[Deano7/11]

i have been using a mach 3 post that has been modded to suit a 3 axis mill with manual tool change, the notes in the post say it will return the z to the top of the travel to make changing tools a breeze.

the post was downloaded from a site that gets mentioned quite a bit on a google search and i assume many other mach3 users are using the same post and would also assume that any bugs would have well and truly been ironed out of it due to the large amount of users. this makes me think the issue may be a mach 3 or mastercam setting issue not a post problem as why would the author of the post say it does a certain move and then when put into practice is doen the opposite.

the issue i have is at tool chane and end of program it outputs a move that wants to send the cutter through the job or table or vice.

it outputs something like

g0 z25
g49 z0
x0 y0
a0

then goes into tool change or end of program.
all i have been doing to fix this is delete the z0. i am tipping this z0 is ment to be in mach co-ord so that it returns the spindle to the top to change tools.

what do you guys think?

[txcncman]

Problem seems to be in the post processor. Why they would advertise something that is not true could be because they did not test it in all conditions or they lied. G49 is tool length compensation cancel. This puts the zero point back to the spindle face. Then the spindle tries to go to the Z0. level. You can edit your post and remove the Z0. for every line that has G49. Now, this will not give you full retract for tool change. To retract Z to a tool change position, you will probably either need to use G28 G91 Z0. or G53 Z0. If you need to add this after the G49 lines, use the syntax of the rest of the lines in the post processor as example.

[Deano7/11]

i have attached a copy of the post i am using.

i had a play around tonight with a line of code as per your suggestion.

i found another post that output similiar to your below line of g91 g28 z0 so i replaced parts of my code to replicate it and it worked great.

so it went from what i typed in my first post to this (example from tested code)

N6690 X80. Y7.75 I0. J1.5
N6700 G0 Z10.
N6710 M5
N6720 G91 G28 Z0. M9
N6730 X0. Y0.
N6740 A0.
N6750 M01
N6760 G49 T6 M6
N6770 G0 G90 G54 X-3. Y14.29 A0. S4000 M3
N6780 G43 H6 Z10. M8

this code worked good but has 2 issues. first on line N6770 it outputs a xy move for what looks like no reason. i would understand if it output a move before the tool change to get the job out of the way of the tools to avoid any accidental damage when changing.

next it doesn't move to the x0 y0 on line n6730. i assume this is because i need g0 in front of the x0 y0?

my next question is how do i edit the post to give me what i need?

[txcncman]

G28 is a non-modal command. You will need to repeat it on block 6730. Otherwise it is just doing an incremental (G91) X0. Y0. move.

[Deano7/11]

figured it would be something like that.

any ideas on editing?

[txcncman]

The post you uploaded is doubtful to have been edited to output the code you uploaded. Here is the first instance of problem(s):

#pfbld, n$, sgabsinc, *sg28ref, "Z1.", e$
#pfbld, n$, *sg28ref, "X0.", "Y0.", e$
#pfbld, n$, sg92, *xh$, *yh$, *zh$, e$
pfbld, n$, "G49", "G0", "Z0.", e$
pfbld, n$, "X0.", "Y0.", e$

Probably needs edited to:

#pfbld, n$, sgabsinc, *sg28ref, "Z1.", e$
#pfbld, n$, *sg28ref, "X0.", "Y0.", e$
#pfbld, n$, sg92, *xh$, *yh$, *zh$, e$
#pfbld, n$, "G49", "G0", "Z0.", e$
#pfbld, n$, "X0.", "Y0.", e$
pfbld, n$, sgabsinc, *sg28ref, "Z0.", e$
pfbld, n$, *sg28ref, "X0.", "Y0.", e$


The next area of concern is:

#pfbld, n$, *sg28ref, "X0.", "Y0.", e$
#pfbld, n$, sg92, *xh$, *yh$, *zh$, e$
pfbld, n$, "G49", "G0", "Z0.", e$
pfbld, n$, "X0.", "Y0.", e$

Should probably read:

#pfbld, n$, *sg28ref, "X0.", "Y0.", e$
#pfbld, n$, sg92, *xh$, *yh$, *zh$, e$
#pfbld, n$, "G49", "G0", "Z0.", e$
#pfbld, n$, "X0.", "Y0.", e$
pfbld, n$, sgabsinc, *sg28ref, "Z0.", e$
pfbld, n$, *sg28ref, "X0.", "Y0.", e$


Do you see the pattern yet?

The next area is:

# pbld, n$, sgabsinc, sgcode, *sg28ref, "Z1.", scoolant, e$
# if nextop$ = 1003 | tlchg_home, pbld, n$, *sg28ref, "X0.", "Y0.", protretinc, e$
# pbld, n$, sgabsinc, "Z1.", scoolant, e$
pbld, n$, "G49", "G0", "Z0.", scoolant, e$
pbld, n$, "X0.", "Y0.", scoolant, e$

Should probably read:

# pbld, n$, sgabsinc, sgcode, *sg28ref, "Z1.", scoolant, e$
# if nextop$ = 1003 | tlchg_home, pbld, n$, *sg28ref, "X0.", "Y0.", protretinc, e$
# pbld, n$, sgabsinc, "Z1.", scoolant, e$
#pbld, n$, "G49", "G0", "Z0.", scoolant, e$
#pbld, n$, "X0.", "Y0.", scoolant, e$
pbld, n$, sgabsinc, *sg28ref, "Z0.", e$
pbld, n$, *sg28ref, "X0.", "Y0.", e$

Notice, I did not delete anything. I commented out the lines to be edited and then added new lines under those.

[Deano7/11]

The post i attached doesn't output the N6720 G91 G28 Z0. M9
this was what another mach3 post output but that post has issues in another area as it wont do arcs for some reason. mach3 posts an error.

the post that i have been using and want to keep using so far works everywhere else but on the end of program and on tool changes due the to issues you have pointed out.

anyway i had noticed the g49 g0 z0 areas that you make mention of but i don't know how to edit and resave as a .pst file.

yes i see the pattern you mention. basically i assume that mastercam will ignore a line with # at the start?

so anything with the G49 G0 Z0 and x0 y0 needs to be commented out and more or less changed to the g28 z0 and g28 x0 y0

did i need the g91 in there aswell?

is there something within mastercam that lets me make these changes???