Bit and Toolthpath

This forum is for general discussion regarding VCarve Pro

Bit and Toolthpath

Postby JMOlshefski » Mon Jul 22, 2019 1:33 pm

I have a 2 inch thick piece wood, I want to cut into a circle, however, I want the top of the piece (circle) to be 5 inches and I want the bottom (circle) to be 5 7/8, how do I create a toll path to tapper it out from the 5 to the 5 7/8 and with what bit?
JMOlshefski
 
Posts: 23
Joined: Sat Nov 22, 2014 11:32 pm
Model of CNC Machine: CNC Shark II

Re: Bit and Toolthpath

Postby dealguy11 » Mon Jul 22, 2019 7:49 pm

The moulding toolpath is your friend here, with a ballnose bit. For something this large and simple, I'd use at least a 1/4" ballnose. If you want the bottom of the taper to be sharp, you'll need to extend the toolpath beyond the thickness of your material so it cuts either into the table or into a sacrificial piece underneath the good material. The bigger the diameter of the bit, the deeper you'll need to go.

Edit - since you're using a Shark, I wouldn't go any bigger than the 1/4" bit.
Steve Godding
D&S Artistic Woodworking http://www.dsartisticwood.com
User avatar
dealguy11
Vectric Wizard
 
Posts: 1445
Joined: Tue Sep 22, 2009 9:52 pm
Location: Henryville, PA
Model of CNC Machine: Anderson Selexx 510

Re: Bit and Toolthpath

Postby 4DThinker » Mon Jul 22, 2019 11:46 pm

You can also use the fluting toolpath with an endmill. It will eliminate the need to cut deeper than you board is thick. Use the circular array tool. Start with a single vector from edge or the inner circle to the edge of the outer circle. Move the line over 1/2 the diameter of the bit (.125") before using the array tool to copy it. I used 360 vectors that ended up about 1/16" apart. For a smoother conical face use more. Example provided.

6 inch cone 4D.jpg
Attachments
6 inch cone 4D.crv
(227.5 KiB) Downloaded 19 times
4DThinker
Vectric Wizard
 
Posts: 1276
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro

Re: Bit and Toolthpath

Postby JMOlshefski » Tue Jul 23, 2019 12:43 am

THANKS
JMOlshefski
 
Posts: 23
Joined: Sat Nov 22, 2014 11:32 pm
Model of CNC Machine: CNC Shark II

Re: Bit and Toolthpath

Postby JMOlshefski » Tue Jul 23, 2019 1:28 pm

Two follow up questions, I have not used the molding or fluting toolpaths yet:

With the molding tool how am I drawing my circles and how do I set the deep of the cut, in the profile toolpath I select the number of passes?

Thanks for the sample with the fluting toolpath, it really help understand the "How" it was going to work, but same question as above , there no number of passes to set in the fluting, how does the bit clear matetial away without plunging down 2 inches?

Thanks
Joe
JMOlshefski
 
Posts: 23
Joined: Sat Nov 22, 2014 11:32 pm
Model of CNC Machine: CNC Shark II

Re: Bit and Toolthpath

Postby Adrian » Tue Jul 23, 2019 1:39 pm

The moulding toolpath cuts as deeply as it needs to do the job. It won't plunge 2 inches in your example though as that wouldn't be respecting the angle of the cut.
User avatar
Adrian
Vectric Archimage
 
Posts: 9703
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Bit and Toolthpath

Postby 4DThinker » Tue Jul 23, 2019 2:32 pm

JMOlshefski wrote:Two follow up questions, I have not used the molding or fluting toolpaths yet: There no number of passes to set in the fluting, how does the bit clear matetial away without plunging down 2 inches? Thanks Joe

You can do a profile pass around the outer circle to eliminate the need for the fluting pass to cut all that wood. Make sure the circle of wood is held down as the entire perimeter will be cut. I will use a hot glue gun or super glue with blue tape in those cases.

