Help with Point Round over bits

Software Carbide Create
1

I just bought a few point round over bits. Specifically Whiteside 1570 and 1572. I bought them because I am a round over type of person (lol). I like things smooth on the edges and I have lots of ideas in my particular style of art. I envision a lot of my projects being edge finished with these, inside, outside, all the sides.

Before I start breaking these new bits I figured I’d get some advice.

Take the 1570 as an example, it is 3/16 radius, 3/8 cut diameter, 3/8 cut length.

First, how do I add this bit? The point is narrow. It’s measuring .05" at the tip. So I would add an endmill bit in the toolbase that has that diameter yes?

Second, to get to the absolute edge and NOT touch the wood with the point, I would have to create an offset of .05 for whatever I am rounding? (and go to a depth of 3/8") Is this correct?

Third, do I need to make/run two projects? I am thinking so. I don’t want this bit plunging into any wood.

Let’s say I want to make a circle, the diameter is .5", I use a 1/4 bit to pocket, but that leaves no stock, so if I set up a new path with the offset (or even without), it will not cut anything, there will be no moves. So I need a second project right?

I am new to all of this but I know CC has limitations. If I use a 1/4 endmill bit to pocket out the circle, that leaves no stock if I then switch to a thinner bit, CC will not “see” what a point round over bit is doing, and thus… there will be no path. If I run the round over first into uncut wood, I risk breaking the tip.

I just don’t want to break a bit testing…

2

Carbide Create doesn’t support this endmill geometry and can’t do a 3D preview using them.

I looked into this a bit at:

You can use them using offset geometry if you’re willing to work w/o a 3D preview.

3

I have one of those and … its nice

you are right you want to make an outside offset (0.02" is likely enough).
You also want to run this bit after part of the cutout phase obviously and out of paranoia I ended up doing a extra broad cutout (basically a 2nd cutout pass to the depth I used the roundover pointy bit at an extra offset to make even more sure there was space for the bit)

so what I did (my stock was thick enough that I did not need to go all the way in with the roundover bit)

  1. cutout (outside contour) to MOST of the depth (leaving 0.05" or so for work holding)
  2. cutout (outside contour) at an outside offset of half the diameter of my cutout bit also to this depth
  3. then an outside contour with 0.025" offset with the roundover bit to a depth I liked (I tested this by hand)
  4. final cutout contour to full material depth

I ended up adding it as a V bit but… it doesnt really matter, it wont simulate “correctly” either way.

2 Likes
4

Will, I am aware of the limitations, you’ve helped me before on that :grinning: I am just curious as to how to go about setting it up (tool paths) in CC for the final result. Preview doesn’t matter.

My issue, in my mind at least, is how to use the round over without plunging the tip when something like a circle is already pocketed out. I have a circle, it’s cut, now I want to round over the top edge of that circle perfectly, like a wormhole opening. I assume I have to make a different file and run it because otherwise CC would not have a path to cut as the round over point is “cutting” air and thus would not generate a toolpath.

So, I have to duplicate the complete file and all the round over paths be the only active toolpaths… or something like that and at the same time be sure that my round over paths are offset by half the width of the tip of the point round over bit.

Am I even explaining this correctly? LOL.

5

As @fenrus noted, just offset by the tip radius (and a bit more for safety) and then plunge down by the rounding radius (less the bit more added for safety) and use a no-offset contour toolpath applied to that geometry.

If there are any acute points on the original geometry you’ll need to edit/adjust the offset geometry accordingly.

1 Like
6

I just setup a test. Just a simple .5" circle. and an inside offset path of .025 (half of the round over point tip diameter).

I selected the first .5 circle used a 1/4 endmill for the pocket, created that toolpath. I selected the offset, added the new tool, adjusted it’s max depth to the depth size of the round over (3/8). Preview. No tool path generated for the round over toolpath. Which I expected to happen. So I am missing something.

I know if I run it a second time, export a new nc, with the first pass disabled, it will work, but how to get it to work in the same file?

edit: ok weird, tried it again, just deleted toolpaths, added tool paths now it looks like there’s a tool path for the round over… wth? Is CC “blind” in this regard, will it run the second toolpath or not? Note this is really the only thing I am concerned about, I understand the geometries.

7

the toolpath should just work. As Will said, just do a contour path with no offset and CC will “blindly” create the gcode as if it was a flat endmill… it doesn’t know any better :slight_smile:

1 Like
8

Great, so I guess this is an instance where a software limitation is a good thing? :rofl:

9

I would like to think of it as a great feature: it’s a “do exactly what I tell you to” feature that … is sometimes underappreciated in fancy “fashion like” software nowadays

2 Likes
10

Could you fake it by increasing the actual bit diameter by 0.04", twice the offset?

11

that works (assuming you want to use this for an outside contour)

1 Like
12

Would cambotics show the roundover?

13

I don’t believe so — one can set up a “Stub” endmill as a dovetail, but I don’t believe there’s a way to set up a cove radius endmill.

14

This topic was automatically closed after 30 days. New replies are no longer allowed.