Box Top Clearance Z Move

[warrguitars]

Is there a way to set the Z movement to move faster when it comes to the "Box top clearance"?

I have tried a bunch of things and have not figured out the magic code- Lol

G00 G49 G40.1 G17 G80 G50 G90 G64
G20
M998
(Brass_FlatEnd_.25)
M6 T1
M03 S10000
G01Z0.5000 < this move here I would like to move faster

Thanks

[Dan B]

You're telling the machine to do a linear move to Z0.5, but you aren't telling it the feed rate to use. Adding an F(something) at the end of the line should give you control over how fast it gets there.

Something like this:

G00 G49 G40.1 G17 G80 G50 G90 G64
G20
M998
(Brass_FlatEnd_.25)
M6 T1
M03 S10000
G01Z0.5000F100

I'm assuming you are working in inches so that F100 would move the machine to that specified Z location at 100 inches/minute. For subsequent linear moves, that feedrate will "stick" until you define another. Like this:

G00 G49 G40.1 G17 G80 G50 G90 G64
G20
M998
(Brass_FlatEnd_.25)
M6 T1
M03 S10000
G01Z0.5000F100
X2.0000Y2.0000 (the G01 and feed are carried over from the previous line)
G01Z0.0000F50 (using an new F value will cause this line to move at the new feed rate.)

Depending on your controller, the above example may or may not work. Some controllers may need the command (G01) and the feed (F) defined on each line. You probably already know what works for your machine.

I'm a little surprised that your machine moved at all without a feedrate defined. I've seen this happen here, but we get a warning on the controller that a feed is missing (Heidenhain controllers). But again, there are a lot of variations when it comes to controllers.

Hope this helps,

Dan

[warrguitars]

Thanks Dan,

I am using Mach 3 inch. Do you know if I can define it in the post processor and if so where? At this time I figured out how to insert M998 and M997 for my purpose of tool change position and moving the spindle out of the way.

I have tried a bunch of things and can not seem to make it work. I have been using RhinoCam and the way it is working is as follows; I start the code and M998 takes the spindle to home in rapid fashion, then the spindle goes to the work piece x y in rapid fashion, then z in rapid fashion, then the programmed x y z feeds that I programmed take over.

Here is what I am using at the moment with regard to the post processor;

//MadCAM_POST_2003-12-10
*VERSION*
1.0_031210
*FILE_NAME*
Mach3_Gcode
*FILE_EXTENSION*
txt
*FILE_DEST*
c:\postfiles\
*FILTER*
0.001
*OUTPUT_WIDTH*
4
*OUTPUT_DECIMALS*
4
*SCALE_X*
1
*SCALE_Y*
1
*SCALE_Z*
1
*AXIS_1_CHAR*
X
*AXIS_2_CHAR*
Y
*AXIS_3_CHAR*
Z
*CUTTER_REFERENCE*
TIP
*RAPID*
G00"x""y""z"
*END_SECTION*
*RAPID_APPROACH*
"x""y""z"
*END_SECTION*
*RAPID_RETRACT*
G00"x""y""z"
*END_SECTION*
*APPROACH*
G01"x""y""z" F"feedz"
*END_SECTION*
*FIRST_CUT*
"x""y""z" F"feed"
*END_SECTION*
*CUT*
"x""y""z"
*END_SECTION*
*TOOL_CHANGE*
("toolname")
M6 T"toolnr"
M03 S"speed"
G01"zhome"
*END_SECTION*
*TOOL_STOP*
M997
M5 M9
*END_SECTION*
*PROGRAM_START*
G00 G49 G40.1 G17 G80 G50 G90 G64
G20
M998
*END_SECTION*
*PROGRAM_END*
M30
*END_SECTION*
*LINE_START_NUMBER*
1

Thanks much,

Mark

[Dan B]

Hi Mark,

Add this section to your post (don't know if it matters, but I have this right above the first rapid section):

*FIRST_MOVE*
(define your moves here)
*END_SECTION*

Here is a sample from my Haas post:

*FIRST_MOVE*
N"lnbr" S"speed"M3
N"lnbr" G01"x""y"F10000
N"lnbr" "z"
N"lnbr" "coolant_on"
*END_SECTION*

This should help.

Dan

[warrguitars]

Thanks Dan,

I tried some of that and it does not seem to make a difference. I did remove the "zhome" line all together and its seems to work. Doing this, will it cause any kind of safe clearance issues???

Getting close and thanks. Just trying to tweak.

Mark

[Dan B]

The "zhome" variable is how you get the values on the post page to show up in the code. (see the attachment)

I would suggest you don't put a linear move in the "Tool Change" section. Let the "First Move" section handle that.

Let me know how that works. I'll attach my Haas post for reference. Sorry, I don't have one specifically for your machine, but maybe this will help.

Dan

[warrguitars]

Hi Dan,

I figured it out. I just inserted a F80 next to the G01"zhome" like this;

G01"zhome" F80 and it all works the way I want it now without compromising or losing the "Box Top Clearance" setting. I hope this helps any other Mach 3 user.

Thank you for the time trying, it is greatly appreciated!

Mark