Printable View
I have used a 1/32" ballnose on my final pass with 12 spacing.
attached in is an image showing the tool marks. Is the only way to smooth this out by decreasing my spacing which significantly increases my carving time?
I would appreciate any thoughts.
Thanks,
Groovy
the extra time it takes to run a 6 percent stepover will be a lot less than the time it takes to fix it by hand and the result is better.
What size is the piece? A 1/32" ballnose is pretty small and the design doesn't have that much detail. 8% stepover works well for most ballnose bits that I have used. Don't use the "Offset" strategy, use raster and make it raster parallel to the gantry. 3D work requires a proper set of ramp values tailored to the task or you'll get axis "jiggle" and possible lost steps with a standard controller. Also, make sure you have no play in any axis, adjust and tighten up as needed.
http://www.shopbotblog.com/2008/03/a...m-performance/
This is a tip I copied from an older thread I hope it helps.
Too much wasted time, just use the 3D roughing toolpath and use a 0.25" downcut end mill (not a ballnose) at 48-50% stepover with a machining allowance of 0.04" and up to 0.375 per pass depending on the quality of your end mill. Run it as 3D raster across the grain (keeps long slivers from plugging the dust foot). Then run the 3D finish toolpath across the grain as well with an 8% stepover. Done. You may think that a final finish pass across the grain will leave scoring, but with the proper tool and stepover, it will be fine and have a lot less fuzzies to clean up.
Phil
Scott will forget more about 3-d then i will ever learn. That said I am curious about the size of your model. Do you know how to determine which size ball nose to use? It would not hurt to post a preview of you tool path. I typically use 8% stepover
The best way I have found to determine what size ballnose to use is with the toolpath animation. For example start with a .25" ballnose and follow up with a .125", slow the animation down so you can observe the difference. If necessary follow up with a .062." Experience will help.Quote:
Originally Posted by cowboy1296
Phil
yup that is exactly how i do it. And if the differance in the preview is not so great go with the larger bit, if it is great go with the smaller bit.
JMO, but it looks like it may be the model. The tool marks aren't symmetric, so the model might require some smoothing.