UCCNC post processor tool change doesn't stop spindle

[Anonymous]

I'm using UCCNC with the 2017 screen set and tool change macro on my home built router.  I have the post processor tool change option turned on and everything works as it should except that when the spindle moves to the tool change position and waits for me to change the tool, the spindle does not shut off. The code produced does not have an M5 to turn the spindle off so I currently have to edit the code and insert an M5 for every tool change.

Here is a sample of the code produced for a tool change.

(Parallel1 (2))
M9
T2 M6
S10000 M3
G64
G54
M8

Can anyone tell me how to edit the post processor to output and M5 prior to the M6 tool change? I appreciate the help.

[randyT9V9C · Accepted solution]

Which UCCNC post are you using? I tried both the generic and the stepcraft. Both inserted spindle stop ahead of the manual tool change. Make certain the post property useToolChanger=NO, otherwise it will not insert the stops as it is likely implied.

https://cam.autodesk.com/posts?p=uccnc

https://cam.autodesk.com/posts?p=stepcraft_uccnc

Here is what my code looked like:

M9
M5
(Move to tool change position)
G53 X0. Y0.
M0 (Pause program for tool change)
T15 M6 (right hand tap D=0.19 #10 Form Tap)
S500 M3
G61
G54
M8

[mwbarre1]

I'm currently using the Roland DG ISO Post processor.  I have the same issue with a failure to stop the spindle so it can change it's tooling for the next step.  i know i'm missing the M05 call out.  I can manually edit but I want the post processor to fix it so I don't have to.   i've tried just changing the post processor option "use tool change"  yes/no option.  "Yes" does not put any M code in.  "NO" puts and M0 call, which I don't think is correct.  It should be M5 or M05.  So i think something is wrong.

In the Roland DG ISO brackets, i've located a possible position where it might be located, but I'm still not familiar enough with G-code to make this correctly.  Rather than stumble in the dark.  i was hoping someone might have a suggestion.

what i found:

Line 967     onCommand(COMMAND_STOP_SPINDLE);

it's by itself and doesn't seem complete.  Everything else has "writeBlock(gAbsIncModal.format (91));  etc etc etc...

I was hoping I could add the "writeBlock" command for the M05 command but it's not working.

Any ideas?

[randyT9V9C]

@mwbarre1, in the Roland ISO post change the IF statement on line 465 to include the command to stop the spindle prior to the unconditional stop.

    if (!properties.useToolChanger) {
      onCommand(COMMAND_STOP_SPINDLE);
      onCommand(COMMAND_STOP);
    }

Additionally you can change line 50 to default as useToolChanger: false so you don't have to remember to flip the properties when posting.

[mwbarre1]

Well, i'm not sure if it worked.  As I started the program, it moved to the machine zero and just stopped.  I think it added a machine stop / spindle stop at the beginning lines.

G90 G94 G17
G21
G91
G28 Z0.
G90
(FACE2)
(T1 D=3. CR=0. - FLAT END MILL)
M5
M0
S7000 M3
G54
G0 X97.87 Y1.35
G43 Z9. H1

i'm going back through and checking everything.

[randyT9V9C]

It is going to do an unconditional stop prior to each tool. Simply press the start button to continue after the stop.

Basically it runs the code to the stop and waits for you to press start to continue.

[daniel_lyall]

http://cnc-programming-tips.blogspot.com/2014/11/m00-m01-optional-stop.html