Nasty bug or weirdness with Project plus Offset

[Anonymous]

I wanted to make a rectangular block with a sort of squiggle cut in one surface. Also, I wanted to work out the geometry for the rectangle and squiggle in a base sketch (or top-level sketch if you prefer) before I started creating 3D forms. Here are my steps:

1. Start new model.
2. Make BaseSketch on XY plane - a rectangle with an inscribed curve (multiple line and arc segments) as a guidline for the "squiggle".
3. Close sketch
4. Make New Component1 and make sure it is activated.
5. Make base sketch visible.
6. Make new Sketch1 in Component1 on XY plane: a rectangle snapped to the BaseSketch rectangle.
7. Extrude the rectangle in +Z direction.
8. Make new Sketch2 in Component1 on front face of extrusion (offset from XY plane).
9. Use Project to copy curve in base sketch to Sketch2 - it appears as a connected series of lines and arcs with magenta color.
10. Exit Project command.
11. Select all the magenta lines and arcs and start Offset command.
12. Set offset distance and click OK.

Result: Offset lines and arcs are created but in the wrong sketch! They appear in BaseSketch even though Component1 is active and Sketch2 is the sketch being edited. These offset entities are of no use within Component1. I guess I could use Project again to copy them back into the sketch in which I am already working. But does this make any sense as a workflow: draw in base sketch, Project to component sketch, Offset back to base sketch and finally Project again to component sketch?

Here is the link for my test model: http://a360.co/25ThRNB

Additionally:
a) Using Offset on entities created by Project seems to be hit or miss. Sometimes all the selected entities get offset and sometimes only the one. The 'chain' option does not seem to work at all for projected entities. (saunde35 has already commented on this.)
b) For Project one must start the command and then select the entities. For the conceptually similar Offset one must select the entities and then start the command. Guys!!

[jeff_strater]

Hi @Anonymous,

Thanks for posting.  I agree that if this is reproducible, it is a bad bug.

However, so far I have not been able to reproduce the bug, either in a new design, or in your test model.

I do see the problem where offsetting projected geometry does not chain properly.  We'll continue to work on that bug.

One small point:  In your list of steps, you create the base sketch in the top-level component, but your sample model has it in Component1.  I don't think this should affect offset at all, however.

Here is a screencast of me trying to reproduce the problem:

The only theory I have is that somehow you were accidentally editng the base sketch, but that would have caused a rollback, and it would have been obvious.

If you can reproduce it in a screencast, it might give us some clues as to the nature of the problem.

thanks,

Jeff

[Anonymous]

Jeff - Thanks for looking at this.

My screencast is still pending so I can't insert it, but here is the link: http://autode.sk/1S9hilD

Here is what is happening: If the sketch in the component is being edited and is angled to the display plane then the bug DOES NOT occur (as you did it). If the sketch is aligned to the display plane the bug DOES occur (as I did it). This is not good.

I had an earlier conversation regarding Cut/Through and how it depended on component visibility. I commented then on the complicated ways that F360 mixes display and geometry to determine what action a command takes, saying that this could lead to problems for both users and developers. This seems to be a case of that mixing.

I also noticed other oddities that depend on the alignment of the sketch to the display plane. When it is aligned I can snap to geometry in the base sketch, which is on a different, but parallel plane. But when I then tried to select and delete one of the projected lines it would not delete; apparently the line in the base sketch got selected instead of the projected line in the active sketch. It makes things very confusing when the geometry (which is persistent) depends on how the display appears at the time of creation (definitely not persistent). I think this can lead both to bugs and an inability to create a consistent user interface. If F360 is intended to use Project to constrain to off-sketch-plane geometry (unlike Solidworks way of snapping to almost anything) then that should be consistently how it works. And when editing a sketch the geometry in the sketch should always get selection priority over any external geometry, independent of viewpoint. If there is a need for overrides then this should be deliberate rather than some side effect of the viewing direction. Certainly the user should not have to keep changing the viewpoint back and forth to create or delete geometry correctly.

[Anonymous]

It occurred to me that what is actually happening: When the sketch is aligned to the display plane and I click on a projected line the underlying line in the original sketch is getting selected instead. So there are really two problems, both of which seem serious to me:

1) The Offset tool will create offsets in any sketch, not just the one being edited. If sketch A is being edited and I click on a line in (a visible) sketch B then a new line is created in sketch B rather than sketch A. Is it possible that this is the intended behavior? Does it make sense that an accidental click could create nearly invisible additional geometry in a sketch that the user has no intention to edit? My take on this: Offset is a sketch tool; sketch tools work within the sketch currently being edited; therefore, Offset should only work within the sketch currently being edited.

2) If a line or other geometry in the sketch being edited directly overlies other geometry, shouldn't it still get priority for selection when clicked? Maybe this is Solidworks thinking, but isn't that the sensible approach? It is always more likely that you will want to work with an element in the current sketch than to reference some other geometry. Better to hold down the mouse button to get the other geometry when needed.

[jeff_strater]

Hi @Anonymous,

Sorry for the delay in replying.  Thank you for the thorough debugging!  You are absolutely correct - if you are looking straight down on the sketch, and if you pre-select the curves, offset puts the curves in the wrong sketch!!  

I will take care of filing this bug and seeing that it gets fixed.

Jeff

[Anonymous]

Jeff -

Thanks for the reply. Please see my additional post above. I realized that the "bug" is actually a combination of two other bugs (features?).

There is a lot to like about F360 and I am introducing it to a group of medical students who are creating a makerspace at their hospital. But I find myself returning to Solidworks because I keep running into these odd bug/features. They always seem to revolve around F360's odd (to me at least) mixing of (persistent) feature geometry and (non-persistent) feature visibility to determine how a command will work. I think that until this is sorted out F360 will keep having odd behaviors like the one I found here. I would be happy to have a conversation on this topic.

[Anonymous]

I tried several times but could`t reproduce the problem. I was looking straight to the sketch plane and it offsets to the right sketch.

I don`t know what you guys did

[Anonymous]

Interesting. Where you trying to offset a line that was a projection from
another sketch? What seems to be happening is that the original line in the
underlying sketch is selected instead of the line in the current sketch.

Michael Wollowitz
Tangible Design Inc.

[jeff_strater]

You may have to have the "select through" flag turned on to see this bug:

[jeff_strater]

@Anonymous,

Again, your debugging skills are correct (we should give you a job!).  As you can see in this screencast, that is exactly what is happening.  When you look straight down on the sketch, and just select sketch curves, (I think you have to have the "select through" flag on), you get the back ones.

I think (memory is foggy on this point) that I remember having a discussion where, if you have a normal curve and a projected curve on top of each other, we want to give preference to the normal curve.  Of course, that should only be if they are both in the active sketch.  I'm willing to bet that this is the problem.

I like your "makerspace for medical students" idea.  I do wonder what they will make there.

Regarding Fusion vs other CAD tools (I can't bring myself to use the "S" word  ), I understand your concerns here.  However, we hope that you continue to give Fusion a try.  We are a relatively young product, and a lot of these annoyances I would classify as "growing pains".  We certainly are striving to keep getting better all the time on these sorts of bugs.  Input from users such as yourself is very valuable in finding and fixing these.  In this specific case, I have done similar operations (projecting from one sketch to another) dozens of times, but, as you saw from my earlier screencast, I don't often sketch looking straight down on the sketch.  So, a wide variety of usage styles is important.

thanks again,

Jeff