depending on the time of the year, mine will look similar.  more humid?  hotter? you'll get that... if it's an issue, use sanding sealer before cutting- do whole sheet of ply right there on the table... it dries in like ten minutes even in heat and humidity... it'll eliminate or at least reduce the shredding of the veneer.

in other words, it's more of a material issue than one with the machine... unless it's an engineered composite, you'll get that.

I have a SVC 4x4 and I just cut out a few patterns in a 1/2 inch piece of plywood.  After putting the second piece of plywood on the machine for the next cuts, it wont go through the plywood as instructed.  I powered the machine off then back on.  reset the X, Y, and Z axis and it still will not go through the plywood like it did earlier.  I re-installed the post processor and that did not fix it.  I regenerated the file from another computer in the house and still acting the same.  Can anyone point me in the right direction for a solution.  I even manually set the Z axis without the puck and that did not work.  I am out of options.

Regards,
Connal

how much does it 'miss' from going through?  plywood is rarely consistent in thickness, sometimes (and often) from one side to the other. 

are you using v-carve?   

How would a G offset behave any differently? Are the G offsets not relative coordinates themselves?

two seemingly conflicting statements:

so when you move your machine over to where you want the origin to be by aiming for the corner, center, ect, and assign that as 'home' (origin) the machine is absolute from that point... you actually changed your absolute base coordinate, but you placed it in a relative (arbitrary to the machine) place.  once your g-code starts being parsed, it'll 'consider' the moves absolute from that (relative) point...

the machine and the cut path being given to it via thumbdrive+gcode file aren't connected- the machine just does as it's told.. but, you can 'tell' the machine to do things PRIOR to it digesting the code- and can even do so WITH the code. 

the machine is absolute until it's told to think relative.  it's even then absolute, but from a relative position.  it just does exactly what it's told with the only concerns being "you can't go this far or that far, else crash, and i won't let you do that"....

yes, in direct response to your question, an offset is relative to something/somewhere.   you can either plop that relative (user defined) origin at a known location (to either you or the machine) or from just some place in space the machine doesn't care about with the exception of making certain it's within the work space envelope.  by leveraging one of the pre-defined offsets and having THAT ALSO as your 'user origin', you've just mapped out precisely, in code and repeatable programmatically, where that location is... so long as your workpiece is placed in precisely the same place (using registration points?) you can use that position as long as you want without changing a thing, and by either directing the machine to 'origin' OR by programmatically calling the corresponding offset (g57 as example) in the gcode. 

the machine is absolute- and the offsets are absolute positions- the relative comes in after the offset is called, as all moves are now relative to the offset not machine home or user defined origin.

Is it practical to setup G offsets for one-offs? Sincere question - I haven't played with them much.

maybe not... but what IS useful is homing the machine (mechanical zero) and then jogging to where you want user defined origin to be, and before assigning it as such- jotting down those coordinates.... I don't do this that often... i do it when i'm working on a piece that either i'm going to have to remove and then cut again (painting, perhaps?) or a piece that is hard to replace.  IF you choose this manner, you can toss out the jive above in the first question. 

I did consider writing down the mechanical coords once my origin was set. Is there a "Go To" type function in the HD-100? E.G. Go To 250,350,30

not that i know of there is no "go to this place" button... but it can be done by populating an offset BEFORE the gcode is introduced and moving relative from that point, OR, it can be brought up programmatically by either going to the predefined offset location, OR, by entering a line in the code by hand right after the GO X0 Y0 Zsafe that says GO X250 Y250 Z30.... i've done it both ways...

to be forthright, I don't have a single offset programmed in my DSP controller.... i just make mark of the origin's coordinates from mechanical zero and i use registration blocks to press the material up against... which works out the same without all the confusion or different approaches.   and to further present, i got one of those 300 win mag rifle casings with a laser pointer in it... if I lose position in space on an irreplaceable material, i'll slap that thing in the collet (300 winmag fits nicely in a half inch collet) and run code well above the workpiece and with the spindle off, and to make sure the cuts are where they should be.  i'll often 'cut air' above an expensive work piece with the same gadget before running the cut, just to make sure.   

There is a little block in fusion that's way too easy to look past... it refers to g51,54,55- the offsets.. I haven't seen a post processor for the hd100 in quite a while, but I can tell you when autodesk introduced that option a couple years back it wreaked havoc with folks not knowing where the problem was..... turns out autodesk populated the offsets with a value and if you didn't deselect that option, you'd have an offset...

Scour the beginning of the gcode for any of those g5x codes... it'll appear but once after the headers and before the first cut.

