2 Files in NC format....How to change...

[MarcoKnjaschewitsch]

Ok so my question is how do i change my X and Y Reference points on my machine as it is at the outter egde of home...As X=0 Y=0 at the home position of the machine but my machine references the pins at x=120 and y=49... do i have to go through each line and change the co ordinates?????

[Jody Wilmes]

Typically, you would use your G901 fence location (pop-up pins) in the program.
Then add in an Xshift and Yshift commands.
This will shift the current G901 location towards HOME by the amount that you specify. Below is a sample if I were using a 4x8 sheet;

Code: Select all

G90
SET WASTEBOARD=0.2550
G901
SET ZSHIFT=0.7500+WASTEBOARD
SET XSHIFT=96.0000
SET YSHIFT=48.0000

[MarcoKnjaschewitsch]

So if i wrote code like this would this work to shift the axis???

M98PSTRTTIME.SUBL1
M48
G90
SET ZSHIFT = 0.867
(Enter Material Thickness)
SET XSHIFT=120.0000
SET YSHIFT=49.0000
G09F8
G52L1
T1 M3
S15000

[MarcoKnjaschewitsch]

M98PSTRTTIME.SUBL1
M48
G90
SET ZSHIFT = 0.7500+ what i figure my waste board is
(Enter Material Thickness) This material thickness is left the same???
SET XSHIFT=120.0000
SET YSHIFT=49.0000
G09F8
G52L1
T1 M3
S15000

[Jody Wilmes]

Nope. The X and Y shifts will only work with a G901 or G902. It looks like you are using a G52L1. You can either;

Change the G52L1 to G901
Or adjust the G52L1 offset and remove the X and Y shift from your program. I would choose the first method as long as your G901 is setup correctly...which I believe we setup here at the factory.

[MarcoKnjaschewitsch]

If i put the G901 in and the prog what could be not setup with it? What would be a result perhaps?(Dont want to wreck the machine really lol)

So if i wrote it as :

M98PSTRTTIME.SUBL1
M48
G90
SET WASTEBOARD=0.2550
G901
SET ZSHIFT=0.7500+WASTEBOARD
SET XSHIFT=120.0000 (We have a 5x10 Table)
SET YSHIFT=48.0000
G09F8
G52L1
T1 M3
S15000

Would that reroute where its start point would be for the one piece????

[Joe Soto]

The G52L1 location would be used because it is after 901 and axis shift. You need remove the G52L1 for this to work. What you have now is


G901 (moves X0,Y0 to pop up pin location)
SET ZSHIFT=0.7500+WASTEBOARD
SET XSHIFT=120.0000 (We have a 5x10 Table) (moves X0 120 back towards home)(Axis Shift moves the zero location/fixture offset to the corner of the sheet, closest to the HOME position of the machine)
SET YSHIFT=48.0000 (moves Y0 48 back towards home)
G09F8
G52L1 (moves X0,Y0 to fixture offset #1)This will be the offset used because it is the last one control reads before any movement.
Hope that helps, Joe

[MarcoKnjaschewitsch]

ah that makes sense...thats what i get for writing this at 11am in the morning on a Sunday haha...I remember him saying thats what it was for in a post before lol

[Dennis Englert]

On a machine equipped with locator pins, the X0 and Y0 locations are normally located in the opposite corner from machine home. This location is specified in a program with the G901 macro. If you use the "Part Locator" (L-shaped fixture) for locating parts for flip-ops or other reasons, then the location is G902. The SET XSHIFT and SET YSHIFT commands move the zero coordinate by the specified amount towards home. Therefore, an XSHIFT of 120 will move the X0 location towards home by 120 units or inches.

One critical item that I note in the previous thread is the SET XSHIFT and SET YSHIFT statements must be above the G90? series macro, so should read:

G90
SET ZSHIFT = ##
SET XSHIFT = ##
SET YSHIFT = ##
G901
T# M03
S18000

The AFL shift commands for X and Y can be swapped, but must be above the G901. The ZSHIFT must always be above the tool call. If this sequence is not followed then the SHIFTS are not applied. With the X and YSHIFT, you'll probably get an out-of-bounds indication and you may with the ZSHIFT, but as Murphy's Law does still exist, if you don't shift the Z axis up for the material and wasteboard thickness, then you will be boring into the wasteboard and the spoilboard by your depth of cut settings.

There should be pertinant material regarding this subject in both the User's Manual (hard covered blue book) and the Training Guide that you received.

You can also use the G52L# fixture offset code, but it does not work with the SET XSHIFT and SET YSHIFT. If you prefer to use the G52L# fixture offset codes, tere are another set of AFL statements to be used. Example as follows:

G90
SET ZSHIFT = ##
[ADJFIXOFF, 1, -120]
[ADJFIXOFF, 2. -49]
G52L#
T# M03
S18000

Again, the AFL statements are above the fixture offset codes. The AFL statement must be enclosed by square brackets "[ ]", not parenthesis. The 1 and 2 represent the X and Y axis, while the values 120 and 49 represent the amount of adjustment on each axis. If the G52L# fixture offset represents the same corner as the G901, then the offset would be reduced towards home, thats why the value is represented as a negative.

[MarcoKnjaschewitsch]

Ok So it moves now to the right end of the field but being that it is Working from the 0.0 Point it goes off the table????? Heres some lines and it i think would have to reference 0.0 As the center of the work piece which would be 18" Overall so 9" center...Now How do i shift in the x,y cords so it does not run off the table???




T1 M3
S15000
(0.125 inches dia. slot drill)
G0 X0.0000 Y0.0000
G00 Z0.5000
M31
G00 X10.8817 Y15.9619 Z0.5000
G01 Z-0.1250 F10.0
G01 X10.8817 Y15.9619 Z-0.1250 F50.0
G2 X10.8690 Y12.2200 I-1.8808 J-1.8646
G2 X7.1270 Y12.2259 I-1.8680 J1.8774
G2 X7.1183 Y15.9619 I1.8684 J1.8724
G3 X2.1144 Y6.8580 I1.8966 J-6.9696
G3 X7.5507 Y1.9340 I6.9060 J2.1615
G3 X16.0111 Y7.3345 I1.4428 J7.0669
G3 X10.8817 Y15.9619 I-7.0175 J1.6664
G00 Z0.5000
G00 X9.3645 Y16.8374

[Dennis Englert]

The important part of the program is above the lines that you sent me. Per the example provided before you need to have your fixture offset information above the tool number to shift the X and Y axis.

Example:

G90
SET ZSHIFT = your material thickness
SET XSHIFT = Material length
SET YSHIFT = Material Width
G901

The text in the example goes above your tool call.

[Dennis Englert]

Marco,
Also, please contact our tech services via Virtual Service. They will be able to verify that the G901 is setup and will also be able to review your program. Plus talking to each other live would certainly be a quicker solution to this two day puzzle for you.
Dennis