No More Magenta Projected Sketch Features

[beardytroll]

The magenta projected sketch features are really frustrating, the entire point of making separate sketches is to keep the sketches clean and clear. But you still need to reference external geometry and sketches. I thought the deselecting the "Auto project edges on reference" box in the preferences would solve this but so far it seems to make absolutely no difference.

The problem. Start a sketch, draw a circle, extrude to cylinder, start a new sketch, draw a rectangle, make an edge tangent, close sketch, hide the cylinder body. At this point the last sketch with the rectangle is the only thing showing, but it includes a projected circle from the original cylinder....WHY!!!!! This is such a frustrating issue, it makes me not want to use this software.

This does not happen in any of the other CAD package I've used, and there needs to be a way to turn it off. 

[kb9ydn]

The over-reliance on projecting geometry has bothered me from the beginning.  But turning off that setting should make it stop auto-projecting (it does for me).  This might be a bug.

C|

[kb9ydn]

Yeah, I definitely think this setting is broken.  If I turn it on it does nothing, which is not right.

C|

[wilwyn]

I don't think this is necessarily a bug for the example you have used. In your scenario the projected circle is only added when you include the tangent constraint. This is logically required for the internal consistency of the sketch as the constraint must apply to geometry that is part of the sketch.  If you stop the second sketch before adding the constraint, the reference to the circle is not added.

The latest version includes two settings in Preferences relating to auto projecting geometry: "Auto project edges on reference" and "Auto project geometry on active sketch plane".  I have not fully explored the these two interact, but I do not seem to get a lot of extra projected artefacts in my sketches when I have them off.

[kb9ydn]

@wilwyn

The way you describe it I would agree is probably not a bug as far as the way Fusion is supposed to work.  But I would say it's unnecessary to show projected entities even when referenced.  My other other CAD program doesn't do this and I'm thankful for it.

As far as the two auto-project settings, they seem to be totally inactive for me, meaning they don't do anything.  Which I'm pretty sure is a bug.  Or there is something else going on that I haven't figured out yet.

C|

[beardytroll]

I agree with the comments above, the projection does not occur unless a constraint is added. And as far as I can tell the two selection options in preferences don't change much. I understand projecting references literally to the current sketch may be how fusion is currently designed, but this is not necessary with any other CAD system. The additional projected geometry is a problem because it clutters the sketches and makes it really difficult to keep things clean. I find it really frustrating, and CAD programs figured out how to handle projected references back in the early 2000's.

If from a programming perspective this is a requirement, then is it possible to have ALL the magenta reference geometry auto hide when the sketch is not active? 

[jeff_strater]

As near as I can tell, the Autoproject options are working as intended.  Perhaps some explanation is necessary:

• "Autoproject edges on reference".  This option has existed for a while.  This option controls whether you can infer relationships to edges which are not yet projected into the sketch.  It only works when you are looking straight down on the sketch "auto look at sketch", or if you manually view the sketch.  This option will project a referenced edge into the sketch.  But, I just verified:  With this option off, no auto-projection happens.
• "Auto project on active sketch plane".  This option is new.  It controls whether geometry from a face that you select for a new sketch.  Today, Fusion does not display that geometry in the magenta color, but you can still infer to it.  Fusion does show the profile of those geometries.  This, also, appears to be working correctly.  If it is turned off, and you create a new sketch on a planar face, no geometry in the sketch is created.

It is a valid request to not show any projected or auto-projected geometry in the sketch (or to have an option to turn it on and off, like with Profiles and Constraints).  Fusion could work that way.  However, that geometry will have to be in the sketch, whether it is drawn or not.  All CAD programs work this way - there is no way around it.  It has to participate in the solve.

[kb9ydn]

@jeff_strater

Ahha, that explains it.  Both options are working; I was just confused on what they are supposed to do.  (In my defense it's been a long time since I've thought about auto-project)  

Regarding auto project on reference; having this only work when your view is near to normal of the active sketch plane makes no sense to me.  If you're going to be referencing geometry outside of your sketch it's far easier to see what you're actually selecting if you view it from an angle outside of normal.  Why is there this limitation?

And for auto project on active sketch plane; this would be completely unneeded if auto project on reference worked for all geometry all the time.  What difference does it make if geometry is in the active sketch plane or not?  If you want to reference it, you want to reference it.  Project it in to the sketch and either show it or don't based on a setting.  I guess I'm just not really getting what the long term vision is for geometry referencing in sketching based on the currently available settings.

As far as projected geometries having to be in the sketch (in order to solve) regardless of whether they are shown or not; that makes perfect sense.

C|

[beardytroll]

@jeff_strater It makes sense that the references need to be included at the solve level of the sketch, but in every other CAD system I've used that is not a visible part to the UI. Assuming the references are included then they are hidden and the only sketch geometry shown are the features created by the user. All the magenta sketch lines, endpoints and profiles end up getting pretty messy, and It would be extremely helpful to have a setting to turn visibility of those features off. 

Now there are times that you do in fact want to have reference geometry projected into the sketch, and in this case you could use the project command. In SW this was called "convert" and this would project the selected line segment into the active sketch. But all other externally referenced sketch constraints would not add additional sketch geometry.

Also, when actually "converting" projecting reference features to the active sketch, they should be trim-able, which they currently are not. 

[jeff_strater]

@kb9ydn:  The reason why we limit autoprojecting edges to looking down on the sketch is this:

In this picture, the sketch plane is on the top plane, but the edge is actually offset vertically from that plane.  So, autoproject would result in a line that is different from the preview.  We thought that would be confusing, especially for people that are not that 3D aware...

[jeff_strater]

@beardytroll,

I agree that both of these (being able to hide the projected geometry, and the ability to trim projected geometry) are valid product requests.  I found this idea:  trim-projected-curve for the second.  I didn't find one for hiding projected geometry - this idea could evolve into that request, or feel free to add a new one.  My only point in commenting here was that, to the best of my knowledge, the existing options are working as I expect.

Thanks!

Jeff

[MetalDawg]

Please just let us turn off the magenta, and clean up our view.  I don't care what is happening in the background.  I just don't want to see it.

Thanks!

[Anonymous]

A box inside the sketch tool palette that will allow you to turn on/off projected geometry. It will make it easier to see your curves when things get too fussy!

[Scoox]

 +10000

Also check out this other idea: Selection filter: 1) Projected items, 2) Missing references