Cannot create arcs on rectangle in sketch

[fsonnichsen]

This should be basic. I am trying to use the 3-point arc command to crate an arc on the end of a rectangle in a sketch.

I make 3 clicks. One at each vertex of 2 vertexes of the rectangle and one between the two. It does not work.

Clearly I am missing something simple here

https://autode.sk/3b2Dotm

thanks

fritz

[jeff_strater]

turn off 3D sketching - the triad is getting in your way:

[fsonnichsen]

Jeff-removing the 3D Sketch option from the Palette did not help

https://autode.sk/37bRG9N

thanks

Fritz

[jeff_strater]

Is the rectangle in the active sketch?  Is it on the sketch plane?  If you can share the file, it will likely be pretty easy to find out more

[fsonnichsen]

Thanks Jeff. This is a 2 component file. After sketching and extruding component 2 it will be subtracted from component1. I have done this before but probably not used the arc command. I was of the impression that components are quite independent of one another. Here is the complete file

Fritz

[jeff_strater · Accepted solution]

OK, that helped a lot.  The problem is that this rectangle is not on the sketch plane.  So, my advice to turn off 3D sketch was exactly wrong.  But, it's hard to tell just from a screencast that this geometry is not on the sketch plane.  So, turn on 3D sketching.  Then, you can pick the rectangle corners, but you do have to zoom in to pick the other corner (so I was right that the triad was getting in the way.  Then, for the third point, it will default to the wrong plane.  Then, you have to pick the correct plane, and you can then create the arc.  See the screencast.

But, the bigger question is why the rectangle is not on the sketch plane.  Was that intentional?

[fsonnichsen]

Thanks Jeff. That solved the immediate problem. It opens a whole bigger question about 3D sketching. 

First to answer your question--no--I had not intended to leave the sketch plane and I am not sure what happened. 

Not having any organized  written documentation for 360, I cannot be sure what is intended in its design principles, but up to this point I have viewed sketches as somewhat like perpendicular planes in an orthoscopic projection as used in old fashioned drafting. So I always keep sketches on a plane in my mind at least. 

    I am not sure where fusion 3D sketching is used or if it has to be used but I will look thru the 2500 or so entries on this topic under "product documentation".  It sure looks interesting.

  The following entry was useful and I put it here for others to see:

https://www.autodesk.com/products/fusion-360/blog/fusion-360-tech-tip-sketching/#:~:text=There%20is%....

Clearly this entry indicates that I can turn off 3D sketching for now so that this does not happen again.

Many thanks for your time

Fritz

[jeff_strater · Accepted solution]

To be honest, I'm not familiar with any really good documentation on 3D sketching in Fusion.  I suspect there are some good tutorials out there, but I'm just not familiar with them.  But, here are a few points to be aware of:

• All Fusion sketches are inherently 2D and 3D, regardless of the state of that setting.  This is fairly unique to Fusion.  Each sketch has a sketch plane, which is where the "2D" geometry lies.  You can draw a rectangle on the sketch plane, then use Move to move it out of the plane, rotate it, etc.  Then, the lines in that rectangle become "3D" geometry.  That may well be what happened to the rectangle in your model
• The "3D Sketch" flag is more accurately described in the preferences dialog:  "allow 3D sketching of lines and splines".  All this option does is enable some creation commands (lines, splines, and some others) to create geometry that is not on the 2D sketch plane.  You can snap to model geometry, or use the triad to easily sketch on planes other than the sketch plane.

Jeff

[fsonnichsen]

Thanks Jeff.

 I looked some more and I can guess where 3D sketching may come of use. It seems to prevail in "pipe like" structures but also splined curves in 3 space.

     I guess one of the problems in general with drawing tools is that there are so many different approaches that lead to the same results. And these occur both within a given tool or between them. Probably keeps the machine visualization guys heads spinning!

    Your help was useful and I will stick to the "old fashioned" orthoscopic way of thinking for now. I was able to get my simple construct together now.

cheers

Fritz