Ball nose bits

[sawkerf]

I need to know where to find a ball nose bit to carve some extruded moulding. I need to carve as deep as 1 7/8" so a regular bit won't do. I have over 200 linear feet to carve so I would rather not have to rough with an end mill first if possible. TIA, Kip

[Brady Watson]

Hate to say it...but, you're gonna have to rough with an end mill 1st. There's no way you are going to get good detail without doing a roughing pass or breaking lots of bits.

Your other option is to buy a small molder and get knives made. The job sounds big enough to pay for it.

-B

[hines]

Here is someone who has been popular amongst the botters.

http://www.beckwithdecor.com/Cutters.html

[sawkerf]

Brady, I have a Shop Fox molder but it won't cut deep enough to the job, 3/4" max depth of cut. It takes a major molder to go 1 7/8" deep. I managed to get the extrusion process and toolpath worked out, so now I'm thinking I can copy just the deepest portion of my vector and rought out that part with a big honkin bit and then finish up with the ballnose. WHEW! this is tough goin' for a cabinet guy, all I do is cut out suqares and rectangles. It's like goin' straight from pre-school to graduate school! Oh, How long do you think it would take to run a 5 3/8" W x 96" L ?
Obviously the stepover makes the dif, but what's a good guess? Also, how do you set the depth of cut when using the Extruder? I haven't had time to figure that one out yet. Thanks Dave, That's exactly what I had in mind.

[Brady Watson]

Kip,
You'll definately want to do a quick hog out of the deepest part, leaving yourself .03 of meat on it for the ball to clean up. Here's the trick...cut the 1st few passes slowly, let's say 1.5 IPS. After it gets into the piece and you see the chips coming off, crank up the speed. MAKE SURE that you are rastering in the X direction. Cutting an 8' piece in the Y will take 8 to 12 times LONGER!!! So after doing the 1st few passes, crank the speed up to 5 IPS. See how it handles it, adjust RPM if needed. If all goes well, I don't see any reason why you can't run it at 7 or 8 IPS since it is only taking off a little at a time in Y (this depends on your step over).

My advice would be to make yourself a long vacuum pod that allows you to swap material on and off of it. A ShopVac will hold it down if there are no leaks. Leave the hogging bit in & hog out all the parts (after you try running one whole part to finish to see if the hogging & 3D toolpaths work)...Then you have no tool change until it's time to run 3D. The pod will work better than a large table with bleeder (which probably won't work at all for this application)

-B

[conceptmachine]

Kip,
I havn't tried it on the bot yet,but on my cnc mill i have roughed out the part with a ballnose and it worked great!machine along the x axis with a stepover of .01 in the y axis and you should get a good finish,but remember not to cut deeper than the LOC on your cutter.