Need Help!- G54 explained

[hackmeister]

Hi, I'd like to get a good understanding on how the G54 coordinate system works. Any online tutorials? I'll need something with drawings so I can comprehend it.
I'm running a Doosan Puma 280 tuning center with a fanuc controller.
I am familiar with G, and M codes ,but just have not yet been able to fully understand how the machine "knows" where the tool is in relation to the part using the G54.
I just got a job where I'm going to need to know this.
I also need info about how to use the Q setter. It's been years since I used one,and the shop I'm at does not know how ,or even want to use it. It seems to me that the Q setter should help set up times get quicker.
Thanks in advance.

[Jim G]

G54 is an offset to the machine home position.

For a mill:

Call the lower left corner 0,0 machine home with a table that's 20" x 16".

If you wish to indicate your part 0,0 to the center of the table, then your G54 offset (shift) will be x+10.000, y+8.000.

Whenever your g-code program goes to a position, it will add +10.000 to your x & +8.000 to y.

It's really handy if you have multiple parts.
You can indicate 0,0 on each of the parts and set the offset to G54, G55 etc.

The hole locations, and thus G00 X Y would still be located in relation to 0,0 on your part.

I made a quick drawing, put cnczone isn't letting me attach it.

[dcoupar]

On the Doosan machines, when you "home" the machine (REF. RTN), the Machine Position display will usually show some fairly large numbers.

The machine postition at X home should be the diameter at the centerline of the ID holders. So, if you index the turret to an ID holder and handle X down until the machine position shows 0, you should be on center. On a Puma 280, it's about 16.535" This way, your drills should always be programmed to X0, and you shouldn't need any X geometry offset.

As close as I can figure, the machine position in Z is the distance from the face of the spindle mounting face to 1-1/4" from the qualified surface of an OD turning holder. On the Puma 280 I think it would be about 31.299"

The Absolute Position display will differ from the Machine Position display by any active G54 Z value and any active tool offsets.

You'll use G54 Z to establish your Part Zero (usually the finished face of the part) G54 Z will be the distance from the spindle mounting face to the Part Zero. IIRC, you'll see a number like 9" for a 4.5" long part clamped in a 4.5" long chuck. But don't set G54 Z until you've touched your tools off the Q-Setter:

Put a turning tool in one of the OD holders (lets say station 1).

Index the turret to T01. Lower the Q-Setter (the display should change to the Geometry Offset page and the cursor should be in offset 1).

Handwheel the tip of the tool close (within 0.04 or so) to the Z+ pad on the Q-Setter.

Jog Z- until the Z-axis stops and the red lamp on the probe lights. You should now have something like -0.025 in Geometry Offset 01 "Z".

Now jog Z+ to clear the probe, and Handwheel up in X and left in Z to put the tip of the insert over the center of the X+ pad.

Jog X- until the X-axis stops and the red lamp on the probe lights. You should now see a value in the Geometry Offset 01 "X".

Move away from the probe, retract the probe, and repeat for the remaining tools.

Now that you've measured your tools you can use any one of them to set your G54 Z work coordinate. Make sure G54 is active. If it isn't, MDI in a G54; INSERT then CYCLE START.

MDI in an index to tool 1. T0101; INSERT then CYCLE START. If the turret is not at station 1, it willl index to that tool and activate Geometry Offset 01.

Handwheel up to the face of the part. Change the display to the WORK offsets page, and move the cursor to G54 Z. Lets say where you are touching the part is 0.03 from where you want the finished face to be.

Press Z 0.03 [MEASUR]. Your Z Absolute Position display should read 0.0300.

Congratulations, you're ready to run! If you leave the tools in the turret and run a longer or shorter part, all you have to do is re-set your G54 as above.

[hackmeister]

Thanks so much! I was hoping for a step by step explanation. I will try this out hopefully in a few days after I get through running an important job using the "system" they have been using.
!st. You would change parameter 1241 to give the turret an index position.
2. Single step the program to G30 U0 W0
3. Go to the position page,and in relative hit U origin,and then W origin.
4. Then go and touch off the tools on the part in X, and Z. This involves having to add the part dia. to the number displayed in X relative. (Just touching off the tool on the Q setter seems like the faster, easier way to go don't cha think?) Then you need to edit into the program these touch off numbers in X,and Z. (lots of chances for mistakes here)

Just thought of a couple more questions.
On the machines I ran that had a Q setter they also had a tool library. Do I need to set up something like that? if so how? I don't remember seeing anything about a tool library in the manual for it.
Thank you all very much.

[dcoupar]

I've never seen any reference to a tool library in the Doosan manuals, unless you have an MX with milling spindle and ATC.

I believe your machine has 32 sets of Geometry/Wear Offsets. When you program you can use any offset with any tool (T0101, T0121) but the machine is set from the factory to set the offset number associated with the T number (T0101) when using the Q-setter. You can change this with a parameter, but it's a good safety feature when you're starting out.

Here's a little macro program to set the G30 X and Z to the current machine position. This eliminates changing parameter #1241.

Jog the X and Z to an index position then MDI in G65 P9010; INSERT, then CYCLE START. Parameter 1241 X and Z will be modified to the metric equivalent of the current machine position.

%
O9010(G30 AUTO SET)
#101=#5021*25400.
#102=#5022*25400.
G10L50
N1241P1R#101
N1241P2R#102
G11
M30
%

[Jim G]

Sorry, didn't notice the turning center note.

In addition to setting up tools with the offsetter, I also use the G54's on the Haas Lathe to run mutliple parts before feeding the bar.

If your part is .500 long, you can set the face of the next part at .650 with another offset.

Ie, first part, G54 = X0, Z0
2ND PART, G55 = X0, Z-.650
3RD PART, G56 = X0, Z-1.300

This gives .500 for the part, .120 for the cutoff tool and .030 to face the next part.


Edit:
It let me upload the file this time.

[hackmeister]

Thanks again guys. Jim G that picture helps, and I understand what you mean about how to do multiple parts.
dcoupar, I don't know anything about macro programing... yet. Is the program you wrote needed at the beginning of each tool in the program, or just once at the beginning of the program.
I was thinking more about the tool library thing, and both of the machines I ran that had one were also conversational in how they were programmed( one was a Mazak, and the other was a Hitachi-Seiki that had FAPT) so my guess is that the library was the tool info the machine used to generate a program.