Negative fillet radius?

michael3424

I'd like to put an inside (negative?) fillet on a part, much like you'd get with a ball end mill, but can't see a path forward.  Is there a way to do that?

My part is a 1/4-in high octagon and I'd like to put a 1/8-in inside radius around the top edge.  I can do each edge separately by extruding a circle, but that has to be done on each of the 8 top edges and seems too convoluted.  Another work around just occurred to me - use a octagon sketch to put a ledge around the edges and then do a standard fillet at the ledge of the corner.  That's still convoluted but much easier.

Anyway, if there's no way to do it with a single tool now, could OnS please add the request to the wish list?

Mike

3dcad

Just sweep through path.

- Draw circle on separate sketch
- Sweep that sketch and choose edges of octagon as path.

pete_yodis

Michael3424 said:

Thanks - that worked with a little fiddling around.  User error, probably, by not paying attention to what field geometry selections are being placed in.

I still think it would be useful to able to specify a more direct to do this - does negative radius for something like this make sense or would it lead to issues?

Mike

I think your request would only be for outside edges, in which case the method recommended by using a swept cut would work just fine... or swept body cut if that's in store.  I could see some really strange results in inside corners and inside edges if the fillet tool created "negative" radii.  I think it couldn't be applied well to the full scope of cases the fillet tool would be used for.

michael3424

I'd like to put an inside (negative?) fillet on a part, much like you'd get with a ball end mill, but can't see a path forward.  Is there a way to do that?

My part is a 1/4-in high octagon and I'd like to put a 1/8-in inside radius around the top edge.  I can do each edge separately by extruding a circle, but that has to be done on each of the 8 top edges and seems too convoluted.  Another work around just occurred to me - use a octagon sketch to put a ledge around the edges and then do a standard fillet at the ledge of the corner.  That's still convoluted but much easier.

Anyway, if there's no way to do it with a singletool now, could OnS please add the request to the wish list?

Mike

3dcad

Just sweep through path.

- Draw circle on separate sketch
- Sweep that sketch and choose edges of octagon as path.

michael3424

Thanks - that worked with a little fiddling around.  User error, probably, by not paying attention to what field geometry selections are being placed in.

I still think it would be useful to able to specify a more direct to do this - does negative radius for something like this make sense or would it lead to issues?

Mike

pete_yodis

Michael3424 said:

Thanks - that worked with a little fiddling around.  User error, probably, by not paying attention to what field geometry selections are being placed in.

I still think it would be useful to able to specify a more direct to do this - does negative radius for something like this make sense or would it lead to issues?

Mike

I think your request would only be for outside edges, in which case the method recommended by using a swept cut would work just fine... or swept body cut if that's in store.  I could see some really strange results in inside corners and inside edges if the fillet tool created "negative" radii.  I think it couldn't be applied well to the full scope of cases the fillet tool would be used for.

3dcad

I agree with Pete, it would be a very specific tool for narrow segment and kinda overlaping with sweep. Sweep will do the work and let's you easily modify the shape of edge / groove in whatever you wan't.

What I would like to see in future after all the basics are there would be sweep tool that acts like 5-ax router and has easy control over depth in different points and angle of the tool. I would like to just draw profile of blade into 'blade library' and then choose blade, add depth/angle points set path with offsets and see the result. Currently even the simpliest paths in 3-ax machine with any varying in depth needs a lot of modeling to follow real world. Usually it's easier to take a piece of mdf and test the looks in real world rather than try it on cad.

Here's example of simple shape that takes less than 3 minutes to program and run with cnc (ball head router) and far longer to model in 3d. If someone want's to give it a try, ballhead R=4mm, depth on both ends = 2mm, depth on intersect = 1mm

andrew_troup

@Michael3424

Another way to create your rebated octagon would be to provide a plane, set at 22.5 degrees from your construction plane. Extrude the cross section shape you want, complete with rebate, up to that plane. Mirror the resulting wedge. Circular Pattern the resulting wedges and combine into a single solid.

I created a demo model using that method, which anyone can open at
https://cad.onshape.com/documents/5bc9292bc9e9417482eace51/w/6e93f7910b86460499c6a1b8


 To my way of thinking, an essential feature of a fillet is edge tangency, which locks down the geometry. Hence the radius alone is sufficient to finalise a fillet. Even the 'sign' does not have to be specified: a "negative" (concave) fillet is automatically applicable to an inside corner, while a "positive" fillet is a convex round to an external corner.