I set the pass depth to 2 inches because after the first plunge, every following plunge is only skimming off 1/16" of wood as it plunges. I usually slow down the feed speed manually in the controller software until the first plunge is done as it will want to hog out the full width of the bit. You could also separate the first plunge from all the rest, and give it a shallower pass depth so the slope will be cut gradually rather than all at once. Follow with all the rest of the vectors plunging 2" as the quickest way to get the job done.

4D
4DThinker
Vectric Wizard
 
Posts: 1276
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro

Re: Bit and Toolthpath

Postby dealguy11 » Tue Jul 23, 2019 4:00 pm

Whether you use a fluting path or a moulding path, you have same issue at the bottom of the part if you use a ballnose to make it. See the picture. The circle represents the tip of the bit. There's a little curve at the bottom where the bit meets the table.

Moulding bottom.JPG


You can either stop at the bottom of the part, and then run a profile path to cut off the little curve at the bottom, or you can continue down into the table a little less than the radius of the bit. Option A leaves a little flat to be sanded off. Option B cuts into the table. Pick your poison. To implement Option B, you would make your profile vector for the moulding toolpath a little larger (increase both width and depth proportionally). If the toolpath starts at the top of the material block, then it will then automatically go a little deeper as it's cutting.

Between the 2 options (moulding and fluting) I find the moulding toolpath to be easier to set up and use, but that's me. I know a lot of people have used the fluting approach for a long time and it works for them.

Edit: One more point. However you cut this, you are going to need a fairly long bit. The profile on the edge of this piece is 7/16" wide, so your collet is likely to hit on the top if your bit is too short.
Steve Godding
D&S Artistic Woodworking http://www.dsartisticwood.com
User avatar
dealguy11
Vectric Wizard
 
Posts: 1445
Joined: Tue Sep 22, 2009 9:52 pm
Location: Henryville, PA
Model of CNC Machine: Anderson Selexx 510

Re: Bit and Toolthpath

Postby JMOlshefski » Tue Jul 23, 2019 5:42 pm

The bottom is not an issue the piece will actual be 1 7/8 when done, my idea was to just cut off 1/8 on bottom on band saw, that way do not have to worry about securing I'll just clamp down four corners.
JMOlshefski
 
Posts: 23
Joined: Sat Nov 22, 2014 11:32 pm
Model of CNC Machine: CNC Shark II

Re: Bit and Toolthpath

Postby 4DThinker » Tue Jul 23, 2019 9:24 pm

dealguy11 wrote:Whether you use a fluting path or a moulding path, you have same issue at the bottom of the part if you use a ballnose to make it. See the picture. The circle represents the tip of the bit. There's a little curve at the bottom where the bit meets the table.
Using the fluting toolpath for tapering a shape you use an end mill.

4D
4DThinker
Vectric Wizard
 
Posts: 1276
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro

Re: Bit and Toolthpath

Postby dealguy11 » Tue Jul 23, 2019 10:15 pm

Interesting. I guess I've been using Aspire for carving so long that it didn't occur to me to use an end mill. It would leave a scalloped finish, but I guess the ballnose leaves a slightly scalloped finish, too, and on a regular shape like this there isn't a lot of difference. I still like the moulding toolpath because it seems like it would be faster going around the part, but would be interesting to try both and compare.

Before the moulding toolpath came along I used to make curved crown moldings. The carving toolpath was set up to run up and down the face of the molding rather than lengthwise with an offset carving path, because it produced a much better finish. It took forever to cut. Nowadays I use the moulding toolpath for that kind of work, which provides a much nicer finish and dramatically shorter cutting times than either of the other approaches.
Steve Godding
D&S Artistic Woodworking http://www.dsartisticwood.com
User avatar
dealguy11
Vectric Wizard
 
Posts: 1445
Joined: Tue Sep 22, 2009 9:52 pm
Location: Henryville, PA
Model of CNC Machine: Anderson Selexx 510


Return to VCarve - General

Who is online

Users browsing this forum: BigC, Google [Bot], ozymax, Ronwoodson2, sylvan356 and 12 guests