being able to convert to G-code format if you prefer that. I prefer to leave the programs in I-Guide (as I call it) format, because they usually store in less memory. You can simulate machining with the 3D graphics and the programming macros are quite extensive.

Milling I-Guide on the other hand is very basic. Only drilling/tapping functions, island milling/pocketing for basic shapes (rectangles, ellipses, circles), slotting, and simple (one depth) profile milling. Simulation leaves a lot to be desired, with the whole program being simulated with one tool size. That said, the machining centres that we have supplied with Manual Guide-I are lower end machines, so maybe they have lower end software.

regards, Oz

[TURNING MAD]

I AGREE WITH OZEMALE6T9. FOR TURNING AND MILL/TURN THE SOFTWARE IS OF GREAT USE AND VERY POWERFUL. LACKING IN MILL FUNCTIONS THOUGH, BUT STILL USEFULL IN SIMPLE THINGS LIKE MAKING FIXTURES FOR MILL/TURN WORK. THE OTHER THING TO CONSIDER IS WHAT TYPE OF CONTROL DO YOU WANT TO USE THIS ON. I USE THIS SOFTWARE ON THE FANUC 18i TB. THERE ARE OTHER BENIFETS TO MANUAL GUIDE i. IT GIVES YOU EXTREMLY FLEXIBLE EDITING CAPABILITIES WITH ALLOWING YOU TO COPY,PASTE,MERGE FROM DIFFERENT PROGRAM SOURCES AND FORMATS.ALSO THERE IS MEASURING CYCLES FOR PROBING, FIXED FORM SENTENCES FOR CUSTOM PROGRAMS,CANNED CYCLES, AND MACROS. OUTSIDE OF OKUMAS IGF IT IS ONE OF THE BEST CONVERSATIONAL SOFTWARES I HAVE SEEN. GOOD LUCK!!

[ezavarse]

I run a fanuc with Manual Guide It was hard to learn by my self does'n have information how to work with and the only information that you can find is very old and out of date the japs never uptoday the information?

[christinandavid]

Hi

My only Fanuc experience is with 31i on a horizontal machining centre. Didn't have proper manuals so have learned by trial and error. It probably helped that I was new to Fanuc and I quickly abandoned the old program format for the new cycle/figure format. The logic behind it becomes clear.

As mentioned previously in this thread, the program is more concise and easier to manipulate. Free Form figure creation is extremely useful (no calculator required).

A lot still needs to be done to improve some of the milling cycles but in general you can get them to behave the way you want with experience, and you no longer have to memorise a bunch of address codes.

I also like the intuitive file management, fixed form sentences and shortcuts to the offset tables.

DP

[sinha_nsit]

If we create a program without using Manual Guide i, can we import the program and see its 3D simulation in Manual Guide i?

[Ozemale6t9]

If we create a program without using Manual Guide i, can we import the program and see its 3D simulation in Manual Guide i?

Yes you can. You will need to insert the data for the blank near the top of the program, and also enter the relevant tool data for the simulation to work.

This simulation is no different to running a program which has been created with MGi then converted to NC.

regards, Oz

[ProToZyKo]

Hi.

Im after the same as thread starter, but im wondering what would be best, manual guide i or edgecam, mastercam, gibscam?
We usually have allot of different parts but mostly the same, just a few differences here and there. Im thinking that changing speed, feed and depth of cut would go faster on manual guide, then a cam software?
Mostly easy part's we program, but we want to be able to do some milling work, pocketing etc.
Anyone know if it's possible to import drawing?
Is writing on parts an option?
Turning of cordinate system to drill and tap with angle head?
Load monitor?
And everything else that's nice to know.

I have experience with Okuma's IGF and Fanuc's FAPT. If this is better great

Omega om80 Fanuc 18iTB

[christinandavid]

Hi,

The main differences with the 'standard' format as far as I am aware are the new display, shortcuts via softkeys and new embedded cycles. The 31i we have can be run using the original 'hard key' displays also, but I find the manual guide interface a lot more logical and user friendly.

