Been a Carbide user a while now and use Fusion as my CAD/CAM software and drive the Shepeoko with CM. My setup requires a re-zeroing of the Z axis after each bit change (i.e., no automatic bit changer and no bit-zeroing device). Thus, when running a Fusion job with several operations and several bit changes, I must re-zero my Z after each bit change (though the X-Y settings, in this case set at stock center origin) remain the same.
I am new to 2D surfacing as a first operation, and what I am having trouble understanding is how I should set my Fusion toolpath settings requiring a different end mill subsequent to a surfacing operation. So, that is, if I create a setup using stock from a solid, and that stock is .25" thicker than my model’s top and has .25" of axial stock, if I run a surfacing operation first that skims off the excess .25" of top stock, how do I set the parameters for any operation (say a pocket using a different end mill) when I no longer have a “stock top” to which I can re- zero after the tool change? What I am finding is that if I re-zero the new bit to the newly created stock surface, after making the tool change, and then run the second operation, my pockets end up .25" deeper than modeled.
Should I be referencing Z from another location (say, the spoil-board) so as to maintain original Z? I understood that Fusion took into account that the surfacing operation removed stock above the model top and generated tool paths that accounted for this, but running this way produces cuts that are referencing from the newly created surface and still taking into account .25" of stock.
If you know the first cut was 0.25 deep, and your Z zero is on top of the stock (which is now gone).
Touch off to the new surface, and go to Set Zero and instead of clicking the Set Z Zero button, type in -0.25 and hit Enter.
In Fusion, your could create different Setups with the facing operation Origin at the stock surface and the rest of the operations under a Setup with the Origin on the Model Surface.
Or, what Tod said…
Or, zero off the wasteboard.
Or, get a BitSetter…it’ll change your life.
Without a bitsetter my workflow has been Fusion CAM file per tool and to almost always zero off the spoilboard or workholding jig, not the stock.
I also name the GCode files “Project - file number - tool name - zero position” to reduce idiot errors, e.g. “Phone stand - 03 - 0.25 compression - FLSBZ” where FLSBZ means Front Left SpoilbBoard Zero
If my stock is now .25" lower due to facing and I touch off on new face and type in -0.25, wont that tell the software to “start” .25" lower, thus making my first cut .25" deeper in the material than programmed? Seems like it should be +0.25
OK, so tried this. See question above to Tod re suggestion to type in - .25".
Tried doing multiple setups using the stock top for first origin and model top in subsequent setups and operations. Also tried setting cuts off the spoilboard. While depth of cut is accurate, the machine cuts air on subsequent setups because the program still assumes the stock height is where it was before surfacing (that is, stock mode–second tab on setup–is set to “from preceding setup.”
So, the only solution I have been able to find so that depth of cut remains correct AND the machine does not cut air at the beginning of each toolpath subsequent to facing is to switch the stock tab setting in a subsequent setup to reflect stock that is .25" less tall.
Oh, and BTW, I did order a bit setter. For a $100 or so bucks it should improve my workflow.
When you touch off to the surface after cutting, your cutter is -0.25 in relation to the original zero which was 0.25 higher than where you are now. When you type in -0.25, you are telling the machine, “I am at -0.25 right now.” After typing in -0.25, move your cutter to Z0.0. Where is it? Right at the old zero, correct?
When you hit the “Set Z zero” button you are telling the machine, “I am at Z 0.0 right now.” It just types in the 0.0 for you.
I use this trick a lot. After cutting a surfacing toolpath, either for my wasteboard or for the initial stock for a part… after the cut the tool moves up and back & waits. If I want to remove another 0.010", and my cutter is now at Z3.123, I just open the Set Zero dialog & type in 3.133. Now the machine thinks I am 0.010 higher than I was, so when it move back down to zero it will be 0.010" lower than last time.
I just hit Start → Start & cut it again.
Thanks to all for the answers. This was, as always, helpful advice from the community.
I ran my job using the method I described in my last post. That is, I did a second setup, changing my stock source to one that reflected a lower z-height by the amount taken off with the surfacing.
