Inventor CAM - Follow a 3D fillet with a ball nose?

[tdswanson]

This is not my IP, so I really shouldn't post the part.  I've cut this part with a 12mm ball nose using the 3D contouring strategy.  It came out fine, but the filleted areas could be better.  This seems to be due to the nature of the "top down" section by section nature of the 3D contouring strategy.

I've messed around quite a bit and is there not a simple way for me to just force the bottom center of the tool to follow the selected lines?  FYI, the fillets in the model are R6, so everything should match up quite nicely.

The parallel strategy (second pic below) seems to come close, but it's still just basically moving the section-by-section work from a vertical strategy to a horizontal one.  There's got to be a simpler way to slick up the corners.  Suggestions?

[lenny_1962]

First: you should use a smaller Dia. ball, say 6mm.

Second: have you tried blend? include the fillet.

Third: try a pencil cut to clean up the rad. use your 12mm ball.

Red is the edges you'll pick for Blend and yellow are the faces for blend.

Not sure if Blend in IVCAM is in beta mode as it is in HSMWorks. I use the heck out of blend for areas like this.

[tdswanson]

Hey Lenny:

These parts are proto parts that will eventually be cast.  I'm just up against a huge profile tolerance, so there's no dimensional worry, I just want them to look decent.  Don't really wanna use a smaller tool and then have to step over a bunch of times.  We typically just match tools to the fillets and go.

It doesn't appear that Inventor CAM has the blend strategy.

In the side that's shown, what I found that works is the Trace option.  But it works out best not to choose the contour lines that represent the bottom of the tool, but rather the side lines where the fillets meet the vertical wall.  Then add your sideways offset and a negative axial stock by the ball radius.  This worked very nicely and smoothed out the contour interruptions very nicely.

As a side note, it's curious that (at least in Inventor CAD), they've placed "Trace" in the 2D milling section.

Thanks!

[lenny_1962]

read this and it will show you where blend is

https://forums.autodesk.com/t5/hsm-support-forum/flow-toolpath-symmetry-issues-split-path-and-wrong-...

[lenny_1962]

---

@tdswanson wrote:

Hey Lenny:

These parts are proto parts that will eventually be cast.  I'm just up against a huge profile tolerance, so there's no dimensional worry, I just want them to look decent.  Don't really wanna use a smaller tool and then have to step over a bunch of times.  We typically just match tools to the fillets and go.

It doesn't appear that Inventor CAM has the blend strategy.

In the side that's shown, what I found that works is the Trace option.  But it works out best not to choose the contour lines that represent the bottom of the tool, but rather the side lines where the fillets meet the vertical wall.  Then add your sideways offset and a negative axial stock by the ball radius.  This worked very nicely and smoothed out the contour interruptions very nicely.

As a side note, it's curious that (at least in Inventor CAD), they've placed "Trace" in the 2D milling section.

Thanks!

---

All I do is prototypes that have to look good so that's why I suggested smaller tool and Pencil. I don't use trace, I use project instead.

I'm a Model Maker by trade so it is hard for me to let it go as is.

Never hurts to try something cause I bet you'll need it somewhere down the line.

[lenny_1962]

here's a Pencil (12mm ball) and Blend (6mm ball)

[tdswanson]

That's pretty cool.  First I've heard of blending.  I've got it turned on and I'm playing with the program now.  Thanks a bunch.