topic Re: HELP - fillets in Fusion Design, Validate & Document Forum

HELP - fillets

Ariel — Mon, 11 Jun 2018 11:51:30 GMT

Ok, this has been bothering me for sometime and I thought I might bring it to the attention of others and see if they are being held back by this.

Attached is a pic of the before and after from the fillet and you will notice that the fillet function does not retain the length of the contacted extrusion. It extends the extrusion I have created, but only in parts where it needs to. This causes me some grief when I have to then design the part which this is located in. Just to explain a little further, I work with a 3mm recess in the adjoining part, but I will have 2mm+ which extends past this recess. Not a nice look in my opinion and unfortunately for me no real work around.

Now as for a solution, I am completely stuck

- A revolve of a circle/arc will not work since it comes in contact with different surfaces and therefore the tangency is different. This eliminates this as a possible solution.

- leave it without a radius and play around with fillets options on the CAM side of things. I am yet to try this, it is something that just crossed my mind. This is where I need people with more experience on the CAM side of things to chime in (I know it isn't the right part of the forum)

Ideally, what I would like to see if a consistent radius fillet which is tangent with all the surfaces it comes in contact with, without modifying any existing features and therefore reduce the likelihood of chatter during roughing or finishing if I was to add no fillet.

Happy to share as many screen shots as possible, but I can not share the file.

Thanks,

Ariel

Any thoughts or ideas would be much appreciated.

Re: HELP - fillets

jeff_strater — Mon, 11 Jun 2018 15:13:35 GMT

I assume that you are talking about the thickening in this area:

While this is undesirable for your design, it is the correct result, geometrically. A fillet is a blend between two surfaces, and that surface extends onto that tab.

There are a couple of ways that I can think of offhand to work around this. I would probably try to isolate the tab from the rest of the geometry, for the purposes of that fillet. You might be able to rearrange your timeline (assuming you have a parametric design), so that the fillet is added before the tabs are added to the design. You might, also, be able to use Split Body to temporarily remove the tabs, then add the fillet, then put the bodies back together again.

Re: HELP - fillets

Ariel — Mon, 11 Jun 2018 21:23:29 GMT

Hi Jeff, it actually thickens that complete extrusion all the way around. I have tried both your suggestions but with no success. It still adds to the flange (extrusion) thickness.

Re: HELP - fillets

jeff_strater — Mon, 11 Jun 2018 23:23:51 GMT

That is pretty much what Fillet does for a concave edge - it adds material to both adjacent faces. If you want to keep that entire flange a constant thickness, I'm not sure that Fillet is the correct tool to use. Perhaps I don't understand what geometry you are trying to get to with this operation - can you sketch out what you think the result should be? If you want to keep the flange constant width, then the adjacent face (indicated by the blue arrow below) would have to shrink in order to have a blend between it and an adjacent face. Any additional information you can provide would be helpful.

thanks,

Jeff

Re: HELP - fillets

Ariel — Mon, 11 Jun 2018 23:47:40 GMT

Hi Jeff, I can't really sketch it since the fillet comes in contact with several faces. What I would like to achieve is a fillet which is tangent to all the surfaces, remains a constant radius and doesn't modify any features. So the fillet created increases/decreases in (chord) length accordingly, while maintaining the same radius.

Re: HELP - fillets

Anonymous — Tue, 12 Jun 2018 00:40:21 GMT

I believe I have found a solution using the Sweep + Guide Rail tool, though I'm not sure if this is exactly what you're looking for.

I first isolated the area in which you have a protrusion in the flange using a patch surface + split body tool.

To set up the sweep, I created a side profile of the fillet I was looking to create, which was just a quarter circle. I then went and created a spline curve on the face of the flange as the "limit" for the fillet, you can adjust this to whatever amount you desire, even selecting the edge of the flange before the sweep is created.

Create a sweep using the quarter circle as the profile, the original connecting edge as the path, and the spline (or whatever curve you choose) as your guide rail.

This should define your special fillet in the protruded area of your flange. You can create fillets normally in adjacent sections, then join the bodies if you choose to.

Hope this helps,

Shihao

Re: HELP - fillets

Ariel — Tue, 12 Jun 2018 07:39:16 GMT

Thank you Shihao. That does the trick and is exactly the end result I would like but I am sure we can both admit it does so in a very long winded and time consuming manner.

Any idea why it does not produce that result as part of the fillet function when selecting a line?

Cheers,

Ariel

Re: HELP - fillets

Anonymous — Tue, 12 Jun 2018 13:49:07 GMT

For something slightly faster in exchange for less control, use variable radius fillets:

As to why your original raised the height of your flange, here's a visual for what Jeff was explaining.

In order to try and match the large radius that you give it, Fusion automatically raises the flange in order to have the same initial top height and radius.

Re: HELP - fillets

Ariel — Tue, 12 Jun 2018 21:35:56 GMT

What is the chance of having the functionality to create this style fillet with out modifying the base features and simply creating a fillet as a tangent to the adjoining faces? Like below

Re: HELP - fillets

Anonymous — Tue, 12 Jun 2018 21:44:52 GMT

In that case, there must first be a heard break between the different height sections (such as done by a split body). Then the resulting file will be nonuniform in that there will be no smooth transition.

(I also didn't quite understand what you were trying to show in your previous image >_<

Re: HELP - fillets

Ariel — Tue, 12 Jun 2018 21:59:52 GMT

Just trying to show how the fillet moves up the surface (green fillet on the right) to satisfy the geometry all while remaining tangent to the surface/s and not modifying the existing geometry.

Looks like I just have to live with it or go the long way about it.

Re: HELP - fillets

TrippyLighting — Wed, 13 Jun 2018 00:12:39 GMT

Please mark one of the answers as the solution.

Re: HELP - fillets

HughesTooling — Wed, 13 Jun 2018 10:00:09 GMT

@Ariel wrote:

Thank you Shihao. That does the trick and is exactly the end result I would like but I am sure we can both admit it does so in a very long winded and time consuming manner.

Any idea why it does not produce that result as part of the fillet function when selecting a line?

Cheers,

Ariel

Some programs have an option to hold a fillet to an edge, I'm pretty sure inventor does so it's probably just not in fusion's UI. I've seen the way a fillet's added in Fusion flip to holding an edged at some sizes as well so there is some logic\ability in Fusion you just don't have control.

Here's an example from another program.

Mark

Re: HELP - fillets

HughesTooling — Wed, 13 Jun 2018 15:41:19 GMT

Here's a workaround that might work, add a small fillet around the outer edge first then add the convex fillet.

With the small fillet added first the convex fillet holds the edge and doesn't increase the thickness of the flange.

Mark

Re: HELP - fillets

Ariel — Wed, 13 Jun 2018 22:03:38 GMT

"hold fillet to an edge" that is exactly what I have been trying to verbalise, thank you!!

I have tried it in Inventor but had the same result. Edit - I just got it to work with a 1.1mm fillet on the extrusion edge and 6mm fillet on the line.

It would be nice to have "hold fillet to edge" added to the UI.