JMD2 wrote:Don't know if this has been covered or not.
I would like to setup a job, with the "Z ZERO" set to the spoil board and the cut starting at the top of the part. Every time I try this, the machine, CNC SHARK PRO, moves to zero, on the spoil board, then tries to starting cutting. This berries the cutter in the job and is not a pretty thing to see. Is there a work around for this? I am using the latest Vectric V-Carve Pro 9 program.
Thank you for any help.
John
When you set the origin (X0Y0Z0) at the bottom of the material, all your toolpaths have to then "start" cutting--that is, the TOP of the cut--from a value equal to the total thickness of your stock, then down to that height minus the cut depth.
As example, say you're cutting into a 3.25" thick piece of wood, and you want to cut a hole 0.7" deep. When the Z0 is at the bottom, that means the top is at +3.25, and the bottom of your hole is +3.25 - 0.70" = +2.55". So, your start of cut would be up at 3.25. If the software asks for "bottom", you give it the 2.55 number. If it asks for "total cut depth", you'd just use the 0.70".
But, there's also another aspect here. It might not be your toolpath at all, but the initialization positions (home position, heights) set in the control panel preferences, or in the software. Always make sure your home position and safe heights will result in the bit at the proper height. So in the example above, to keep 0.25" room above the stock (and to account for stock height variations), you'd set the start position / height as 3.50" (3.25 stock + 0.25 safe). As for the control panel, if you consistently use the spoil board for Z0, then make sure the control panel's safe height is above the thickest stock you use.
But, in the end, there's no substitute for VERIFICATION. I'm talking examining exactly where that toolpath will go, long before it hits a machine. For that, you want a "GCode Backplotter". It's somewhat like the Vectric Preview and Simulation facilities, but because it's working from the GCode, you can inspect things like starting heights, positions, etc. Likewise, because it's independently produced (not from Vectric), I know it's not going to be using the same algorithmic fiction that Vectric might have used. I use the one by CNCCookbook (
https://www.cnccookbook.com), their G-Wizard Editor. Fantastic, and more than worth the price*. When you load a toolpath into it, it will display a 3D rendering of where the tool tip goes. By simply clicking on the "Front" view, you can tell exactly where that bit is going to enter the cut, and ever part about it. Independent verification of toolpath output, to me, is crucial. I don't run ANY toolpath anymore unless I've first verified a whole bunch of things.
Hope that helps. The intricacies of machine, part and tool datums can get confusing sometimes, and tool entry is something the normal simulators don't do well at representing.
Regards,
Thom
* Lots of people whine...yes, WHINE...that GWizard costs money. Yeah, well 5 pcs of a good quality 0.25"D, 2flute extended-reach, 0.020" radiused endmill that can cut a 2" deep hole in a block of aluminum costs well nearly $500. Not running that 12mm D x 52mm deep bore through major validation will burn through those 5 endmills long before the bottom of the first hole is reached. The cnccookbook F&S and editor paid for themselves in literally the first major bore I passed through them. Feeds and Speeds, and toolpath verification need to become your best buddy if you want great quality, safe cuts, and most importantly: getting all the cutter life you paid for.