[Mihelich]

I am currently running the EMC software and am running into an issue that I am hoping someone can steer me in the right direction.
I have homed out the machine at 0,0,0. (no issue here)
I then located the part home which can be seen in line N35.

My issue is when I run the code it heads from the machine home to the part home but then instead of staying at the part coordinates and moving to the next line of code it heads back up to the top of the Z axis.
It then tracks through the rest of the code way above the part.
Clearly it is not remembering the part home and instead is still using the machine home.
What in the heck am I doing wrong here?


N30 G00 X 0.000 Y 0.000 Z 0.000
N35 G54 X -2.757 Y -0.276 Z -9.507
N38 M3 S4000
N40 G00 X -7.037 Y -4.071 Z 0.250
N50 G01 Z -0.200 F5.0
N60 G01 X -0.463 F10.0
N70 Y -3.971
N80 X -7.037
N90 Y -3.871
N100 X -5.958
N110 X -5.960 Y -3.871
N120 X -5.969 Y -3.869
N130 X -5.994 Y -3.864
N140 X -6.019 Y -3.859
N150 X -6.024 Y -3.858
N160 X -6.044 Y -3.853
N165 M5
N170 G00 Z 0.250
N180 G00 X 0.000 Y 0.000
N190 M0
N200 M2

-Tom

[Geof]

Unless EMC is doing things very differently that is not how you enter the part home.

Those coordinates should be entered into a table somewhere then in your program you have the command G54 G00 X0. Y0. Z0. and the machines moves to thos coordinates because they are where the part zero is.

Actually having a Z value in the part zero is sometimes not good practice and it is better to leave that coordinate at zero and then bring your tool down under the tool length offset.

[mactec54]

Hi Mihelich

How much Z travel do you have I think you have set your Z axes/or tool #1 not correct you need to look at the tool offset page

Also with programing like this G0Z.250 then G0X---Y--- if you don't move the Z up before a X/Y move you will crash at some time & break your tool

[pminmo]

I suspect it's the stored values for your g54 coordinate system. Take a look at section 3 here: http://wiki.linuxcnc.org/cgi-bin/emc...rdinateSystems

[Mihelich]

Thanks for the replies guys.

I sort of found a round about way to solve my problem.
Seems the G92 code starts the machine in the right part position after I do a machine home check then slew it to this position before I execute the code program. I do have a tech call in as to why the settings tab in my program menu is blank and thus prevents me from zeroing out the axis properly on the part.

N10 G92 X 0.000 Y 0.000 Z 0.000
N15 G00 Z 0.250
N20 M3 S5000
N25 G00 X -7.037 Y -4.071
N30 G00 Z -0.250
N35 G01 Z -0.200 F5.0
N40 G01 X -0.463 F10.0
N45 Y -3.971
N50 X -7.037
N55 Y -3.871
N60 X -5.958
N65 X -5.960 Y -3.871
N70 X -5.969 Y -3.869
N75 X -5.994 Y -3.864

[HuFlungDung]

It sure sounds like you don't quite understand how work offsets work. Yes, G92 can do anything, including screw you over if you abort the program and start at the wrong place

Calling G54 does not zero out anything. It invokes an offset of a work datum G54 X0Y0Z0 from the machine home G53X0Y0Z0.

So you measure the distance from machine zero to part zero via jogging motions and edge finders. When you have that figured out, then you enter those values into a G54work offset register in your control. Then within the body of your program, you simply call G54 to invoke the offset.

I don't know what EMC has for axis display options, but the machine position display will be different than the current work offset displayed position (by the amount in the G54 register), so you need to check out which is which, so you don't get confused.

[pminmo]

Thanks for the replies guys.

I sort of found a round about way to solve my problem.
Seems the G92 code starts the machine in the right part position after I do a machine home check then slew it to this position before I execute the code program. I do have a tech call in as to why the settings tab in my program menu is blank and thus prevents me from zeroing out the axis properly on the part.

N10 G92 X 0.000 Y 0.000 Z 0.000
N15 G00 Z 0.250
N20 M3 S5000
N25 G00 X -7.037 Y -4.071
N30 G00 Z -0.250
N35 G01 Z -0.200 F5.0
N40 G01 X -0.463 F10.0
N45 Y -3.971
N50 X -7.037
N55 Y -3.871
N60 X -5.958
N65 X -5.960 Y -3.871
N70 X -5.969 Y -3.869
N75 X -5.994 Y -3.864

That makes sense, but you need to get an understanding of the coordinate systems and offsets or your going to be misarable. Your machine has absolute coordinates that you have defined in respect to HOME. Then there are relative coordinates which are typically used to redifine the coordinates based on the part to be cut location. If your using AXIS as the display in EMC, you can drop down one of the menu's and you can select which is displayed, relative or absolute. G92 in line 10 sets the relative coordinate offsets of X, Y and Z all to zero at the absolute position where the machine is located at that instant it is executed. G54, G55, etc are stored coordinate systems that can be recalled by executing those commands. So for example if you have a fixture that holds a part to be cut, rather than going through the motions of a resetup each time you can use one of the stored coordinate systems.