SOLIDWORKS Design & Help

This fillet's radius is 1 cm (10 mm)...

I've just modeled it in SW 2016 without any problems:

Hi, there is no problem with the construction of a fillet in Solidworks 2016.

If you need I can throw off the model.

These are its 3 sketches in order:

In Sketch 3 - Which one are you using fillet or Arc. I have tired different methods if I give fillet feature or Arc (Sketch) its working.sketch fillet is not working.

Tangent Arc

A good practice in Solidworks if you are adding fillets and chamfers is to add them after the sketch and boss are complete. This makes it easier to go back in and edit your sketch if needed. Based upon the new edited dimensions you will be warned of invalid geometry if the old fillets/chamfers are too "big" for the new dimensions.

That's why I made an arc, not a sketch fillet.

Besides, making fillets as separate features increases the file's size, so adding them in sketches - when possible - is a better choice.

That's wonderful! In his original statement the term fillet was used, not arc. It all still depends on what relations you use and how many times you plan on coming back and touching the sketch to modify it as well.

Check the attached file. Maybe this helps. Solidworks 2016

https://we.tl/t-r33OIX07jQ

Unable to attach file here,

You get this error because you have two perpendicular lines, and the sketch fillet radius you try to apply is equal to the length of one of the lines. It means that it should delete one of the lines and this way replace two lines with a line and an arc. Sketch fillet simply cannot do that. It can only replace two lines with two lines and an arc, so when the radius is larger or equal to either line length you'll get an error message.

You can get around it quite simply: just make a sketch fillet with a smaller radius that works, delete the short line, merge the two endpoints, set the right radius and make the arc centre point coincident to the line on the other side.

Just one note: It's pretty obvious that you're miles away from being able to decide how to do things in Solidworks. Believe me, its not that simple. In fact, fillets are usually better be applied as a feature than in the sketch.