How to remove fillets from a sketch?

66point99

I've added a load of fillets to my sketch, but wish to remove them (and apply them instead via the 3D tools, post-extrusion).

How do I remove a fillet from a sketch?

Related: in trying to figure this out myself I've inadvertently broken a number of lines into segments (by deleting the fillet curve, and then using the extend tool to hit the old corner) - is there a way to remove the redundant points along these lines?

Thank you!

3dcad

You can use Extend command to return the lines, if you don't mind some extra points; line tool might be even faster.

Then use Trim to remove fillet arcs. (Scissor icon in toolbar, Extend can be found in this same button under dropdown)

traveler_hauptman

This raises an interesting question... Why is there a sketch fillet tool? Is it ever a good idea to put a fillet in a sketch?

coleman

Traveler_Hauptman said:

This raises an interesting question... Why is there a sketch fillet tool? Is it ever a good idea to put a fillet in a sketch?

I like to put fillets in sketches when I KNOW there must be a fillet on a feature.  For example- if I am creating a pocket on a part that will be CNC milled....I know there must be a fillet in the corners (for the endmill).  This way I wont forget to add them later.  

traveler_hauptman

That's a good one. I use them when I need a specific wall thickness as well.

andrew_troup

I'm broadly with @coleman: if a fillet is intrinsic to the geometry of a feature, rather than being a superficial, optional finishing operation, I find models more robust to manipulations and future changes if that fillet is made part of the sketch.

There are too many instances to list, but one common reason is that the location of the tangent point (where a fillet meets an adjacent entity) needs to be finessed, and this may be difficult if the fillet is added as a feature at a later stage.

"Intrinsic" fillets which spring to mind include corners of the paths for swept O-ring grooves, profiles of rectangular hollow sections or pressings, or corners of lightening apertures or access holes ...

Another reason to sketch fillets is that in some cases, (say a rectangular box with faces drafted for casting) a conventional fillet will produce the wrong result, because it will have a circular profile on a plane which is normal to the edge being filleted, whereas we may require it to have a cylindrical profile on a plane which is parallel to the reference face for draft. 

This public model
https://cad.onshape.com/documents/076b3d5d142d4aefb2e89e0c/w/50f9ee88ffee48178c20c7dd/e/310a7896297a488c9e63d361
(shown in screenshot - click to see full size) illustrates this situation.

Because we want to counterbore cap screws at the corners, the mismatch will be visually jarring if we add the fillets as features.

It is true that a conic fillet can approximate the desired result more closely than a conventional one, but the tangent points will still be in the wrong place, unless we fiddle with the nominal dimension of the fillet, and we will also need to do some trig or fiddle about some more to determine the rho factor.
And even then, any future edits will require carrying out this iterative process all over again.

The simple approach is simply to add fillets to the base and top loft profile sketches (currently square-cornered rectangles).
This will automatically generate elliptical fillets which will intersect the top face as true circular arcs, about the desired centre.

traveler_hauptman

Nicely put! That would be good info to add to the training material.

billy2

I tend towards more features and less sketch entities. I'd add the rounds later. If you double click the pocket, you'll see a better representation of the pocket and it's size without the sketch fillets. The thought in the early days would state that less sketch entities produced a more robust part. We'd say no more than 10 sketch entities per sketch. Of coarse this was from our pro/e training classes so it's pretty old wisdom. 

coleman

@andrew_troup - nice post.  

3dcad

Good question and answers. All overlaping features should be gone through like this.

Beside the mentioned cases, I tend to use sketch fillets when creating a path for router (sweep) since this way I can re-use the same 'coordinates' on cnc program-editor to create fully parametric cnc program.

lougallo

@andrew_troup You are a word smith my friend.  Very well put.

jakeramsley

traveler_hauptman said:

This raises an interesting question... Why is there a sketch fillet tool? Is it ever a good idea to put a fillet in a sketch?

I use it mostly as a shortcut for tangent arcs between two lines.  If I am using my sketch as something that doesn't create an edge (such as a loft profile, guide curve, or sweep path), then I find it much nicer to make a polyine and fillet rather than make two lines an approximation then spend the time making tangent arcs.

For the most part, it is is easier to undo changes by making my sketches blockier and rounding edges off the part rather than having to delete/edit sketches.

traveler_hauptman

@lougallo Are there any thoughts about a wiki or other way to consolidate tips and tricks like this?

brucebartlett

traveler_hauptman said:

@lougallo Are there any thoughts about a wiki or other way to consolidate tips and tricks like this?

That an interesting thought, the community contribution to a moderated tips and tricks. The good stuff would have to raise to the top some how. Would these come from the forum or on an alternative platform? 

@lougallo what's the idea behind the zendesk support page  do many use this?

Dann

I know this thread is a tombstone but just for anyone still having this issue, I have found the solution: Change the sketch fillet radius to 0 and it will disappear.

martin_kopplow

At least they get invisible. They do not really go away, though. Draw a rectangle, make a fillet in one corner, set to R0, then delete the two tangent lines, see there is the fillet, still with it's dimension tag on it and three points plus all their coincident conditions. To compare, delete two other lines of the rectangle and see there are no points remaining at their former corner. I can imagine this might lead to downstream issues, so I'd be careful.

You could set the fillet to zero and then fence-select and delete it, of course. That will remove the the fillet together with all coincident conditions at the corner, though, and you'd have to reinstall one. After that, the model should be fine.