Finished edges on 3D model

This forum is for general discussion regarding VCarve Pro
Post Reply
giametti
Posts: 14
Joined: Sun Mar 09, 2014 4:16 pm
Model of CNC Machine: Shopping for one

Finished edges on 3D model

Post by giametti »

I have a request to make a large quantity of wooden salad spoons. They will be mounted on Sterling silver handles and need to be of exceedingly high quality. The STL I'm importing seems to be detailed enough.
I tried to do it using 2 sided machining, but that doesn't work because I have to have different Z planes when orienting the model in order to machine the hollow of the bowl deeper than the rim of the spoon that must be machined from the back. (I have not used 2 sided machining before so if I'm setting it up wrong, let me know.)
Currently I'm running 2 files, one with the concave face up, and the other with the convex bottom face up. In both cases I have to orient the model's z plane low to machine the bowl front and back completely. I'm using a 1/4" ball nose to rough and a 1/8" BN for the finishing. This works pretty well except that the shaft of the spoon is not finished on the sides (the finishing doesn't go down to the center line of the shaft). I hope to get a nice tapering oval section along the shaft, that I would get if I were machining it on a rotary axis. These rough sides require a good bit of hand shaping with a fine toothed rasp to get a proper shape.
I'd like to avoid as much hand shaping as possible to keep my bid down. While I can machine using a rotary axis, I would prefer to do it two sided so that I can machine multiples on the bed rather that one at a time on the rotary. This would significantly reduce the time I spend changing bits and attending the machine where I could be doing other finishing tasks while the machine is running.
I'm currently using other software for my rotary work. Would upgrading to Aspire help improve the quality of the finished piece?
Any advice would be appreciated. This could be a lucrative project if I can solve some of these problems.
Jim Eddy

User avatar
ohiolyons
Vectric Wizard
Posts: 1701
Joined: Wed May 27, 2009 7:16 pm
Model of CNC Machine: Laguna IQ
Location: Kettering, Ohio

Re: Finished edges on 3D model

Post by ohiolyons »

What is your modeling resolution? Better be at least 7x. I would go even higher.

It can be a 2 sided job, you just have to assign negative depths to your zero planes to get all the way into the spoon area.
Watch the chess piece or marlin demo to understand 2 sided machining and negative zero planes.

You will know you zero plane is negative enough when depression in your spoon is all one color.

Normally your negative zero plane is the diameter of your finish bit according to the chess and marlin tutorials.
But you will have to go even deeper to hollow out the liquid portion of the spoon.
John Lyons
CNC in Kettering, Ohio

User avatar
adze_cnc
Vectric Wizard
Posts: 4324
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Finished edges on 3D model

Post by adze_cnc »

Without seeing the model you are trying to import / use it's very difficult to offer any firm suggestions. Can you take a screenshot (you can use the Windows Snipping Tool built into Windows 7+) of the STL file?

Depending on the model you might be able to just specify an "overcut" distance when importing the model rather than messing around with multiple zero planes and models with or without a negative something-or-other.

This image shows a model where the overcut distance is set to allow the cutter to cut down to the center of the fillet as pointed to by the red arrow:
 
overcut.png
 
lid.jpg
 
The only "zero plane" used was the default one that VCarve sets as the centre of the model.

Also, it might be possible to re-orient your model (again depending on what it looks like) to avoid odd cutting angles. Also, you might be able to model in a skirt in the originating 3D model software that will allow the bit to follow the complex edge. Both techniques I've done before.

User avatar
adze_cnc
Vectric Wizard
Posts: 4324
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Finished edges on 3D model

Post by adze_cnc »

Oh, I forgot. Are you sure that you want to use a ball-end cutter for roughing things out?

I always wonder why folks don't immediately choose a square-end cutter for roughing but rather choose a round-end cutter. Since the flutes of a round-end cutter come to a "point" that has very little if any cutting edge it seems to me a poor choice for roughing.

User avatar
SteveNelson46
Vectric Wizard
Posts: 2282
Joined: Wed Jan 04, 2012 2:43 pm
Model of CNC Machine: Camaster Stinger 1
Location: Tucson, Az.

Re: Finished edges on 3D model

Post by SteveNelson46 »

adze_cnc wrote:
Thu Mar 09, 2023 6:38 pm
Oh, I forgot. Are you sure that you want to use a ball-end cutter for roughing things out?

I always wonder why folks don't immediately choose a square-end cutter for roughing but rather choose a round-end cutter. Since the flutes of a round-end cutter come to a "point" that has very little if any cutting edge it seems to me a poor choice for roughing.
I agree. I've always wondered that myself.
Steve

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Finished edges on 3D model

Post by martin54 »

As others have said it is easier when you have something visual to work with :lol: :lol:
Uploading the crv file would be helpful but if that is not possible for copyright reasons then screenshots are the next best thing. :lol: :lol:

RickW3DS
Vectric Craftsman
Posts: 165
Joined: Sat Apr 02, 2022 6:55 pm
Model of CNC Machine: LongMill 30x30

Re: Finished edges on 3D model

Post by RickW3DS »

I do a lot of bowls and trays with a 0.25 ball nose bit for 3D roughing and finish paths at 120 ipm. Works just fine and one less tool change. You can run them at the same feed rate as an end mill for the roughing pass with same steppover for roughing. Combine the tool paths on export and just run it. I would not try that with smaller ball nose bits... Broke one of the smaller ones...

Post Reply