Big ballnose for chair butt?

[EricSchimel]

Hey all, I'm going to be doing some 3D milling of some chair bottoms. They are those standard wooden chairs that have that carved out section for your butt, just like this:

29412

I'm thinking of using a bigger ballnose. The plan is for me to hog out the wooden blanks and the woodworker will hand sand them to a smooth finish. If I were doing one of these I'd probably just do it with my 1/4" ballnose one afternoon when I had nothing else to run, but I'm going to be doing 50 of these so I'm thinking I'm going to need a big ballnose to make this effecient.

Has anyone done something like this before? I've got them model all set, I just need a recommendation on a bit if anyone's got one...

[guitarwes]

Probably need to get a bowl cutter bit or run a 3D toolpath with a large ballnose.
Ajcoholic does these I believe.

[EricSchimel]

Perhaps a 3/4" wide version of this (http://www.toolstoday.com/p-4969-core-box-router-bits.aspx?variantids=5688,0/?gdffi=df1cb0f3ab644accbe5cae9671f148bf&gdfms=B06AD62428AC41D99A253CD36292A4F2&gclid=CjwKEAiAvs7CBRC24rao6bGCoiASJABaCt5D49UH-XvBZTkHieNmH_EUm9MPCLKPsabW5QtcUSNYLxoCaULw_wcB)

[Gary Campbell]

Eric...
I've cut them for a customer, used a 1 1/2" core box from magnate

[Ajcoholic]

I do cut a fair number of chair seats in my shop. Ive always used an Onsrud 5/8" diameter solid carbide, two flute spiral bit. I generally use about 7% or 8% step over (allows for a very smooth surface with little sanding to do).

I dont run a roughing toolpath. I usually start at the rear of the chair seat and work my way forward, going back and forth 90degrees to the grain direction.

I have often thought about trying a larger diameter bit. But, with my method I cut the average seat in 15 to 20 minutes. Im a custom shop, not a production shop so its fine for me.

1/4" would be pretty slow though, and youd have to slow your feed and depth of cut might be an issue. I cut at 360 to 400 IPM with that 5/8" bit.

[richard_saylor]

Not to hijack the thread, but how does one go about creating a tool to use a large cove bit? For instance, 1 3/4" dia., 1 1/2" radius, 5/16" depth.

[Kyle Stapleton]

Your number do not add up, your radius must be half or less than half of you dia.
That said, you need to make a new tool in your database by drawing only the right side of the tool.
http://screencast.com/t/fPENtZOjx99v

[richard_saylor]

Item #
Large
Diam.
Radius
Depth
of Cove
Carbide
Height
Shank
Size




#7873
1-3/4"
1-1/2"
5/16"
3/8"
1/2"




http://www.talkshopbot.com/forum/attachment.php?attachmentid=29443&stc=1
From your post I am assuming this is only possible in Aspire?

[Kyle Stapleton]

Ahh.
Here is an ex: http://screencast.com/t/6m3vjp839Z1E
Numbers may be a little off, just winging it, but you should get the idea.

[Gary Campbell]

Richard...
You can enter that as a 3" ballnose with a .3125 depth of cut if you are only going to cut 5/16 deep. If you will cut deeper then enter it as a form tool

[richard_saylor]

Thanks to both of you for the fast replies.
I used Kyle's great example and made a form tool.
Funny how you can use something for so many years and still not have a clue what it's capable of.