Compound radius with fluting tool?

This forum is for general discussion regarding VCarve Pro
Post Reply
User avatar
fretsman68
Vectric Wizard
Posts: 1084
Joined: Tue Sep 02, 2008 7:16 pm
Location: Pa. USA

Compound radius with fluting tool?

Post by fretsman68 »

Hi, all,

I'm trying to make a standoff box to mount to the side of a 5 gallon bucket. I'm showing a drawing of it below for you to help illustrate my part. The center rectangle is hollow, with the left and right ends showing the radiused features. I only showed the ends "pulled away" to the left and right to show the cut of the radii.

Now the 5 gallon bucket is a trepezoidal (technical term...lol) radius, so I'd like the mounting/mating face of my rectangle, to match the surface shape of the bucket. Is there a way to cut a 6 inch radius in the left end of the box, while fading into the 5 inch radius on the right side of the box? If so, do I have to cut the "whole" rectangle? Or is there a way to save time and just cut the top side of the hollow rectangle (in red)?

Did any of that make sense? lol!
Attachments
Inked5 Gal Stand-Off_LI.jpg
--------------
Dave

User avatar
FixitMike
Vectric Wizard
Posts: 2173
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: Compound radius with fluting tool?

Post by FixitMike »

Not exactly, but awfully close. The following assumes a piece 2" high and 6" long.
This method is based on the principle that the chord for the 5" radius is shorter than the one for the 6" radius. Thus the fluting drive vectors will vary from one length to the other as you cut from one end to the other. Some of the cut will extend beyond the material. There will be a very, very, slight slope to the resulting cut surface. And, with the fluting toolpath, there will be a 1/4" wide flat in the center.
The first picture shows the construction to determine the lengths of the vectors to be used for fluting.
Draw the parallel vectors for fluting. Draw them spaced at 1/16" for a 1/4" end mill. I trimmed them using the Trim selected Vectors tool so the lengths vary from one end to the other. The vectors are 1/4" shorter than the constructed ones, since they control the center of the end mill and it cuts 1/8" past its center on both ends.
The result is shown in the second picture.
T. Radius.png
T Radius.jpg
T Radius.crv
(593 KiB) Downloaded 42 times
Good judgement comes from experience.
Experience comes from bad judgement.

User avatar
fretsman68
Vectric Wizard
Posts: 1084
Joined: Tue Sep 02, 2008 7:16 pm
Location: Pa. USA

Re: Compound radius with fluting tool?

Post by fretsman68 »

Thank you very much for your work, Mike, I will look this over. Quick question, is it impossible to skip all the air cutting, and just cut along the sides?
--------------
Dave

User avatar
FixitMike
Vectric Wizard
Posts: 2173
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: Compound radius with fluting tool?

Post by FixitMike »

fretsman68 wrote:
Mon Feb 22, 2021 8:24 pm
Thank you very much for your work, Mike, I will look this over. Quick question, is it impossible to skip all the air cutting, and just cut along the sides?
There is only a little air cutting. It could be eliminated by calculating the depth of cut for each vector and having a separate fluting toolpath for each one. But I believe there would be a minimal time saving, and the work would not be worth it unless possibly you are intending to cut hundreds of blocks. In addition, one would have to do a lot of editing to eliminated the air moves from one vector to the next.

Most important is to not have a low plunge rate setting for the tool, since the feed rate for fluting toolpaths are often limited to the lowest of the tool feed or plunge rates.
Good judgement comes from experience.
Experience comes from bad judgement.

User avatar
fretsman68
Vectric Wizard
Posts: 1084
Joined: Tue Sep 02, 2008 7:16 pm
Location: Pa. USA

Re: Compound radius with fluting tool?

Post by fretsman68 »

Thanks again for your help and information, Mike-
--------------
Dave

Post Reply