Setting G28 Points

[CHampshire]

Hello Everyone. I have a quick question on how to set a Reference point on my mill. It is a Bridgeport with a Fanuc OM control. I want to set a reference point at the front so that the mill returns in the middle of the door for easy unloading. I have already figured out that G28Y0 will bring the table all the way forward, But X0 is table all the way to the left.

Is there a way to set say, G28P1, where the p would be reference point 1? If so how would I go about doing this?

Thanks for any help!

[dcoupar]

There is a G30 P2 (2nd Reference Position), but it's an option, and you may not have it.

You can try to MDI G30 X0 and see if you get an alarm.

The other option is to use the G53 Machine Coordinate System. If your machine has 30" travel in X, and you want to center it, use:

G00 G91 G28 Y0 (Y-AXIS HOME)
G53 G90 X-15. (X-AXIS CENTER OF TRAVEL)

[angelw]

Originally Posted by CHampshire Hello Everyone. I have a quick question on how to set a Reference point on my mill. It is a Bridgeport with a Fanuc OM control. I want to set a reference point at the front so that the mill returns in the middle of the door for easy unloading. I have already figured out that G28Y0 will bring the table all the way forward, But X0 is table all the way to the left. Is there a way to set say, G28P1, where the p would be reference point 1? If so how would I go about doing this? Thanks for any help!

G28 corresponds to the first Reference Point and that's the Zero Return position of the machine;this can't be arbitrarily changed. Your control should have G30 for 2nd, 3rd and 4th Reference Points, depending on the model of the your OM control. If its a model A, you may only have one G30 available. G30 is often used when your tool change position is different to the Reference Point, so if your machine has a tool changer, make sure you don't conflict with it's G30 position if used.

You have to set a parameter for the 2nd Reference Point position. For the 2nd Reference Point in X its parameter 0735. Set this to the distance from the Reference Point of the machine to your desired 2nd Reference Point. Include the "-" sign if its a minus direction from the Reference Point. This function is available after power is turned on and Reference Point return is performed.

Its a good idea to use G91 with both G28 and G30. Both of these functions go to their respective reference points through an intermediate point. G28 X0.0 or G30 X0.0, if G90 mode is in place, will go to the X0.0 point of the work before going to the Reference Point, whereas G91G28 X0.0 or G91G30 X0.0 will got directly to the respective Reference Points.

If your control has more than one G30 Reference Point available, the 2nd, 3rd and 4th Reference Point is selected by G30 P2, P3, or P4 respectively. If the P is omitted, the 2nd Reference Point is selected.

Regards,

Bill

[angelw]

Originally Posted by dcoupar There is a G30 P2 (2nd Reference Position), but it's an option, and you may not have it. You can try to MDI G30 X0 and see if you get an alarm. The other option is to use the G53 Machine Coordinate System. If your machine has 30" travel in X, and you want to center it, use: G00 G91 G28 Y0 (Y-AXIS HOME) G53 G90 X-15. (X-AXIS CENTER OF TRAVEL)

Sorry for cutting in dcoupar. I was still typing when you made the post.

All of my manuals show G30 2nd Ref Point as a Basic function, even on the A model.

Regards,

Bill

[CHampshire]

Thanks for the quick replies guys. I will give your suggestions a try tomorrow and let you know what I come up with.

[dcoupar]

Originally Posted by angelw Sorry for cutting in dcoupar. I was still typing when you made the post. All of my manuals show G30 2nd Ref Point as a Basic function, even on the A model. Regards, Bill

Thanks for the heads up, Bill. I don't know why I thought it was an option...

Keep up the good work,

Dave

[yoshi900]

I use the G53 method also. "G0 G53 X16. Y0"

My mill has the umbrella type toolchanger. With the usual "G0 G28 Z0" at the end of each tool, it has to come back down like 4 inches for tool change. waste of time. So I use this instead "G0 G53 G49 Z-4.5866", saves another 2-3 seconds at each toolchange.

[CHampshire]

Hey guys. I figured I would fill ya in on what I did. Ended up trying the g53 x-(value) y0 and it worked like a charm. Quick and easy to do. I also went in and changed my post so that from here on out all programs will have this move at the end.

Thanks for the quick responses and all the help. Its the little things like this that make it easier for everyone!

[stevo1]

Originally Posted by dcoupar Thanks for the heads up, Bill. I don't know why I thought it was an option... Keep up the good work, Dave

Dave,
I would have ass u med the same thing. I am not positive on the Oseries control but I know on the 10,11,12,15 series that I have set up that these are options that need to be set in order to get the 2nd, 3rd, 4th reference positions. IIRC I also saw these settings in the Oseries but I am not 100%.

Stevo

[angelw]

Originally Posted by stevo1 Dave, I would have ass u med the same thing. I am not positive on the Oseries control but I know on the 10,11,12,15 series that I have set up that these are options that need to be set in order to get the 2nd, 3rd, 4th reference positions. IIRC I also saw these settings in the Oseries but I am not 100%. Stevo

Stevo,
That's correct with the 10 - 15, but the OP was referring to an O series, and G30 was a basic function for that control; see attached pdf.

scan0006.pdf

Regards,

Bill

[stevo1]

Originally Posted by angelw Stevo, That's correct with the 10 - 15, but the OP was referring to an O series, and G30 was a basic function for that control; see attached pdf. Attachment 129153 Regards, Bill

Great information, good to know. Thank you.

What is odd is on my options list I see the 3rd, 4th reference position in the 900 parameters for the Oseries. I am wondering if maybe the 1st and 2nd are standard and the 3rd and 4th are options. I looked at the PDF and my G-code lists for the 10-15series also list the G30 on the standard list but they are still an option. So I would assume that just because it is on the G-code list does not mean it is a standard code yes?

Stevo

[angelw]

Originally Posted by stevo1 Great information, good to know. Thank you. What is odd is on my options list I see the 3rd, 4th reference position in the 900 parameters for the Oseries. I am wondering if maybe the 1st and 2nd are standard and the 3rd and 4th are options. I looked at the PDF and my G-code lists for the 10-15series also list the G30 on the standard list but they are still an option. So I would assume that just because it is on the G-code list does not mean it is a standard code yes? Stevo

All of what you say is correct Stevo. The documents I have show only the 2nd reference point for G30 as being standard, and there are only parameters available to set the one (2nd) reference point for X,Y,Z,4th.

Reference to G codes as shown in most Fanuc manuals doesn't necessarily mean that they are standard. The list that I have show those G codes that are Basic and those that are Options.

Regards,

Bill