[2013Asadi]

Hi,

I was doing a Facing Operation (lathe) in Manual Guide i. I am having trouble facing the part over the center line (axis of revolution) so it wouldn't left any burr.I had tried try to offset the start point to -5.0 DX in the ZX PLANE TURNING FIGURE and face the part. But Manual Guide i wizard doesn't seem to face the part over the centerline.

Any idea to overcome this or is this the limitation of MGi? I have no problem programming it in ISO G-Code. The reason i started using MGi is i wanted to give training to a new guy in my shop and MGi is much easier to learn than ISO programming.

Thanks.

[fordav11]

MGI is really long-winded and annoying to use.
it would be better to write the program with G72 & G71 and use MGI only to get the XZ profile coordinates which are then inserted into the G71.
Or use some PC-based CAM software that will do the job properly and isn't annoying to use ;-)

anyway if you must use MGI, follow the procedure attached, but instead of the example end point DX=20 put DX=-2.0
if that doesn't work come back here and let us know what it did (assuming this is different to how you are programming it)

[2013Asadi]

Yes. I did put -2.0 DX and it still only facing until DX 0. It still behave as if it will only turn only to centerline DX0.

BTW,i am curious how u mix G72 and MGi XZ profile? All i can find at Fanuc website is this function of Manual Guide Oi:

Easy Contour Figure Entry

A contour figure in turning or milling consists of lines and arcs. Guideance screens simplifies the generation of these contours with advanced figure calculation functions (11 calculation functions can be performed) and then suitable G-codes (G01/G02/G03) is generated.

Thanks

[fordav11]

your last statement gives you the answer.....
"and then suitable G-codes is generated"

put depth of cut at 50mm then create the single pass cutting with the required tool.
Copy the G-code and paste it into a G71.....

I write most of my programs that way it saves memory and is easier to read.

[uperez]

it will not go down below x0 even if you write a negative value. what you need to do is to define that line as blank (there's a selection between blank or part for an attribute) then the machine knows to compensate the tool radius registered in the tool offset.

ex,
start point x0 z2,
line left z0 (define as blank)
line up x? (define as part)

not sure though why you're facing from center out?

[dcoupar]

Yes. I did put -2.0 DX and it still only facing until DX 0. It still behave as if it will only turn only to centerline DX0.

BTW,i am curious how u mix G72 and MGi XZ profile? All i can find at Fanuc website is this function of Manual Guide Oi:

Easy Contour Figure Entry

A contour figure in turning or milling consists of lines and arcs. Guideance screens simplifies the generation of these contours with advanced figure calculation functions (11 calculation functions can be performed) and then suitable G-codes (G01/G02/G03) is generated.

Thanks

Here's an example I just ran through my EZGuide-I (Doosan's MG-I). It faces past center.

[2013Asadi]

it will not go down below x0 even if you write a negative value. what you need to do is to define that line as blank (there's a selection between blank or line for an attribute) then the machine knows to compensate the tool radius registered in the tool offset.

ex,
start point x0 z2,
line left z0 (define as blank)
line up x? (define as part)

not sure though why you're facing from center out?

Well,i don't use nose compensation in ISO programming, that why I need to lathe off the burr.It always will have some burr if u don't lathe it below center (negative DX).Or am i missing something with the nose radius compensation in MGi?

[2013Asadi]

Here's an example I just ran through my EZGuide-I (Doosan's MG-I). It faces past center.

Will try ur example.

[uperez]

Well,i don't use nose compensation in ISO programming, that why I need to lathe off the burr.It always will have some burr if u don't lathe it below center (negative DX).Or am i missing something with the nose radius compensation in MGi?

the machine always use the nose compensation when you use the MGI, so you have to have the correct radius in the register against your actual tool. it also uses the tool angles set in your tool shape to calculate the actual path, if you don't set it the machine will do any shape even if its impossible to the insert you use.

[2013Asadi]

Hi
I try the example given by dcoupar.
It will go over the center after i have put in the tool nose radius and set the tool nose orientation. I guess this is what MGi required. The question now is no matter how big the negative DX u give (eg: -10mm DX) it will only go down to double of ur tool nose radius (eg:0.8 nose radius,i will go down -1.6mm max)

Thanks.

[fordav11]

double the nose radius below X0 is correct behavior and is enough.
I don't see why you would need to go more than that when facing?

[2013Asadi]

BTW,Do you guys use G54 offset for Fanuc Lathe? Currently i always touch of all of my tools when i program a new part.

Thanks.

[fordav11]

G54 is the default workshift used. for normal turning G54 is enough. if you are doing only first side of a part you dont even need to specify a workshift because on power-on G54 is current.
you only need more workshifts if you are doing more complex operations (turn/mill etc), or doing both ends of a part using multiple workshifts to shift the zero on the 2nd end and/or have 2 chucks. there are other reasons to use more workshifts but all of them are more complex than standard turning of first side of a part.

as for touching all tools on a new part, you only need to set tools if they are not set (i.e. not in the machine and not already set)
if tools are set you can use them as-is without doing anything.
all you need to do is set a new Z workshift, add some wear offset to each tool (for safety to avoid scrapping the 1st part) then run the new program.

[2013Asadi]

Guys, a little off topic. Do you guys have any idea on what the RESIDUAL MACHINING in MGi does?
I can't get to make it working.

[fordav11]

it is used to turn out a section of an undercut or pocket that a standard tool can not reach due to tool angles.
because the function is very simplistic its uses are limited. it is better to draw the area you need to machine (the missed part of the pocket) then use a different tool (such as a left hand turning tool) to machine it.