CNC Shark Forum

Does the shark post processor accept tape splitting commands? They do not seem to be listed.

If not, can anyone point me to instructions on manually breaking up large tap files that use a single tool into smaller chunks?

Thanks hugely!

(Sorry for the delays....the system refused to let me post the text. Something wrong in one of the lines of typing...still have no clue what it was that upset it so)

I have to assume you mean the VECTRIC post-processors for the Shark, correct?

The capability you're after would actually have to be part of the Vectric tools. Say, "Maximum toolpath size = X Kb" or similar.
Sadly, there is no such capability in the Vectric Software that I'm aware of.

If you want to manually split the files, that can be done, with a little preparation.

You'll first need to choose the base post-processor you want to use. Once you have one that works correctly,
make a copy of it, and call it something like "Splittable-Shark...." or something you'll recognize.

Now, use a text editor like notepad, (I prefer notepad++, a free download) and edit your custom post-processor.
Find the sections that start with "begin HEADER", "begin NEW_SEGMENT" and "begin FOOTER".
In the first two (HEADER and NEW-SEGMENT) add a comment line like below as the LAST line in those sections.
Use something like this, and be sure to include the quote marks:
"( ++++++++++++++++++++++++++++++++++++++++++++++++++ )"

In the last one (FOOTER), add a comment line like below as the FIRST line in those sections.
"( -------------------------------------------------- )"

Save the post processor file and maybe restart Vectric, though usually it's not needed.

Now, design your toolpaths as normal, but when you save those ginormous 3D carves that you want to cut up, use your
customer post-processor.

Next edit the tap file it produces. Because it's a big file, that's why I recommend you download and install
notepad++ (https://notepad-plus-plus.org/), because it can easily handle really big files.

Now, locate the section at the top of the file that ENDS with the ( +++++ ) line and copy that. That part is called
the preamble, or opening.

Go down through the file, adding those copied lines in to make new chunks. You'll later save those as your new files.
Add a few blank lines into the file ABOVE where you put the preambles. When I'm doing this, I often try and find where
it's moving to a new Z-level, but pretty much anywhere will do.

Then, go all the way to the bottom of the file, and copy from the (----) line to the end of the file. That's called the closing.

Now scan UPWARD in the file, and everywhere you placed the preambles, paste that closing section BEFORE the preambles you
pasted in a moment ago. Of course, don't past the closing at the very top of the file

Now the work is to just save those chunks into separate files. There are a few different ways to do that based on which
text editor you use:

If you're using notepad++, you can type Ctrl-N and open a new window, then copy each chunk into a separate window, and
then save each chunk as a uniquely named file. For example, step01-MyAmazingDesign.tap, step02-..., and so on.

If you're using plain old Windows notepad, open a second instance of the editor, and then copy each chunk into there, and
do a File...Save As to save it as those unique file names. Clear out the contents of the second notepad each time you get
ready to copy in another chunk (Ctrl-A, then Delete).

That will do it, and you'll have a bunch of "step" files.

Now, when you want to run them, there's one important thing to do: after you get your X0Y0Z0, jog the router/spindle
well up above the carving and in the general center of it. Do NOT start at Z0, as it's entirely possible it will go directly
down into the carving and completely f*ck up what's been done in the earlier steps. Start above and in the middle, so it
can gracefully angle down into the carving to do the next chunk. Please note, I am NOT saying your X0Y0Z0 needs to be
up the air....that needs to be where it normally is!

Got it? Once you've done it a couple times it will be pretty easy.

For extra credit, you can save the preamble and closing chunks as separate files, and you can just add them in.

Hope that helps. For me, I wrote some software that does a similar thing, for a different CAD/CAM system, but that's
to separate out toolpaths that are using different bits and setups, so sorry, it won't work for you .

Cheers!

Rando

Rando - Thanks for the well written and thorough reply.

In the interim before your response, I did some experimenting by modifying the Next Wave
post-processor. I simply added a single tape splitting command (one line) to the PP near the top of
the file right after POST_NAME, FILE_EXTENSION, and UNITS.

