Buyer Beware

[sharkcutup]

DaveMartin88 ---- Yes I believe you are correct it would be the control software but unfortunately with all that NWA has going on I am afraid that it probably would be way off in the distant future before anything like that happens!!!

In my Setup I have control over both the water-cooled spindle (change speeds on the fly) and the control feed rate speed of the CNC Shark by cutting down the percentage on the control software. By having the water-cooled spindle separate from the controller it provides much more latitude. I have also put in a total system shut down cutoff should anything go terribly wrong (both the water-cooled spindle and the control box are separate entities in my setup)!

Have a GREAT DAY Everyone!!!

Be SAFE around those AWESOME machines!!!

[Rando]

It is actually feasible to stop a cut and then "restart", but it takes some careful attention:

1) Start the original cut
2) When you're ready to stop it, hit the Pause button when the bit is NOT cutting...that is, during some rapid move up at safe-height.
3) Write down the line number in the Gcode viewing window that it is paused at.
4) Click the EStop (on screen!) button.
5) Move the head off your material. If you have a heavy spindle like I do, and the z-axis carriage drifts down when powered off, "park" the head on a block of something that's firm, but crushable. I use florist-foam with a rubber sheet. Most don't have this problem, but ideally you do NOT want to have the system lose z-height when it's off.
6) Turn everything off until you're ready to start again.

When you're getting ready to start again,

7) Make a copy of the .tap file and open it in an editor
8) Locate the place near the top of the file where it moves at safe-height over the material. There will likely be a bunch of M codes, and then one or two G codes.
9) Delete from immediately after the line in 8, all the way down to the line from 3, or just before it. You want to keep the lines where it goes from safe-height down to the cut, but you do NOT want to delete the code where it moves AT that safe-height. This is important if there are areas of the part that might get hit (or clamps!).
10) Save the tap file
11) Open the control panel, jog to safe height
12) Optional, if you think it might have lost ANY z-height at all: re-do the Z-height setting
13) Load the chopped file into the control panel, and run it.

The system does NOT need to be exactly where it was before all this started. Because you stopped the original cut while it was at safe-height, it should move to that safe position over the material, and then start off like it has no idea the earlier steps are gone.

Good luck!

There is another way to do this, but it requires changing the post-process to output block numbers into the GCode. Then you can just add a GOTO line just before the first G00 code. The GOTO should get the block number that is at the line number from step 3, above.

[sharkcutup]

Thank You Rando for the Information (Stop/Restart)!

I will have to try this the next time I have a long cutting operation.

This will come in handy (provided it works out okay) when I want to stop a job, shut down and then continue the job next day.

I have already been reading/studying the g-code and post processor to get an understanding of its logic/processes so I should have no problem with editing the g-code for my needs!!!

Thanks AGAIN!!!

Be SAFE around those AWESOME machines!!!

[rungemach]

Sharkcutup,

I would be very careful about splitting a G-code file and turning the machine off between runs. It's not for the faint hearted., and relies on absolute positioning rather than incremental, so watch out for that.

If the machine fails to stay in sync with the zero positions, your workpiece may be ruined. If you stop the machine and leave it powered on, there is less chance it will fall out of zero.

An alternative is to break the job up into separate tool paths that you run sequentially, with each tool path being able to be run without interruption.
If you plan your zero point at a place that will allow you to rezero the job if needed, you can run any of the tool paths at any time.

As an example, in Mach 3, the "run from here" command actually runs through all of the first portion of a Gcode file to compute where the new "here" starting point is, relative to the original zero points. The head moves to the new staring point at a safe height, and it starts from there.

As with most things, planning ahead saves a lot of " Oh #@%^&# s " later.

Bob

[Rando]

Thanks, sharkcutup.

As you get familiar with the post-processor files, think about putting a comment line, like

( +++++++++++++++++++++++++++++++++++++++++++ )

and with = and -, to set off the "preamble" and the "closing" sections. That will make it a lot easier to see what you need to
keep, and what you can get rid of.

<BobCAD-specific-stuff>
I use BobCAD/CAM a lot more these days than I do the Vectric software, and it will let me output all the steps/operations into a single tap file. I have the post put those markers between the operations and sections, and then wrote a small program that breaks out the one DesignName.tap file into files named "s01-DesignName.tap" and the like. That way all I have to do is set the machining order in BobCAD, post all the operations to one output file, run my program, and all the steps are neatly in order in the toolpath output folder. (Vectric, unfortunately, won't let me output all toolpaths at once regardless of the bit in use). The splitter app even collects the preamble and closing sections and adds them to the individual operation files. It has made my life SO much easier. Some of my parts have 25+ different operations. Next step is to make it a "splatter-gather" application where I can tell it to add together specific steps that use the same bit, and that can be run consecutively. So, if steps 8-12 all use the same bit and are intended to run in sequence, I'll be able to have it combine those into a single .tap file, instead of having to load and run all 5 steps individually.
</BobCAD-specific-stuff>

For me, I've found that three things take the most operator time: changing the bit (and setting Z), changing the part (I tend to run 5+ copies at a time), and loading the new GCode file (more steps = bad). Anything I can do to automate or reduce the work in those areas makes things run a lot more smoothly and efficiently.

Cheers!

Thom