safe z not so safe!

[edowney]

I've been a very happy owner of a slightly used cnc shark for the past year. Then today for no apparent reason it decided that 3/4" is just fine for the safe z value which is set to 1" according to the preferences. I have plenty of clearance and the work I do is 2 dimensional so I could go with probably 2" of safe z height but if I try to tell it to go above 1" it complains. But 1" worked for me so I didn't fight it. Now it thinks around 3/4" is fine but it's cutting it awfully close to hitting my clamping mechanism which obviously worries me. Any idea what's causing that? Thanks!

[Kayvon]

if I try to tell it to go above 1" it complains

Can you elaborate on this? What's doing the complaining, VCarve or Control Panel?

[Rando]

As you've found, there are several places where "safe height" might be set; let's see if one of these is the culprit:

1) The control panel, under preferences, there's a default safe height that the controller tries to move to. That one's pretty easy to find, as you did. Changing this value might (as in MIGHT) require a restart of the control panel software to take effect, but I could be easily wrong on that too.
2) In VCarve, under the material setup panel, there's an entry for safe height.
3) In the post-processor files, NWA's preamble and closing sections, IIRC, have G01 and G00 blocks that do Z moves to a "safe height". I'm pretty sure that is supposed to be for number 2) above, but some post processor files I've seen have hard-coded values. Check and adjust if needed. If the line uses something like [zh], that means the user-specified z-safe height, so that one should come through properly.

I typically think of safe height as being two numbers: one for when it's cutting inside a particular feature, and one for moving between features and on-and-off the material at beginning and end. The first one, the one for "local moves", if you will, I typically run at 0.020" - 0.040". If you're doing any v-carving, setting this as a small (enough) value will vastly improve the cut times, since it will get rid of most of the up and down motions. The second one I typically set to not much more, typically 0.10". Now, I will say that watching an expensive endmill come over a big block of solid aluminum with only 1/10th inch clearance makes me wince each and every time . The only time a problem has happened with that is when I had a bad cut that pulled the bit slightly out of the chuck, and I neglected to get the new Z0. Doh!

Like you found, getting those numbers right can be a strange and maddening experience. But, with a bit of concentration on the adjustments for that, it's a best that can be wrangled.

In my case, the problems come when I'm working over the KURT vise, which only leaves so much space under the z-axis carriage. One of the cuts I do often is a 9-then-12mm stepped bore through a 2" square bar...in one toolpath/feature so the holes are fully coincident. That means the bit is something like 2.5" long, the vise is 2.something tall, and the material is 2" tall...plus parallels to hold the block. That leaves all of about 0.6" of headroom at the very top of the Z, and if that gets exceeded, well we all know the hell that produces. Too bad the control panel won't let me lower it's safe height below 0.5". Scary! So dealing with those safe heights is yet another thing that, for a couple minutes, it pays to VERY closely find all references and settings and make sure they're right .

All that said, in a pinch when you can't get the Vectric (or other) software to cooperate, you can always manually edit the GCode (.tap) file. Those non-local safe-height Z-axis moves should be pretty easy to find at the very top and bottom of the file. If you are writing multiple toolpaths to a single tap file (in that they use the same bit), there might also be those same safe-height Z moves between the individual toolpaths. Okay, I admit it: I hack the bejeebies out of my GCODE and post processor files: I'm evil that way .

Hope that helps,

Thom

[edowney]

The modifying of the safe z is happening in the preferences section of the control panel. But the machine itself is acting wonky in general. My wife and I use it to cut designs into vinyl records so our work material is really flat and is held down by a jig with a bunch of nuts, bolts and washers. When everything was working correctly I would run the file from the control panel at which point the router would lift up a good inch or so travel to where it needed to start the cut and then drop down and do it's business. Now it immediately moves down to approximately 3/4" above the spoil board and begins to move over to it's start location which means it could potentially hit one of the bolts sticking out of the spoil board on its way to the place where it wants to start cutting. This is just different behavior then I've seen from it before - don't like it coming that close to the bolts

[Kayvon]

Do you have an old gcode file you could test with? You don't have to actually cut anything, just run it and see what happens. That would allow you to rule out the gcode and vcarve immediately, then we can focus on the control panel and hardware.