Next, in vcarve I then used my modified PP to save a toolpath. It splits what would be a
long tap file into a series of tap files (as many as you want depending on parameters given
to the tape splitting command). The minimum number of lines before splitting must be at least
600.

As I'm sure you know, vcarve makes it very simple to switch back and forth between the
modified and un-modified PP.

However, although the created series of tap files look OK, due to shop issues I have
not as yet been able to test them out on a machine. Do you think there will be a problem with this approach?

Here's what I never understand:

Why do guys like you, who figure out how to do things like this, NEVER actually include WHAT you did? Nor even where
you found the solution. You know, like a link to the updated Vectric post processor editing guide? Or the line you added?
Or copy the section of the guide telling you what to do? You know, so people in the future don't read the thread and sit
there and wonder WTF you're talking about? Do you think somehow it makes you "better" and "smarter" to hide the
answer from everyone else?

Pure laziness; not impressed.

How about you edit your post and add the information.

Can't answer all the questions in your rant, but there's a document entitled Guide to Editing a Vectric Post Processor that came with my VCarve installation. It's right there in the help menu: Help > Post Processor Editing Guide

I've had good success following its instructions to make custom modifications.

Fine, you lame-ass lazy people. Like I said: an answer isn't much of an answer if all you do is point in the
general direction. What you call a "rant", I call a valid complaint.

You can find the post-processor editing guide either in the Help menu, or also online at:

https://docs.vectric.com/docs/V10.0/Asp ... or-editing

The relevant section is about 1/6th of the way down, and has the following information:

---------------------------------------------------------
Tape Splitting Support

A section that describes how a long toolpath output will be split:

TAPE_SPLITTING=MAX_NUM_LINES LINE_TOL "FILENAME_FORMAT" START_INDEX INDEX_ON_FIRST_FILE

For example a command of:

TAPLE_SPLITTING=1000 100 "%s_%s.tap" 1 "YES"

would lead to...

Output will be split into multiple files of a maximum of 1000 lines (+ however many lines in there are within the footer section of the post processor), if a retract move exists after line 900 (1000 – 100), the file will be split at that move. If the file was called "toolpath" the split files would be named toolpath_1.tap, toolpath_2.tap etc. The first toolpath output will be "toolpath_ 1.tap" there will be no file named "toolpath" without an index number, (as INDEX_ON_FIRST_FILE= YES is used), unless the file was less than 1000 lines long, in which case the file would not be split.

Note

Some controllers that require NC files to be split, also have limitations on the number of characters within a filename. For example they may require the file to be named with the MSDOS style 8.3 filename format. This should be considered when naming the output file.

---------------------------------------------------------

Rando wrote: ↑

Fri May 13, 2022 5:45 pm

Fine, you lame-ass lazy people.

Rando, it's time to step back and take a deep breath.

I agree with your complaint about not sharing the solution the OP found. The more we share, the more we help each other. To that end, I went and looked up how to find the latest version of the document you linked to. (I found the one you linked, also, but the latest PDF is actually found using the instructions I provided.) I'm not sure that that gets me lumped in with lame, lazy people... just trying to add to the solution. You'll note (or you should note) that I'm not the OP, just someone like you trying to help out.

Just as it takes away from the forum to withhold solutions, it also denigrates the community when we resort to name calling. We're better than that. We don't need to sink to that level.

Rando wrote: ↑

Wed May 04, 2022 2:00 pm

Here's what I never understand:

Why do guys like you, who figure out how to do things like this, NEVER actually include WHAT you did? Nor even where
you found the solution.

You're a prime culprit is this regard Rando. You post these long written solutions that actually don't most of the time give enough specifics the OP can use and typically finish them off with "However, I wrote some software...", or modded my CNC or did this or did that, but never posting proof - not even an image when asked. And, when challenged you go off like you did here. Or, you hijack the thread with your bullsh?t pushing your fan dangled crap.