Help with G28, G52-59

[Vortex_bits]

Hello, I'm working with two machines, but basically the same fanuc 180i controller, and have some questions. When the machine uses G28 (Automatic return to reference point), what reference point is it returning to? Is this from the factory home point, or a point that is set up in the controller?

G52-59 I know how to use the normal G54P00 area to move to a different spot on the table, but what if I have a specific program that I always want to cut at a specific spot every time? Do I set up a measurement in the G54P## area to refer to, or how does that work? For example: Most of our nests start at the 0,0 point, but I have a bit diameter check program that I want to be cut in the upper left corner .. say X0 Y58. Can I add a command to the post that will call G54P48 and in the G54P48 slot I'll have the co-ordinates of X0 Y58 Z0. ?? Also, since we use our G54P00 Z to add in our spoilboard thickness, how would that affect such a move?

Also, as a bonus question, the material we use varies about .03" or so, and it's a pain to adjust all the tools when the material is different thickness than what the program calls for. Is there a way to make the programs check one of the work co-ordinate spots for a number that will determine how much farther down or up to go, compared to what the program is calling for?

For example: All our 1.125" material is really about 1.235" (after pressing), but sometimes it's thinner laminate at about 1.2". So if I measure it, I could put a value of -.035 in the controller so that the tools will adjust that much to make up for the difference in actual thickness. Is that possible?

Thanks in advance!

-Zak

[Geof]

I use Haas operating in Fanuc mode and I think the following comments are applicable to most VMC controllers.

Regarding G28 this takes the machine home to the zero position in machine coordinates. You write; (Automatic return to reference point), are you sure it is to not through? On a Haas if I just do G28 it will send all the axes straight home; but if select an axis such as G28 X I have to put a coordinate after the X like G28 X0.0 and in this case it first goes to the X0.0 position in the active Work Coordinate system then goes home. This can be a nuisance so it is b est to program G91 G28 X0. or whatever axis you are sending home and the incremental command of zero means it goes straight home.

For your bit diameter check you could program using G53. This is the machine coordinate system so if you have G53 X-16. Y-9. Z-10. it will always go to that machine position no matter what Work Coordinate system you have active. The G53 is non-modal so you need it on every line in the routines using G53, and it does not affect anything else.

For your thickness adjustment why not just modify your Z coordinate that is used fo the spoil board thickness?

The only other way I know to put in a quick Z adjustment is to use G52 Z-.035 at the beginning of the program. This moves all the Z positions down by that amount. But this is in the program not an entry into the controller.

[MazakMikeO]

Do you not have a 00 or common offset alongside g54-59 on the offset page? Any value you put in this offset will adjust all the other offsets 54-59, by that amount. You could put a Z offset in this offset, and it will change them all.

[little bubba]

I'm assuming whatever you are doing is referenced from the top of the material, engraving or something.

How about set all your tool heights to whatever your material is sitting on, and then measure the material, and put that as your Z offset.

[Vortex_bits]

Originally Posted by Geof I use Haas operating in Fanuc mode and I think the following comments are applicable to most VMC controllers. Regarding G28 this takes the machine home to the zero position in machine coordinates. You write; (Automatic return to reference point), are you sure it is to not through? On a Haas if I just do G28 it will send all the axes straight home; but if select an axis such as G28 X I have to put a coordinate after the X like G28 X0.0 and in this case it first goes to the X0.0 position in the active Work Coordinate system then goes home. This can be a nuisance so it is b est to program G91 G28 X0. or whatever axis you are sending home and the incremental command of zero means it goes straight home.

yes, our post usually calls out something like G91Z0;G28X0Y0, but I want something more like G91Z0;X0Y15. Because the gantry gets in the way of the Dekker when it returns all the way home, so I want it to return 'almost' all the way home after a program. That will make changing tools easier also. I think I've tried G91Z0;G90X0Y15. but I can't remember the result. Another thing I'm wondering, is that our KOMO goes ALL the way back up in-between drills, which I feel is alot of un-neccessary work and time. I figure as long as my safety plane is good, it should be able to stay down while it switches drills.. but it calls a G28 code also for the Z axis I believe.. which causes this.

Originally Posted by Geof For your bit diameter check you could program using G53. This is the machine coordinate system so if you have G53 X-16. Y-9. Z-10. it will always go to that machine position no matter what Work Coordinate system you have active. The G53 is non-modal so you need it on every line in the routines using G53, and it does not affect anything else.

Does that work even if you are in Absolute or incremental mode also? Or does this override those modes?

Originally Posted by Geof For your thickness adjustment why not just modify your Z coordinate that is used fo the spoil board thickness? The only other way I know to put in a quick Z adjustment is to use G52 Z-.035 at the beginning of the program. This moves all the Z positions down by that amount. But this is in the program not an entry into the controller.

If it were me running the machines, I would, but I'm just the programmer, we have some .. untrained individuals running machines, who are constantly frustrated by having to adjust bits because of differences of thickness of material. Personally, I would just subtract or add the difference between what the material is, and what the program 'thinks' it is to the spoilboard thickness, but if someone forgets to put it back, then tries to flycut, they'll probably end up spending the next hour touching off all the bits again. Plus, anything that is a through cut will cut that much more into the spoilboard.. which they hate.

Thank you, I will work with the G52 idea. Any other ideas are very welcome!



Thanks again for the reply!
-Zak

[Vortex_bits]

Originally Posted by MazakMikeO Do you not have a 00 or common offset alongside g54-59 on the offset page? Any value you put in this offset will adjust all the other offsets 54-59, by that amount. You could put a Z offset in this offset, and it will change them all.

yes, we use the 00 common for our spoilboard thickness. What I need to do is be able to 'ADD' (actually litereally subtract) thickness from the spoilboard to make up for the difference in material thickness. So if my 00 common offset is Z0.56 and there is a -.02" difference in material thickness, I need to be at Z0.54, but I would rather keep the 00 offset the same, and just have a spot to enter "-.02" to adjust the bits that much further down than the common offset goes. It occurs to me that the fanuc controller isn't much of a calculator and is more like a spreadsheet. No dynamics here.

Thanks,

-Zak

[Vortex_bits]

Originally Posted by little bubba I'm assuming whatever you are doing is referenced from the top of the material, engraving or something. How about set all your tool heights to whatever your material is sitting on, and then measure the material, and put that as your Z offset.

Yep, we machine from the top. It wouldn't be a bad idea to do that, except that we have constantly changing material thicknesses, and we run other things like plastic, polypro, and about 5 different sizes of materials, all in the same shift. (not engraving) It would be very time consuming to keep measuring and entering Z values all day. It's not the end of the world if I can't work this problem out, it's more of just an annoyance to be constantly changing bit depths up and down. I've finally got the engineers and machinists to accept these changes as a fact of life, but the plant manager is a different story.

thanks,

-Zak

[Geof]

Originally Posted by Vortex_bits ......Does that (G53) work even if you are in Absolute or incremental mode also? Or does this override those modes?....Zak

It will work in either mode but if you want to send the machine to a specific position in machine coordinates you must be in absolute.

[Vortex_bits]

Originally Posted by Geof It will work in either mode but if you want to send the machine to a specific position in machine coordinates you must be in absolute.

Well, yeah, that makes sense. Thanks for the ideas, when I get a chance I'll try them out.

-Zak

[MazakMikeO]

G28 sends the machine to the factory home point. You could use G30 to send it to a second reference position, I can't remember exactly how you set that in the parameters though. We use this in our tool changes.