As previously stated, the cycles are a little clunky, due to the varying opinion in previous posts my guess is that they are still being tweaked by Fanuc. The most useful cycles milling-wise are the 'partial' contours and the mega-easy 'chamfer' cycles. As others have also suggested, don't expect to get great documentation of the new functions - you will be lucky if you get anything other than the standard set of tomes.

Programs are written in what I would describe as a cycle/figure format. You can save templates (fixed form sentences) of your standard program restart sequence, and simply insert a 'cycle', be it drilling/facing/contouring, along with a 'figure' (contour/pocket shape or pattern of holes). This is all done with on-screen pop-up menus.

Drawing a contour is very similar to Heidenhain Free Contouring (but easier). Shapes can be defined with limited information, and options given when more than one possibilty exists. These can be inserted into a main program or defined as a sub program.

When these cycles/figures are inserted into the program it all looks like a load of complete gibberish gobbledygook for a while, but you do get used to it and find that you can make something of it after a while - but there is actually no need as whenever 'alter' is selected and your cursor is within the cycle the menu screens pop up and you enter the info into the boxes as before. You can also convert the program to standard G-code to run on other controls.

Yes, there are engraving cycles available (may/may not be an 'option'). The string required is inserted in the program as a comment, so if you want to create incremental serial numbering programs you will need to get your thinking cap on.

I don't believe there is a facilty to import drawing files.

I haven't really looked at tool load monitoring - but it is a separate entity as far as I am aware.

Three-dimensional co-ordinate rotation is still an 'option' much to my displeasure. If you are only working in the standard working planes, you choose the cycle to suit - I had quite a lucky escape thanks to this, when I failed to re-define my working plane - the new cycles override G17/18/19.

Powerful parametric programs can be created using a combination of the new cycles and a bit of macro b programming.

DP

[ProToZyKo]

Is it still possible to draw the whole part then choose what tool to do the different work? The one thing i love about FAPT.
Is the chamfering like mazak? When entering a 90degree mill and size it will calculate how much to chamfer?
Guess the different cycles maybe look similar to mazak when running, shouldn't take long to get used to, but if you have the opportunity to run process test and 3d graph when running there shouldn't be any problem.

[christinandavid]

Hi,

Sorry, don't have experience with FAPT or Mazatrol enough to make comparison, but it is quite simple to apply different cycles to a defined figure and likewise apply the same cycle to multiple figures. Copy/Paste is useful in that respect.

Chamfering cycles are designed for 90deg inclusive cutters, enter the diameter at the end of the tool to find tool offset, and enter the radius into the tool table as normal. Just apply the cycle to your contour, setting chamfer size and what they call the 'ejection stroke'. This bit is useful to reposition your cutter to avoid pocket walls/floors/corners - or simply to use a fresh part of the cutter.

I'm not sure if this is relevant to all control models (have also had a look at our Puma with an 0i control and there are subtle differences), but on our horizontal mill with 31i, 3D simulation is not possible while running program - only while editing.

Menu-driven Measuring cycles are also available but I don't have that option.

DP

[Ozemale6t9]

I'm not sure if this is relevant to all control models (have also had a look at our Puma with an 0i control and there are subtle differences), but on our horizontal mill with 31i, 3D simulation is not possible while running program - only while editing.

I believe this is the case with all controls having MGi. The problem is the amount of system resources required to run the 3D view. The machine is just not capable of handling the 3D simulation and the machine control at the same time.

That said, you can run toolpath simulation during cutting, which is really all you need anyway, since 3D detail is very limited if you are viewing reasonable size parts.

Another problem I have found with the resource issue is when you have a PMC controlled device, such as a tool changer, and you change to/from the MGi screen during operation of this device. Eg. if the machine is doing a tool change, and you change to/from the MGi screen, the tool sequence can get messed up. In some cases, this has resulted in incorrect tool offset data being used, and the result is not pleasant.

Operator beware...

Oz

[christinandavid]

Took me a while to get simulation working even on Edit as it was freezing up completely at every tool change - don't know whether its something in the tool change macro, but I have to remove M6s from the program to simulate it.

It also freezes the display temporarily if you search a big program in Background Edit - which can be a little disconcerting...