Fusion/autodesk annoys the hell out of me when they update, as even reading the release notes doesn't always describe all the changes... they force the update (cloud) and then don't mention a tiny alteration, and that alteration then cascades into other things... that dang offset back when was a doozy to figure out. 

Edited to add: the offset isn't present in your design- it's added to the output code before be processed to gcode... that tiny little check block asking about "use g5x?" Is where it's controlled/toggled. 

I don’t talk with anyone from there, anymore.  I've no clue what they've published or not published.  I may, maybe, post up what I provided them for owners manual which had a section in there about maintenance... though that was for S series DSP...

Re:repeatability.... if your game is production and running the same files over and over, there are tricks... one I like the best is to set "home" to actual mechanical home, and then set your origin/datum to an offset of something shoved up against your registration pins/block. 

The machine has to be indexed upon power up- it finds those by coming back to trigger the limit switches on the low x, low y, and high z... then, it bumps off of them a specific distance.  You see this every time you turn your machine on and home it... make that your machines "origin" too...

Then, bump over to your registration pin/block closest to the mechanical and machine "home/origin"... write that down, and assuming you're using the lower left aka low x and low y...

In vetrics (or autodesk) set your machine bed size to the limits of your movement, and make a template to reflect that.  Then, when assigning your origin, use an offset which is the coordinates you wrote down. 

^that is pretty much foolproof.  If you lose degrees using that method, you've got big problems as it's using the machines thoughts of what's mechanical home as it's origin, and that shouldn't ever change. 

You can get fancier... I had a routine programmed once that used the same mechanism as the z-zero macro... m105 or something like that (I refuse to memorize m or g code... its too easy to screw up, so I reference a list every time I dig into hard scripting code)... basically, the machine moves until its interrupted... its interrupted by a closing of a circuit attached to the z axis...

what the script did was akin to a xyz touch... an xyz touch, for those who dont know, lowers the z axis and finds the closing of the circuit (surface of material) and retracts a short distance sorta like the z touch... what it does then, which is commonly used in machining, is it moves over a specified distance beyond the corner of a square metal plate on the x axis, drops below the surface, and slowly moves toward the plate... when it touches it, it rebounds a short distance and z retracts again... then it moves over job speed to the same coordinate except y axis this time- drops the z and slowly moves to the plate.. when it touches it, it stops and rebounds. 

That^ xyz touch ensures your material is square to the axis(s) and finds the top of the material. 

My script was different but using the same idea... instead of the two or three inches on the x or y, it would move out to the corner of the material and where I also had a registration block planted. 

I chunked that entire prospect after using it a few times because it took so long to use it that I may as well have manually found home..... that... and DSP has no means to reconcile an error other than just stopping... and...  while messing with the actual code inside the as211 is dangerous of you don't know what you're doing. 

The xyz touch (or zxy as it was) is handy but only for visual confirmation your material is squared.. dsp has no way to interrupt the rest of the code if it isn't.  So, you're standing there watching the operation with your thumb on the cancel button, which takes away any advantage of automating it.... if your registration blocks are right and your origin is good, all you should be interested in is z'ing...thats the rapidedist and mostest accuratedest way... good blocks/pins and knowing exactly where they are in terms of coordinates.

Insofar as maintenance, keep the machine clean.  Rails, motors, electronics.  I use the oiler- never more than five seconds of squirter which is just enough time to load pressure enough to move oil... I also spray all moving parts with silicone spray once a week at least, run the machine to every limit immediately afterward, and then walk away until morning when I'll wipe off the excess.  The silicone dries and leaves a film on the rails and cogs- one that is dry and doesn't collect dust/debris as oil or grease does. 

That's pretty much it, though this post turned into a book I typed with my thumbs.. please forgive the typos.

That's the difference between a clean design and a not so clean..... I love aspire, as it's quick and easy to create something 2D... but... make a circle which is four arcs, right? Now, use the function to place a ring around it a certain distance away while not deselecting the corner/angle option... if you enter node mode, you'll see the circle (still four arcs) but the other one? It'll have a gazillion nodes which are tiny straight lines....

As for the design manifested? If it's wood you likely won"t notice... acrylic, though? You'll see the jagged little edges instead of a smooth cut.  You'll also see in the code one that uses four lines of code for that circle when using arcs... when using a ton of little short lines between a bunch of nodes, that is a literal ton of code...

One of the things i love about this job is i dont manage people with personalities- instead, i tell a computer what I'd like to have... if it doesnt respond predictable, then the fault is mine as it just does exactly as its told.... reminds me of the joke the c+ programmer was sent to the store by his wife with instructions"get a jug of milk and if they have fresh bananas, get six"... he comes home with six gallons of milk.... and he was in the right because her logic failed.