Chamfer magically extends to new surfaces

ty_brown

Good morning!

I've been using Onshape for years now, and while I seem to run in to issues fairly frequently, it's typically due to the keyboard-to-chair interface (Me).

I'm trying to build a stackable frame, leveraging opposing cuts and ribs that fit in to each other.  I'm trying to cut (chamfer) the edge of this floor, while leaving the walls unchanged.  Depending on where I click to indicate the chamfer, different walls get included.  However, no matter how I cut, lay out guidelines, or mutter curses, I can't get it to chamfer WITHOUT cutting the walls.  Heck, I've got the cut set for 2.5mm, but it appears to take much more from the walls (following the created plane).

Is there a way around this?  Is this intended behavior? (If so, it would be amazing, if you could somehow exclude/include it with a radio button or something)

I think I know the fix for THIS drawing, but I'm really trying to learn how this works so I can teach others.

Many thanks!

wayne_sauder

@ty_brown
Have you tried unchecking the tangent propagation? 

S1mon

Hmmm. That's a fun one. As a work around, I would probably convert the chamfer to an extrude/remove and do it up to faces. Alternately, you can split the part chamfer the edge(s) and boolean the parts back together. It's also sometimes possible to add "stopper" extrusions (temporarily) and then delete face/heal the extrusions afterwards. I've done that kind of thing a lot with fillets that try to go too far.

wayne_sauder

@ty_brown
 I better understand your issue now. Please vote on this improvement, it is something that is needed for problems like this.  https://forum.onshape.com/discussion/19599/add-partial-edge-functionality-to-chamfer-feature#latest

steve_shubin

S1mon said:

As a work around, I would probably convert the chamfer to an extrude/remove and do it up to faces.

Yup !

S1mon

It would also be interesting to see what it does if you add the chamfer before the grooves. It looks like they have circular profiles. Sometimes it seems like the kernel has issues with things intersecting surfaces that are >= 180 degrees of a cylinder. Is this a public model?

steve_shubin

S1mon said:

It would also be interesting to see what it does if you add the chamfer before the grooves. It looks like they have circular profiles. Sometimes it seems like the kernel has issues with things intersecting surfaces that are >= 180 degrees of a cylinder. Is this a public model?

Wow !

I don’t know if I ever would have speculated that the grooves were giving a problem to the chamfer — but that’s exactly what it was

I put the chamfer just before the extruded grooves, and BINGO !! It worked like a champ

that is some very nice thinking there Simon

https://cad.onshape.com/documents/84deb3efe2f268cb8271f17f/w/494215775b1a248437be6cdc/e/573decaf94abaa7cf85f65b6

The model is public. I just looked at the name in the screen captures up above and typed that into the public search and it came right up

S1mon

@steve_shubin
Hmmmmm. I played with it a bit myself, and it seems to based on the number or location of those grooves on the open side. If I leave these two off, the chamfer still works after the grooves. I really don't understand what the issue is, but it seems to be some sort of weird topology problem. In any case, I would tend to put that chamfer before the holes/grooves anyway.

On a side note, Sketch 6 has 30 X 1mm diam circles. Each one is dimensioned. Unless they might all need to be different sizes later, I would select all of them and make them equal, and only have one diameter dimension. I might consider patterning features instead of making a sketch like that, but it all depends on how the part might need to change later. I'm also not a big fan of imprinting on faces. The selection for Extrude3 is crazy. If you turn off imprinting, and only make the holes/grooves solid lines, there's one selection for Extrude3 -- Sketch 6. Instead there are a zillion faces to select and manage.

Also Sketch 1 has a weird issue at the half circle which is causing a thin sliver of a gap in the part. I'm guessing this is unintentional.

ty_brown

Oh wow!

This is my first time posting after years of using this product.  I am blown away at the effort you folks put in to your posts.

It never occurred to me to try dragging the Chamfer up higher in the draft.  I've watched so many videos, and read so many tutorials. I just missed this obvious feature.

I'll apologize for the "dirty draft".  It looks like my programming code.  I've been learning all of this on my own, and when I'm really into a project I pursue that (and don't learn new tools).  What I need to do is step back and learn some new tools.  When I finally got a hang of my Sweeps and Revolves (Still cause occasional problems, as you can see by the mess), my work really progressed to the next level.

I think I tried the Tangent Propagation button (It literally sounds like the feature I was looking for), but I don't think it had the effect I was looking for.  I'm almost positive I didn't try it with the three different Chamfer selection points.

Moving the Chamfer higher in the stack absolutely worked.  I'm getting ready to put the item on the printer.

Then, while it's printing, I'm going to be going over this thread to learn.  There's literally concepts here I've never heard of.  I can't tell you folks how much I appreciate feedback like this.