[edowney]

I was thinking the same thing. I loaded up a file that I had just cut two days ago and had not changed since. When I started running that file I saw the same bad behavior with how the router was moving from the start of the job. Does the control box have some sort of memory? I've already rebooted the computer that the shark connects to and power cycled the control box. We have another router (cheap china junk) and it turned out to have capacitors so not only did I have to unplug it but then I had to turn it on to drain the capacitor in order to get a real reset of the box. Forgot to try that last night on the shark.

[Rando]

There are no GCodes settings in the controller to "set" a safe height; they're all just G00 and G01's and such in the GCode. But, the controller does return to the start position after the cut (and you won't find that in the GCode). When I'm doing a cut that I'm worried will hit an outside clamp, I'll often jog the head so it's in the approximate center of the material/part, and "up" slightly above the safe height, then run the cut starting from there. That way, when it moves to the first XY location, the movement should be fully within the work envelope, and hopefully avoid the clamps/bolts. If that's not feasible, you can adjust the starting point so the straight-line move at the start of the cut doesn't hit a clamp, but that can be a little more difficult if the first cut point changes.

Regards,

Thom

[Rando]

The modifying of the safe z is happening in the preferences section of the control panel. But the machine itself is acting wonky in general. My wife and I use it to cut designs into vinyl records so our work material is really flat and is held down by a jig with a bunch of nuts, bolts and washers. When everything was working correctly I would run the file from the control panel at which point the router would lift up a good inch or so travel to where it needed to start the cut and then drop down and do it's business. Now it immediately moves down to approximately 3/4" above the spoil board and begins to move over to it's start location which means it could potentially hit one of the bolts sticking out of the spoil board on its way to the place where it wants to start cutting. This is just different behavior then I've seen from it before - don't like it coming that close to the bolts

Yeah, I know I already replied. But, I just thought of one other thing that might help. Two words: nylon bolts . When I'm indexing a part and there's a chance the bit might hit the vise or workstop, I use a nylon bolt/nut in the workstop instead of the default steel one. I haven't hit it yet, but at least if I do, fewer bad things will happen. Maybe using those will at least prevent disaster if they should hit.

[edowney]

Ok, I think this is a vcarve issue. I compared the top of the header file from two different tap files and noticed that one of my newer files has the z going down to .8 inches while the working tap file is 1.5 inches. So I looked at the bad tap file in vcarve and noticed that I got the job setup material thickness wrong I changed it to the correct thickness of .0787 inches clicked on ok and then edited one of the tool paths and noticed that the bottom with the Safe Z information still had the incorrect information. I tried recalculating the tool path. No go. Tried deleting the tool path and recreating it and the the safe z info is still wrong. How do I force that to change?

[Rando]

Weird!

Wait...you're saying the safe height setting on the material panel had no effect? Did the changed value "stick" if you go back into the panel? You clicked save in the Material settings panel, right? For me, these days with phone apps and computers and tablets all acting slightly differently, it's sometimes difficult to tell when changing a value takes effect immediately, and when I have to find the Save button. I know, I feel almost bad wondering if that's the case...who doesn't click Save, right? I just did a test in VCarve and the value changed...but like you said, only after I saved the value AND recalculated the toolpath.

Okay, here's the one question I think might resolve this. When you changed the safe height value, did VCarve warn you to recalculate all toolpaths, but did not actually do that for you? It's a pretty obvious warning, Windows error sound and all. If you somehow changed the value but did NOT get that, that's a good sign the value didn't actually get changed or saved. Attached is a screenshot of the notice I get:

Anyway, still scratching my chinny-chin-chin on this one.

Thom