Printable View
Hi,
Fusion 360 seems to require the cutter to be slightly smaller in diameter than the width of the slot. To overcome I have sometimes made the slot slightly wider or the cutter slightly narrower, by 0,01mm. Then it works. Is there any other possibility to overcome this problem?
Sketch some lines for the center of your slots, and use the lines for the toolpaths.
Most CAM software won't allow a slot the same with as the tool. Always model the slots slightly larger.
Double check there is no "stock" offset. Everytime I run toolpaths they default the "leave stock" option for some reason. Other work around is as GER21 says. Draw a slot sketch and drive off the stock. Mathematically there are always tolerances in software that can lead to small issues like this.
One other way to do it is to draw a line for the center of your stock in a sketch, and then use the "Trace" strategy to drive the endmill dead-center along your line. (this may actually be what ger21 is referring to above)
PM
Additional.... just made a quick test file. I was unable to cut the slot using the slotting strategy, even when following a sketch line.
I did, however have prefect results using the Trace strategy. (note that the sketch entity needs to be drawn at the bottom of the slot).
Here you go.... sample file: -----> https://www.dropbox.com/s/2pddbeoc26..._slot.f3d?dl=0
PM
you can always say it's a 3.99999mm endmill
Exactly !!! No redrawing necessary.Quote:
Originally Posted by daniellyall
The reason is lead in and lead out. If your drilling a hole, use the bore operation.
Stock left (so you can repeat the operation as a finishing cut easily) will do this, as will the lead-in/lead-out, as will too wide a helix radius if you're ramping in for HSM operations.
Hello, i had the same issue. I fixed it to an unlimmited minium by setting the tolerance in nthe toolpath lower than the additional diameter/distance in the slot/hole.
You can set the tolerance in the toolpath-settings under "passes".
hope it helps