Z axis will not drop

[Scott Marshburn]

Ok I understand that and that’s why I need to input the parts corner to the machines closest point to home but why do not the rest of you guys get the same error. And no we do not have auto pins.so that may solve that problem.

[Gerry A Brown]

Hi,

M61L8 brings the pins up then M62L8 drops them. I guess the good part of working through my problem is I understand the G code a little better.

Scott,
I read in a thread that the graphing almost always errors out even on files the router will run so I just ran the file with my hand on the feed rate control & it went right through. I altered the PP to input M05 at the end to stop the spindle & also added STRTTIME.SUB & ENDTIME.SUB so will get a run time on the program. Now I am waiting for a new cutter as I broke one on the second run.

I am using G52L2 because of the jig I am using to hold the part & the ADJFIXOFF so the spindle starts on the end of the part closest to home.


Gerry

[Dennis Englert]

Scott,

G00 is the command for a rapid movement in a straight line. Without an X, Y or Z coordinate, this command does nothing except it does remain modal or in memory. That means that if the next line says X10, it will move as fast as it can. The G00 stays in effect until it sees a different movement command, such as G01, G02, G03, G12 or G13. (line with feedrate, CW Arc, CCW Arc, CW Ellipse or CCW Ellipse as listed).

The G52L# and the G51 codes are fixture offsets that set up X0 and Y0 or the origin. The G52L# uses the fixture offset table to store the location values, while the location values are stated with the G51, i.e., G51 X10 Y10. The G52L# is the more commonly used fixture offset on machines with popup pins. The appropriate G52L# is setup for the position in Control Nesting. Normallly, G52L1 is the corner of the sheet goods as positioned in the pins, while G52L2 is used with the locating bracket. The G51 is often used when you randomly place something on the table to be cut. For example, you may want to carve something that you designed in ArtCam and you made the mid-point of that design the origin. At the mahcine, you can find the mid-point of your material with the handheld and then use the absolute coordinates for your G51.

Since you replaced the G51 or G52L# with a G00, machine home became X0 and Y0 or the origin. So in this case, machine home and the origin are synonymous. I believe a previous posting indicated that you don't have the popup pins. The M60 series codes cause the pins to pop up and down and also check their status. You would have to either delete them or comment them out for a program to run on your machine.

Dennis

[Scott Marshburn]

Scott,

G00 is the command for a rapid movement in a straight line. Without an X, Y or Z coordinate, this command does nothing except it does remain modal or in memory. That means that if the next line says X10, it will move as fast as it can. The G00 stays in effect until it sees a different movement command, such as G01, G02, G03, G12 or G13. (line with feedrate, CW Arc, CCW Arc, CW Ellipse or CCW Ellipse as listed).

The G52L# and the G51 codes are fixture offsets that set up X0 and Y0 or the origin. The G52L# uses the fixture offset table to store the location values, while the location values are stated with the G51, i.e., G51 X10 Y10. The G52L# is the more commonly used fixture offset on machines with popup pins. The appropriate G52L# is setup for the position in Control Nesting. Normallly, G52L1 is the corner of the sheet goods as positioned in the pins, while G52L2 is used with the locating bracket. The G51 is often used when you randomly place something on the table to be cut. For example, you may want to carve something that you designed in ArtCam and you made the mid-point of that design the origin. At the mahcine, you can find the mid-point of your material with the handheld and then use the absolute coordinates for your G51.

Since you replaced the G51 or G52L# with a G00, machine home became X0 and Y0 or the origin. So in this case, machine home and the origin are synonymous. I believe a previous posting indicated that you don't have the popup pins. The M60 series codes cause the pins to pop up and down and also check their status. You would have to either delete them or comment them out for a program to run on your machine.

Dennis

Ok Dennis I think I think I understand almost every thing you posted except for one thing I am not replacing the G51 or G52L# with a G00 but replacing the G00 with G51 and that’s the only way the machine will come close to excuting the rest of the code

[Dennis Englert]

For example, if you replace G00 X42 Y36 with G51 X42 Y36, then X42 Y36 from machine home in absolute becomes X0 Y0. If that works, I think it is just happenstance. If you replace G00 X42 Y36 with G51 alone, it does nothing at all, the machine does not move nor does it change the fixture offset.

A program, particularly a program that's been generated by Control Nesting contains a lot of code including Advanced Function Language (AFL) programming. For the most part, what each line of a program does is fairly easy to look up and decipher. AFL can be a little harder to understand, since it contains many program variables that you can not look up. Some of the variables are generally understandable as they imply their purpose.

However, I would warn against just substituting one code for another without a full understanding of what that code really does. Fortunately, for 3 axis many of the changes affect only 2/3's of the axis, i.e., X and Y. You must be more cautious with the Z axis, which was the problem noted at the start of this thread. If you have any of the axes that show out-of-bounds, it's typically because the fixture offset is not setup. For X and Y, that would be the G51, G52L# or G900 series codes. For the Z axis, that would have to be a combination of the daylight value in the tool's setup, the SWITCHSPOIL and the Wasterboard variables. On Version 8 or QCore, we also have to consider ORGSPOIL and ACTSPOIL for the Z axis.

So if you are replacing one code with another, you may have the luck of the Irish. Or you may not! LOL

Dennis