Start and endcode added to Mach3 postprocessor after recent update

[info]

Hi to all!

since a recent F360 update the postprocessor for Mach3 adds a start- and an endcode. This caused my machine to crash badly into my vacuum table on start and on end .. Now I have to edit this postprocessor so I do not have to manually edit every single .tap file. The startcode being added automatically:

G28

G91

Z0.

G90

Endcode added automatically:

M9

G28

G91

Z0.

G90

G28

G91

X0.

Not only that his caused my machine to crash two times, I now also have to invest time to figure out how to edit the post processor for it. Any help appreciated.

[info]

Plus my codes are now stopping after each program part... so when I post several programs together, it will stop after each.

[serge.quiblier]

Hi @info 

For the stop issue, by default the post is activating the "Optional Stop" option. So an M1 command will be outputted between each operation.

Just untick the checkbox to prevent this behaviour.

The second one is related to the to the Safe Retracts option. There is 3 choices G28, G53, and Clearance height.

G28 and G53 will use machine parameters that should have been defined by the machine builder. Frequently this should send the tool to the tool change height.

It is always defined on the industrial milling machines. Less frequently on the routers or diy machines.

The clearance height will simply retract to the plane defined in Fusion. As long as you don't use multi axis toolpaths it should be safe enougth.

If you want to kee p the settings, you can edit the post in order to change the following lines.

In the block:

  optionalStop: {

    title: "Optional stop",

    description: "Outputs optional stop code during when necessary in the code.",

    type: "boolean",

    value: true,                                Change this one to value: false,

    scope: "post"

  },

Then in :

  safePositionMethod: {

    title: "Safe Retracts",

    description: "Select your desired retract option. 'Clearance Height' retracts to the operation clearance height.",

    type: "enum",

    values: [

      {title: "G28", id: "G28"},

      {title: "G53", id: "G53"},

      {title: "Clearance Height", id: "clearanceHeight"}

    ],

    value: "G28",                                 change this to value: "clearanceHeight",

    scope: "post"

  },

Have a pleasant day.

Regards
______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[engineguy]

@info 

What @serge.quiblier has given you is a reasonable solution but really you should be setting your machine up with a "Home" position that is a safe position, for example, a position where you would like it to go to to change a tool, then the machine will go to that position (Safe) at the start and end of operations and programs even if a G28 or a G53 is used, can`t crash then !!

What happened was not the fault of Fusion, user error!!

Also if you have now edited your Post Processor then you need to keep it in either your Local/Personal Post Processor Library or your Cloud Library and unless you turn off the automatic updates in your Preferences then your Edited Post Processor could be overwritten at the next Fusion update of that Post Processor, if you have a PP that works fine for you then do you really need it to be updated automatically ??