topic Betreff: Macro to change tool numbers in NC Program in PowerMill Forum

Macro to change tool numbers in NC Program

E-Singer89 — Tue, 27 Feb 2024 18:42:57 GMT

Hey all, so I was wondering if there is a way to write a macro to change tool numbers in an NC Program. The reason I ask is because; all of our 3-axis machines allow up to like 500 tools in the offset page whereas our 5-axis machines only allow up to like 200 (Haas). So, when programming and a job starts in 3-axis and ends in 5-axis, when I go to post out a 5-axis program I have to go into the NC program and manually change all the tool numbers, so we don't get an alarm on the machine. I would rather not have multiple tool libraries or multiple entries in the tool library to accommodate for this. Is there a way to write a macro that would change these tool numbers in the NC Program for me when I'm ready to post? I'm aware i would have to build the list in its entirety into the macro but that's fine. I'm just very unsure of how to phrase all the if-then statements (If that's what I would even use)

Re: Macro to change tool numbers in NC Program

nguyenthinhvt95 — Wed, 28 Feb 2024 03:25:52 GMT

Could you share some picture in detail?

Maybe somebody can help you.

Betreff: Macro to change tool numbers in NC Program

icse — Wed, 28 Feb 2024 07:03:11 GMT

This macro takes every tool in the project with a number larger than 200 and replaces its number with the first free lowest tool number:

int $newToolNumb = 0 foreach $t in filter(folder('tool'),'this.Number.Value > 200') { $newToolNumb = $newToolNumb + 1 int list $toolnumbers = extract(folder('tool'), 'Tool.Number.Value') while member($toolnumbers, $newToolNumb) { $newToolNumb = $newToolNumb + 1 } EDIT TOOL ${t.Name} NUMBER COMMANDFROMUI ${newToolNumb} }

Betreff: Macro to change tool numbers in NC Program

E-Singer89 — Wed, 28 Feb 2024 12:22:35 GMT

Interesting, thank you. But not quite what I need. We have a set tool list of what tool is assigned to what offset number

Re: Macro to change tool numbers in NC Program

E-Singer89 — Wed, 28 Feb 2024 12:40:36 GMT

sorry about that.

here is an example of a 3-axis program

5-axis program before settings change

this is where i change my tool numbers in the nc program

and this is what it looks like after the change, the asterisk notes that a change was made.

Betreff: Macro to change tool numbers in NC Program

icse — Wed, 28 Feb 2024 13:02:11 GMT

you coud make a .txt file for mapping

500|200

400|1

....

so number 500 is changed to 200, 400 is changed to 1 and so on

sry i misunderstood you i rewrite the macro

Betreff: Macro to change tool numbers in NC Program

E-Singer89 — Wed, 28 Feb 2024 12:44:09 GMT

this is what i had in mind for sure. Is this going to change the tool numbers in the project though or just in the nc program? see my pictures above

Betreff: Macro to change tool numbers in NC Program

icse — Wed, 28 Feb 2024 13:24:15 GMT

Try this:

string $mappingPath = "C:\YourPath\mapping.txt" if not file_exists($mappingPath) { message info "Can't find mapping file" return } string list $mapping = {} FILE OPEN $mappingPath FOR READ AS Input FILE READ $mapping FROM Input FILE CLOSE Input entity list $ncPrograms = input entity multiple ncprogram "Select NcPrograms to change tool numbers" foreach $ncprogram in $ncPrograms { foreach $line in $mapping { int $target = tokens($line,'|')[0] int $dest = tokens($line,'|')[1] foreach $tp in filter(components($ncprogram),'this.ToolNumber.FromTool == "' + $target + '"') { $tp.ToolNumber.UserDefined = 1 $tp.ToolNumber.Typed = $dest $tp.ToolNumber.Value = $dest } } }

but please make a backup of your project first i did not tested it jet...

Betreff: Macro to change tool numbers in NC Program

E-Singer89 — Wed, 28 Feb 2024 13:29:49 GMT

I will test this on a dummy file. Thank you! ill let you know how it goes

Betreff: Macro to change tool numbers in NC Program

E-Singer89 — Wed, 28 Feb 2024 13:37:48 GMT

it works!!!! thank you!!!!