Explore the machine coordinate system.
- [Instructor] In this movie, we're going to be talking about the machine coordinate selection command, and that command is the G53 command. Now the G53 command allows you to select the machine coordinate system on the line that it's called on. What that means is it's a non-modal command. So you have to use the G53 on every single line you'd like it to be active on. It's very different from most other work-offsets, like a G54, 55, ones you call a G54 command, it stays active until you select something else. With the G53, it only works on the line you're calling it on.
Now generally, the G53 command is used very similar to a G28 command to return the machine back to the machine home position. Now we can do that very easily with either the G28 or the G53, but the G53 is preferred because it's a little bit safer and it's a little bit easier to understand. One bit of caution though is the G53 a lot of times does not work on older machines or some specific machines that don't have that G53 active. We're going to be working on a fairly new Hause machine, and the G53 definitely does work on this machine and it's the preferred method.
But if you happen to get an older machine or a machine that just doesn't work with G53, you can always go back and use a G28 command in its place. I also want to point out one of the benefits of the G53 is it can be used for positioning the table. A very common thing might be to bring the table forward and centered. When you're done with your operations, you can easily get at your workpiece and get it off the table without having to bend over and hurt your back. So you can use it not only to send the machine back to the home position, but also can be used for positioning using that work coordinate system. Let's go ahead and take a look at some of the G code we're going to be running on the machine so you can see what's going to be happening.
All right, so here is the very simple program I'm going to be running. And notice we're calling out G53 on three individual lines. So the very first line you can see right up here, which is G53 G0 Z0. So what that's going to do is it's going to move the machine up to the Z0 position. Next it's going to move the machine to, machine coordinate system, X and Y. So that should take it all the way back to machine zero. Now notice I'm calling this M zero command, and what that's going to do is it's going to add a pause to my program, so I'm going to have to push the green button again to keep the program going.
Now we're going to be covering the M0 command a little bit later in the course, so all you need to know at this point is that it creates a stop in the program so I'm forced to hit the green button again to continue to program. Then, the next line here you can see I have a G53 X -15 Y0. So that should center the table. Now I'm not sure exactly what machine you're going to be working on, whether it's a 40 by 20 machine or maybe a 30 by 16 machine. So we might need to adjust this a little bit when we get to the machine. But generally, 15 inches is about the middle of the table on a 30 inch wide machine.
We might need to change that to 20 if it happens to be a 40 20 machine when we actually start using this command. And so whenever you're actually using this in your own shop, you want to basically figure out how wide your table is, split the difference, and put the X-value right there, if you happen to have a home position in the upper right hand corner of your table. Some machines have the machine home position right in the center of the table, some have it in the upper left hand corner. There's a whole bunch of different places that machine builders will put that machine home position. But wherever it happens to be, if you use the G53, just figure out how far you need to move the table from the machine coordinates system to get it centered and then moved all the way forward so you can easily get at your work piece.
Now let's head over to the C&C Machine and see how these programs run. - In this example, I'm going to go ahead and show you how to use the G53 command. On newer machines, a G53 command is generally preferred over a G28 to return the machine to machine home position. However, with the G53 command, we can also do general positioning moves. One common use is to move table to center and forward at the end of the program. Let's go ahead and run the sample program and sees how it looks.
First you should see the machine move to machine home position, and then it'll bring the table center and forward. (machine beeping) It's going to pause for a second, and then let's go ahead and hit the green button to bring the table to center position. The G53 command is very simple to use and is simpler to understand than the G28 Because it is a non-modal command, you need to call the G53 on every line that you would like it to be active.
For instance, if your machine was using the G54 workoff set, I could call a G53 command on one line, and on the very next line, the G54 would be active again. So it does not stay active like most other work offsets. We use the G53 command to send the machine back to machine home, and we'll do positioning moves like moving the table forward at the end of the program.
- CNC concepts
- G-code editor and simulator software
- G-codes: G00-G84
- M-codes: M00-M09
- Writing a sample program in G-Code