Problem- G53 g code need a little help is the machine supposed to move?

[woffler]

i am having a little trouble with a G53z0. should this cause a z move its in a line of code as i understand it is a absolute call taking it to mean z 0 am i correct or all wet here ? What happens is the z will move up .45 and no where in the program did i call for this move and i can't find a reason in mach three for this move either. heck i am lost sure would appreciate a ya or nay on this here deal thanks .dusty

[lsalme]

Sounds like in the program the tool is .45 below the z0 of the machine coordinates before the line G53Z0 so it would move up .45 to machine coordinate zero.

[HuFlungDung]

G00 G53 Z0 should cause an axis move to machine zero. If the machine has a homing routine, make sure that you execute it first thing after power up so that all axis are at the reference positions. For Z this usually means tool all the way up and away from the work table.

A little bigger slice of your program code might be helpful.

Also, ensure that any drill cycles have been cancelled by using a G80 in the first line (the safety line) at the top of your program. Drill cycles that are aborted may leave the controller in a state where it is ready to execute another Z axis movement as soon as any axis makes another move.

[woffler]

thanks guys i am starting to see what your saying i just could not figure out where it was coming from i see it is related to machine cooridanates and homing i will home at start up.And go from there i just knew it was the nut behind the wheel .

[woffler]

BobCAD1test two.txt here is the program file sorry i could not figure out how to do this .I think its in there but i am not sure

[woffler]

i am still a little confused lets say that the g53zo. sends the z to machine cord. 0 now you are going to have to come back down and set your z part height to 0 by zeroing your dro and then its going to rapid from that height on its next line move? I'm still missing something here .thanks

[extanker59]

Looks to me as if that first G53 Z0 is a safety move unless your machine requires it. It's not rapiding down to set your DRO. I'm not sure what you mean by that but it's not. It's rapiding down to Z.1 above the work offset G54 which you have (hopefully) already set in your offset page. BTW, that program scares the cr*p out of me. It'll probably work but those G00 moves, that don't actually move, at the start of each section are a potential crash. Maybe its just me. I would say that your Bobcam post needs a bit more work. What kind of machine? What kind of experience on CNCs?

[woffler]

i sent the program to bob cad and they are trying to say its fine it is scary .i was just trying to do a test on this software and every post does some scary stuff like rapiding at zero height and stoping and starting at each z height change.i was just looking for some confirmation it wasnt me that these post 's were a mess .i am running mach three controler on a sqaure coloum mill.the outher post i used would try to rapid at zero part height and get to cut position and then go to rapid height and then go back down to cut height.

[HuFlungDung]

Woffler,
It might help if you understood that there are two coordinate systems being used in your program.
G53 is the machine coordinate system and does not change. Simplistically, it is attached to your machine XYZ and corresponds to axis travels from the home position. So if you want to send the machine to X0Y0Z0, it is possible to do so very simply with the G00 G53 + whatever axis you want.

You can also use other values than zero if you want to part the table in a particular spot.

But, the G53 coordinate system does not typically apply to the part you want to cut. Suppose you had a piece of stock the same size as your table travels. You clamp it so that its one corner lies on X0Y0 of the machine coordinate system. If you want to take a profile cut around the outside of that part, you are screwed because you cannot back the tool off of the corner because the machine is already at max travel on that corner.

So then you must move the stock in at least the cutter radius, in order to just squeeze the tool down to graze the part.

If you think about all movements in the G53 coordinate system, then things become complex very rapidly. Now the corner of your part cannot be at G53 X0Y0 because there isn't room for the tool to do anything on two sides of the part.

So you need to offset the corner, but to keep your sanity, you'd still like to call the corner of the part X0Y0 because that is where you get to measure the print dimensions from.

The good news is that you can create a new X0Y0 point, but no longer in the G53 coordinate system, because that belongs to the machine. It is always there, unchanging.

So this is where your G54 work shift comes into use: this offsets the X0Y0 a certain distance from G53X0Y0. The controller recognizes this offset when you command G54, then it goes and looks at what is in your work shift register X,Y, Z and temporarily moves the work coordinate system to the point you have entered into the work shift register.

For simplicity sake, start with the G54 Z = 0, which means it will correspond to the G53 Z0. If you begin this way, then you set your tool length offsets as lengths measured from G53Z0 all the way down to the top of your part. This distance varies according to the length of each tool as measured from tool tip to the taper socket. But no matter, by jogging the machine in Z, you can use the machine to measure the distance of the tool from the part and that is what is important.
Line N05 calls your G54 work shift.
Line N06 calls for the length offset of T1 by means of G43 H1.
Line N07 calls for the tool to take a position .25" above Z0, but this Z0 is not G53 Z0 rather it is G54Z0 because it is the top zero of the part, not the machine. Because you set your tool length offsets to be the distance all the way from machine Z0 to the top of the part, you have effectively negated the need for a Z value in the G54 register. But the top of the work nonetheless, is still part Z0 or G54 Z0.

There are other things to understand about it, but maybe that will help you get a handle on the fact that there is one machine coordinate system called G53 and then we can shift it around and we call the shifted coordinate systems by new names, G54, G55 etc.

[woffler]

i think i understand about the machine coordinates and g53 now a little .Now lets say i home machine it sets g53 at o now i have a prt at say 3 of the table when i jog down to part height and zero my dros it outputs a g54 offset in mach three telling the machine that this is now zero it still reads what ever i came down in the machine coodinates dros .And now will it go to the rapid height i set in the program .10 and then make its xy move is this the correct order of steps that should happen.i have two sets of dros machine coord. and the offset dros . so when i jog down and zero the offset dros running a g54 it should run the program from there am i correct in this?

[woffler]

I finally got it to go like it should all the info you gave me solved my inexperience problem with the g53 and g54 .I also got a different post processer and that helped evidently i had a bad file and it is okay now thanks to all for your most kind and generous help.