A rebate with a semi-circular profile, which is what you appear to need, is a concave rebate to an external corner. Unlike a fillet, no tangency is inherently specified, so the result is indeterminate. 

Given that such a rebate is so different from a fillet, and requires extra information, it seems to me it would be misleading to use the same tool to create it.

Fillets are universal (I can see dozens from where I'm typing this) and intensely functional: they make prismatic shapes durable and safe.
Whereas rebates are a styling feature in most cases, and the profile of the fillet (and the location of the centre of that profile) is whatever the  stylist wants it to be.

michael3424

Thanks all - I'll withdraw my request for negative fillet radii on the off chance that someone at OnS took notice..

I was frustrated at spending too much time to find a decent solution, but it appears that as is usually the case in such matters the problem was in the user, not the software.  I'm coming here after many years with Alibre/GeoMagic and differences in the UI have me doing some operations with the wrong selections - it's taking a little time to re-orient to OnS's way of thinking.

Andrew - I tried the approach in your example and was able to simplify it a little by playing around a bit.

Mike

andrew_troup

Mike

Care to share your model? I'm absolutely in favour of simplification

michael3424

Andrew,

I tried to make a sample file public.  If I got that right you should be able to get to it from this link:

https://cad.onshape.com/documents/393a1daa601340eebc193e3d/w/a8ec4819978e4b2085630fc4/e/f63bf800728b4ed8bb8fefa2

Mike

PS - I see the file in my Public folder, so let me know if it isn't there.

3dcad

@Michael3424 Did you make the octagon sketch manually or using 'Inscribed polygon' -tool? If manually, then I suggest you to try that tool..

Though, I don't like any tools where you can't go back and edit. That's one reason why I'm great fan of Alibre, I can always go back to edit in same dialog which was originally used to create things.  

michael3424

I used the inscribed polygon tool to make the octagon.  The spinner for the number of sides usually throws me at the end, but it will be become second nature eventually.  That part is the base for a scale model of an Otto-Langen IC engine from 1867 and I'm really looking forward to check out assembly mates after another 50 or so parts are done.  It looks like OnS assembly constraints will be a breath of fresh air after Alibre's.

Mike

3dcad

Michael3424 said:

.. It looks like OnS assembly constraints will be a breath of fresh air after Alibre's.

Mike

+1 for that, 1 constraint per part saves a lot of mouse clicks

fastwayjim

3dcad said:

Here's example of simple shape that takes less than 3 minutes to program and run with cnc (ball head router) and far longer to model in 3d. If someone want's to give it a try, ballhead R=4mm, depth on both ends = 2mm, depth on intersect = 1mm

This is as far as I coud get until OS adds more functionality: https://cad.onshape.com/documents/abad47877aa34b38b439b178/w/61ebfd28679b43c5a9c048a1/e/569d6ac863ae40aea68888f1

It took me 10 minutes to create, between opening the browser window and starting to right this comment, the longest part was futzing around with the curve geometry to mimic your picture. It would prob take me 5 more to finish...

Features needed in OS to finish this:

1a. Allow the boolean intersect feature of two surfaces to create a 3D curve, OR
1b. A "project" feature which allows me to project a sketch onto a surface, thus creating a 3D curve, OR
1c. 3D sketching
AND
2. A sweep feature which supports a 3D trajectory.

So close!

3dcad

@FastwayJim  Don't you wan't to create a plane to each endpoint normal to the tangent and create tool shape with different 'depth' to those planes. Then sweep between geometries and finish the ends with revolves? Or is this loft?

My problems with this approach:
- I wasn't able to create planes normal to tangent of curve endpoint (maybe I'm missing something here?)
- I wasn't able to perform sweep from circle to another (I suppose it's a loft when it goes from figure to another? - which is not supported yet)

so basicly I was stuck in the beginning..

fastwayjim

@3dcad - You have to think about the way this is machined. It is a simple sweep with a 3-D trajectory. The cross-section of the sweep, is the mill itself. Since this is a 3-D path, I'd probably create a second part, and use a Boolean to remove the material. This way, you could avoid having to micromanage the sketch's "normalness" throughout the trajectory, and also avoid having to "round the ends" like you mention.

When creating a new plane, select the "Curve Point" option, as this allows you to create a plane through a curve endpoint and normal to the curve itself. I just added one to that public model if you want to check it out...