cnc shark doesnt support tool changes??

Anything and everything CNC-Shark-related

Moderators: ddw, sbk, al wolford

cnc shark doesnt support tool changes??

Postby jamespotter » Mon May 14, 2018 10:01 am


I have a cnc shark for about a month now, and it doesnt seem to support tool changing from rough tool path to finishing tool path.when i go to save it says it doesnt support the tool change. is it the shark or the software i have Vectric pro 3.1? is there a work around for this problem?

Please help.

I didn't find the right solution from the Internet.


Posts: 5
Joined: Sat May 12, 2018 6:55 am

Re: cnc shark doesnt support tool changes??

Postby Rando » Mon May 14, 2018 10:10 pm


It's not so much that they don't support tool changers, as they don't have an automated tool changer in the first place. ;)

What they don't have
To support in-process manual tool changes requires the system to be fully interactive while you get the new tool's z-height.
The Shark controllers don't support that, so in that sense you're correct. But, that isn't the entire story....

How that leads us to work
This is the part that most-closely answers your question, as it describes how we're forced to work BECAUSE there is no toolchanger.

The normal work method for the Sharks is to output the toolpaths into individual files arranged by which cutting tool they're using.
Of course, they have to be separated into the different work positioning/registration setups also. So, you mount the material,
then run a single GCODE (.tap file extension) toolpath file that can do everything that single tool needs to do. When it finishes,
you change the tool and get it's proper z-height, then load that next toolpath file to run with that bit. Essentially, YOU are the automated
toolchanger. Yeah, who's the robot NOW? Wait 'till you realize you're also a flesh-bag "bar puller" to these machines :twisted:

Wait...there IS a tool change GCode command?
There is, though, one sense in which the sharks DO support "tool changes". Well, let's instead say the controller performs a known
and sometimes-useful action when it encounters an M06 T01 line in the toolpath. What you ask? Well, it pauses the progress
of the controller through the GCode. It then allows you hit continue or cancel. So with no tool changer, and no automated spin-down
of the router/spindle, and no ability to jog to replace the bit, and no way to re-zero for the new bit, just what good is it, right?
Certainly not useful for what we usually think of for a command named "tool change" :(

But without the ATC hardware, it's useless, right?
Well, remember how I mentioned that in addition to being the tool changer, we're also the "bar puller"? Well, a bar puller (apologies
if you already know this) is an automated sub-robot that feeds a new chunk of material into a CNC machine, so it can continue
working, part after part. When you're making, say 20 parts of something you quickly realize that indeed, you're the bar-puller,
or pallet-loader if you will.

Here's what useful about that M06 T01 command: if you surround that with "move the heck out of the way" and "move back where
you were" commands, you can effectively manipulate the part in the vise while the machine is out of the way, paused. You re-load
the current part in a new orientation, or you load a new part, push the Continue button, and the machine continues with the next
step. That's right, we just saved you going over and jogging the machine, loading the part, jogging back, clicking Run, Okay,

The one significant restriction to remember when doing that, though, is that your part registration, work-stops, vises, hold-downs,
whatever you use, had better be EXACTLY positioned, and STAY there no matter what. There's something of a fine art to being able
to rotate a part and have it's new position be consistently proper both in alignment and location, down to 0.001", so that features
that have to match up around corners of the part actually do line up.

Yeah, but how does that actually help?
By combining multiple feature-based toolpaths that use the same bit, and adding in the M06 T01 (with surrounding movements),
you load the combined toolpath once, run the first part, and it moves out of the way for you to do whatever is necessary, even just
measure the part. Then you click continue each time until it's done, and then you move on. For me, with some parts having in the
35+ individual toolpaths, this is a HUGE help. Many projects often have one clearance/roughing and one finish toolpath, so for
those, that slicing and dicing toolpaths won't be that important...yet. Once you start working with fully 3D models, work holding and
registration through moving the part are a big thing, and working in multiple bits becomes more complicated.

For example, consider a sculpture piece that uses a square endmill for rouging, an 1/8" square for some fine material removal, and
then a succession of 1/8", 1/16" and 1/32" taper ball mills to do the finishing work. Five bit changes, at least two, and possibly four
sides. (Again...who's the robot now?) Wouldn't it be cool if you could do ALL of the work of the first bit, then ALL of the work of the
second bit,.... And all you have to do it insert the bit, load a part, run, rotate a part, run, rotate, run, rotate, run, and then set that
part aside. In goes part #2, and it gets all four, same file, same parts separated with continues. So, you still have to stand there
and tend the machine, but now there's nearly zero interaction with the computer part, and it's all about watching the cutting and
moving the part and loading it. If you were doing 5 of those parts and did each part and each bit in series, you'd be looking at 100
tool changes, 100 file loads, 100 z-height settings, and 100 part-loading actions. By using the combination, you take that down to 5 tool
changes and 5 z-height settings. You also drop file-loading from 100 to 5. And clicks to the control-panel software is similarly reduced.
Yeah, it's that powerful.

Sounds complicated! (sadly, it is)
Getting that capability calls for more than a bit of upfront planning. I developed a system using custom post-processor
files for Vectric and BobCAD, and two software tools I wrote: GCodeSG (splatter-gather) that takes multi-toolpath files, chops them up
into steps, and recombines them into "combi" files. It automatically inserts the Pauses that move the spindle out of the way and use that
M06 T01 command (staying on subject ;-) ). The second program, GCodeShim, does what the name implies: allows you to mathematically
alter a GCode file along any axis. Need to move an engraving 0.002" deeper? No problem, just add it to the build script. Then, whenever
a design change happens, I just output the files, run my build scripts, and all the toolpath steps and combi files are put right where I
can find them. No muss, no fuss, no bother. ;-). But, as you'd imagine, if you're not pretty up on working with GCode and post-processor
files already, making that transition with feel confusing for bit.

If the above makes you want to try crazy things
All that said, I'd be remiss if I didn't mention that you CAN BUILD an ATC for the Shark. Well, it SEEMS feasible. There are properly-sized
spindles that include the tool changer hardware. At that point, all it needs to be added are direct spindle-speed control (to stop and restart it),
enough tool-holders with measured z-height tool offsets, and a precision-machined tool holder that is precisely located in the bed of the
machine so the controller can always find it. Which usually means there are limit switches to establish a true machine-Zero location. That's
a whole heaping mess of custom GCode, but I'll bet such a system could be contrived. Not easily, but feasibly :D.

See? And you thought it was a simple question. :D :shock: :roll:

Hope that helps


===================================================== Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
Posts: 583
Joined: Tue Jan 06, 2015 3:24 pm
Location: Hoquiam, WA

Re: cnc shark doesnt support tool changes??

Postby jeb2cav » Tue May 15, 2018 8:40 am

Hi James,

Create 2 toolpath tap files. One for the rough and one for the finish.

Run the rough job, change bits, rezero z for the second bit, and run the finish job.
Site Admin
Posts: 1514
Joined: Thu Sep 30, 2010 7:04 pm
Location: Kentucky

Return to CNC Shark

Who is online

Users browsing this forum: Google [Bot] and 4 guests