Need help with vbit chamfer

[machinemoney (Chris Hayes)]

There must be some obvious solution to this but I’m feeling braindead thinking how.

Lets say I pocket out this shape with a 1/4" end mill. Each corner will have a radius because the end mill can’t get into that tight corner.

So my plan for chamfering was just to create an inner offset, but in my design the shape has hard corners and doesn’t factor in the left over radius. I can’t easily add the radius onto the corners.

I feel like I’m missing something.

[Geeber (Brian Sewell)]

A chamfer is not going to work. You probably want to use an Advanced V-Carve toolpath which is actually two toolpaths; one that hogs out the majority of the pocket with an endmill, followed by another toolpath using a v-bit that pockets areas which the endmill won’t fit and to “square-off” corners tighter than the endmill radius. Be aware the v-bit toolpath will also taper the sides of the entire pocket at an angle equal to the bit.

This is a screenshot of the simulation using a .25" EM and 30° V-bit.

Hope that helps

Brian

[Tod1d (Tod (with 1 'd'))]

Offset inside by the radius you want. Then offset outside by the same amount. Viola! Radii

[Jeffish (Jeff de Ruiter)]

If you are using CC Pro just use the rest machining option after you clear the pocket with the 1/4 endmill

[WillAdams (William Adams (Carbide 3D))]

Note that Carbide Create has 2 specialty corner rounding tools in addition to the inset/offset method mentioned:

The Corner tool:

will find suitably straight edges with corners:

while the Fillet All tool:

will round everything:

(often it’s easier to use the latter and then restore straightness where wanted)

[mhotchin (Michael Hotchin)]

You can pretty easily convert a given shape into the shape you would get when cut by a given cutter. See here for more info:

Chamfer tight letters

How to convert a shape into the perimeter that actually gets carved by a tool of a given diameter. [image] For text, you’ll need to Convert to curves. The first step is you need to separate the Outside cuts from the Inside cuts. In this case, the only Inside cut is the center of the ‘e’. Here are the Outside cuts: [image] Now offset by the radius of the tool. For outside cuts, offset Outside, Inside cuts offset Inside. This basically creates the path that the center of the tool follows…

Once you have the ‘actual’ shape, then things like a chamfer are easier.

[machinemoney (Chris Hayes)]

Thanks guys, big help!

[Tod1d (Tod (with 1 'd'))]

Another thing to consider. You probably don’t want to try to cut with the sharp point, so you’ll want to offset the cutter as well. Draw the part, chamfer & tool in a side view & measure the depth & offset needed…

[BubbaOriley]

Since a 1/4" endmill can’t get into the corners, there’s no reason not to create fillets in those corners for your vector. Creating a 3.175mm or 1/8" radius fillet works perfectly for a 1/4" endmill. Then just cut inside the line with your endmill and on the line with your V bit. Perfect chamfers every time.

[machinemoney (Chris Hayes)]

Looks great, I like the more subtle chamfer and thin wall look instead of the bulky large roundover style and thick / deep pockets.

That piece looks around 0.75" thick am I right?

[BubbaOriley]

23mm. The deep pockets are 14mm and the shallow one 7mm.

[machinemoney (Chris Hayes)]

I’m having an issue, not sure what’s going on

I create my offset, select contour (center) and the toolpath line generates in a strange way that isn’t precise.

Any idea why this is happening?

[WillAdams (William Adams (Carbide 3D))]

That is a preview optimization/shortcut for performance’s sake in the 2D view — the actual cut will be as shown in the 3D preview.