DP

[lil p]

hello,
this is the first time we've gotten our cnc lathe to work (Mori Seiki sl-5 with a fanuc 6tb control). the machine was built in the mid 80's. our problem and hopefully a quick one is that whenever there is a tool change the first approach is always to program zero before moving to the intended co-ordinances. there is no work shift, so i've made the zero of the program through the geometry offsets. using the X and Z co-ordinances from home to the program zero. is there anything i'm doing wrong that makes it rapidly move from home to program zero whenever there is a tool change in the program?

[sinha_nsit]

A tool-change is a tool-change only. There is no reason why the tool would move to any other position on its own, after tool-change.

[Ozemale6t9]

hello,
this is the first time we've gotten our cnc lathe to work (Mori Seiki sl-5 with a fanuc 6tb control). the machine was built in the mid 80's. our problem and hopefully a quick one is that whenever there is a tool change the first approach is always to program zero before moving to the intended co-ordinances. there is no work shift, so i've made the zero of the program through the geometry offsets. using the X and Z co-ordinances from home to the program zero. is there anything i'm doing wrong that makes it rapidly move from home to program zero whenever there is a tool change in the program?

It would be best if you could post a sample of your program so we can check it out.

Oz

[ProToZyKo]

hello,
this is the first time we've gotten our cnc lathe to work (Mori Seiki sl-5 with a fanuc 6tb control). the machine was built in the mid 80's. our problem and hopefully a quick one is that whenever there is a tool change the first approach is always to program zero before moving to the intended co-ordinances. there is no work shift, so i've made the zero of the program through the geometry offsets. using the X and Z co-ordinances from home to the program zero. is there anything i'm doing wrong that makes it rapidly move from home to program zero whenever there is a tool change in the program?

Hm im used to Mori seiki SL25m, there we had to program
G00 X200. Z50.
T0101
X### Z5.
Can't quite understand of it would move to program 0 without you writing
T0101
G00 X0Z0
If you aren't using some sub/macro to change tools.

[sinha_nsit]

Do you have 6001#5 set to 1 ?
If yes, check O9000.

[lil p]

here is the beginning.

(06-10-10 15:25)
G20
(TOOL - 10 OFFSET - 10)
(DRILL 1.25 DIA.)
G0 T1010
G97 S250 M03
G0 G54 X0. Z.25
Z.1
G99 G1 Z-3. F.01
G0 Z.25
G28 U0. W0. M05
T1000
M01
(TOOL - 1 OFFSET - 1)
(OD FINISH RIGHT - 35 DEG. INSERT - VNMG-431)
G0 T0101
G97 S239 M03
G0 G54 X-6.4024 Z.11
G50 S1000
G96 S400
G1 Z-1.715 F.01
X-6.6
G0 Z.11
X-6.2047
G1 Z-1.715
X-6.4224

[Ozemale6t9]

here is the beginning.

(06-10-10 15:25)
G20
(TOOL - 10 OFFSET - 10)
(DRILL 1.25 DIA.)
G0 T1010
G97 S250 M03
G0 G54 X0. Z.25
Z.1
G99 G1 Z-3. F.01
G0 Z.25
G28 U0. W0. M05
T1000
M01
(TOOL - 1 OFFSET - 1)
(OD FINISH RIGHT - 35 DEG. INSERT - VNMG-431)
G0 T0101
G97 S239 M03
G0 G54 X-6.4024 Z.11
G50 S1000
G96 S400
G1 Z-1.715 F.01
X-6.6
G0 Z.11
X-6.2047
G1 Z-1.715
X-6.4224

Your program looks ok, so my guess would be that it is a combination of your tool offsets and the way it handles them.

The older machines were setup to compensate for the tool offset by moving the tool, whereas the newer controls move the coordinate system.

If your machine is set to move the tool when compensating, and the tool offsets are large (eg. the distance from the home position to the work datum) then the tool will move to the X & Z datum positions when it applies the tool offsets.

I am not sure if the 6T control can be changed to move the coordinate system. I do not have manuals for it, but some of the other gurus in this forum might be able to help with that.

Incidentally, on pre-workshift machines, the procedure I used was to redefine the coordinate system at the home position, for each tool (using G50). This meant that the tool offsets were always very small amounts, and therefore no large movements when applying the offset.

,Oz