Z axis Help!

[Tom Curran]

Vertical mill, CamSoft control.

My Z axis home position is currently set with the bottom of the stroke as ZERO and the all the way up as 5.5".

When I hand write programs this works OK, but I run into real problems when I use a code like G0Z0G28 (return to home in Z). The spindle dives into the table.

Should the machine home positions be set as top of spindle stroke as ZERO, and the bottom of stroke as -5.5?

Thanks, Tom

[Karl_T]

I have my machine zero on Z set about 0.050 from top of travel. Makes Zero return go here. Very handy as you need to go to this point often on a mill. If you prefer you could rewrite your zero return to go to machine coordinate Z 5.5 Either way will work. if you want to do the latter way, post your G28 from Gcode.fil and I'll suggest how to edit.

Karl

[Tom Curran]

Karl, thanks for your reply.

Before I make any changes to the Z software limits, I want to know if having Z up as 0 and Z down at MINUS (-) 5.5" will cause any problems with the CamSoft control?

I like your suggestion of G28 at .05 short of the limit.

Thanks, Tom

[Al_The_Man]

It is common to make all the way up on the Z for a mill as zero, you can always change the Z (and X/Y) zero points with the G54 etc, work coordinate system.
With mills, I normally have an automatic referencing, with the Z performed first, once homed, the X/Y home.
Al.

[Tom Curran]

Karl, here is a .fil for G9:
-----G9
!'Like G01 but Decel to stop
!DISPLAY4 {f*(\73/100)}
!DISPLAY5 {s*(\74/100)}
!RUNTIME \4
!DISPLAY8 \4

Here is what I have for G28:
-----G28

That's it. nothing else, no instruction, no commands.

I'm open for suggestions. I never wrote this kind of language before, so if you make a suggestion, I will try it carefully.

Thanks, Tom

[Tom Curran]

Karl, back to your question on the .fil for G28. I think I would like to proceed by changing the UP to Zero, and DOWN to negative 5.5"

I looked up the G28.fil:

This is what is programmed for that command:
-----G28

Other codes have lots of commands, like G9:
-----G9
!'Like G01 but Decel to stop
!DISPLAY4 {f*(\73/100)}
!DISPLAY5 {s*(\74/100)}
!RUNTIME \4
!DISPLAY8 \4
-----G10
-----G11
-----G12 etc.

I am open for suggestions at this point. I will try things out very cautiously. I appreciate your help,
Tom

[Karl_T]

One little detail, I've got used to, but is confusing. The code for the Gcode is ahead of the
----G9. You showed me the code for G10. Look again for your G28. If nothing is there, tell me your words exactly what you need this Gcode to do.

I never let the operator see the machine coordinates. There's no real need. I have the control remember part 0 when ever the operator sets up. And then reload these on machine startup. I only re-home after a crash or cpu malfunction, I've found Camsoft to never lose its spot. In my case, X0 is often the left side of the vice back jaw, Y0 is the face of the vice back jaw. The there's no need to re-indicate in a part in the vice, even after shutdown. Then I use G55 to G59 for any offsets. Just a time saving trick.

To answer your question on a possible problem, if your programmer does everything right it will work perfectly. I would tell you I've personally nver made a mistake and crashed a machine but I might be fibbing

Karl

[Tom Curran]

Karl, this is what I have:

-----G25
-----G26
-----G27
-----G28

When this command is called, I would like the Z axis to go all the way up to home, or just short of home, whichever is safer.

Thanks, Tom

[Karl_T]

Originally Posted by Tom Curran Karl, back to your question on the .fil for G28. I think I would like to proceed by changing the UP to Zero, and DOWN to negative 5.5"

Find your home macro. There will be a command MACHZERO in it. The third paramter is the Z value. You have to know the exact distance between your home position and your upper limit switch. I enter this as a negative value minus the 50 thou to not hit the limit.

Karl

[Karl_T]

Originally Posted by Tom Curran Karl, this is what I have: -----G25 -----G26 -----G27 -----G28 When this command is called, I would like the Z axis to go all the way up to home, or just short of home, whichever is safer. Thanks, Tom

The command is MACHGO
you can just use this or you can cover for other contingencies. Do you want to go there if the machine is not homed? CRASH!!! Do you want to go there at a certain feed rate, might take forever if you're set real slow. i also use this for tool changer, so I wrote the following macro:


'**************************Retract for tool change********************
[[RETRACT]]
LOADING \55:IF \55=0 THEN EXIT
'IF \123<>1 THEN QUESTION Machine not homed Run anyway;\55;N:IF\55<>Y THEN EXIT
\124=f 'current feed rate
f=50

IF \142=1 THEN [GALILERRORS] 'message Galil errors
MACHGO ;;0
f={\124}
IF \142=1 THEN [GALILERRORS] 'message Galil errors



You don't have the LOADING command in Lite, I write for Pro. The \142 is an example of using a flag. In this case, if something is flakey i can set this flag and get all sorts of detailed diagnostic messages. makes machine repair a snap. I think machines should help you diagnose their problems.

Karl

[Tom Curran]

Karl, I have CNC Lite.

Thanks for the tips on the home macro MACHGO. I must get my software limits switched first before I use it, I believe. Make the UP home, and down -5.5.

Thanks, Tom

[Tom Curran]

Got my spindle soft limits reconfigured today. The code G28Z0 send s the spindle UP, like it's supposed to! Hurrah!

Thanks for your suggestions, everyone.

Tim