Hello.
The preferences menu under General -> Design contains two options. One is called “Auto project edges on reference” and the other one is called “Auto project geometry on active sketch planes”. Could someone explain to me the difference between the two options? Based on personal experimentation, it appears that they work as follows:
Auto project edges on reference: Every single bit of geometry that is projectable into the sketch will be accessible from the sketch. The accessible geometry goes beyond the "borders" of the sketch infinitely. When actually referencing the accessible geometry, the geometry is projected into the sketch using the magenta color.
Auto project geometry on active sketch planes: Only geometry that conforms to the object face boundaries that was used for creating the sketch is accessible. For example, if the sketch was created on top of a square face then the four sides of the square will be accessible and nothing more. If the sketch is created on a construction plane, then nothing is accessible because no face was used to create the sketch. When actually referencing the accessible geometry, the geometry is NOT projected into the sketch using the magenta color… but is there somewhere so I am not sure how you would delete the dependency to that projected geometry if you ever needed to do that.
Any help will be appreciated. Specially a link to the documentation (I am sure is there somewhere but I was not able to find it).
Thanks.
Hi @tcrxelizondo,
You are actually pretty close in your description here - you should write a tips-and-tutorials for this.
A couple of small points here:
Auto project edges on reference: Everything you say here is correct. There are a couple of additional small points:
- This only works if you are viewing the sketch straight on (if you have "Auto Look At Sketch" turned on, or have clicked on the "Look At" button in the sketch panel). This is to prevent creating accidental projections that you did not really want, while you are viewing at an angle
- This option is disabled if you have the "3D Sketch" option checked in the sketch panel. This is because the reference to model geometry is ambiguous - do you want to snap to it in 3D, or project it?
Auto project geometry on active sketch planes: Spot on here. We added this option recently, because having the extra geometry from the face can be a problem. It can slow down your sketch, especially if your face has a lot of geometry to it (for instance, a pattern of holes).
"When actually referencing the accessible geometry, the geometry is NOT projected into the sketch using the magenta color." Yes, you are correct. This was a first attempt to address the problem of geometry from the face being in your sketch. Fusion used to show these in the magenta color. But, some customers thought it was "too visually distracting", so we simply turned off the display of those geometries. They are still there, you can select them, dimension to them, etc, and when you do, Fusion will draw them in magenta.
"I am not sure how you would delete the dependency to that projected geometry if you ever needed to do that." Even though they are not drawn, they otherwise behave as any other sketch geometry. You can select and delete them. If you have a dependency to them (e.g. a dimension), deleting the dimension will break the dependency.
Hope this helps a bit.
Jeff
Hello.
The preferences menu under General -> Design contains two options. One is called “Auto project edges on reference” and the other one is called “Auto project geometry on active sketch planes”. Could someone explain to me the difference between the two options? Based on personal experimentation, it appears that they work as follows:
Auto project edges on reference: Every single bit of geometry that is projectable into the sketch will be accessible from the sketch. The accessible geometry goes beyond the "borders" of the sketch infinitely. When actually referencing the accessible geometry, the geometry is projected into the sketch using the magenta color.
Auto project geometry on active sketch planes: Only geometry that conforms to the object face boundaries that was used for creating the sketch is accessible. For example, if the sketch was created on top of a square face then the four sides of the square will be accessible and nothing more. If the sketch is created on a construction plane, then nothing is accessible because no face was used to create the sketch. When actually referencing the accessible geometry, the geometry is NOT projected into the sketch using the magenta color… but is there somewhere so I am not sure how you would delete the dependency to that projected geometry if you ever needed to do that.
Any help will be appreciated. Specially a link to the documentation (I am sure is there somewhere but I was not able to find it).
Thanks.
Hi @tcrxelizondo,
You are actually pretty close in your description here - you should write a tips-and-tutorials for this.
A couple of small points here:
Auto project edges on reference: Everything you say here is correct. There are a couple of additional small points:
- This only works if you are viewing the sketch straight on (if you have "Auto Look At Sketch" turned on, or have clicked on the "Look At" button in the sketch panel). This is to prevent creating accidental projections that you did not really want, while you are viewing at an angle
- This option is disabled if you have the "3D Sketch" option checked in the sketch panel. This is because the reference to model geometry is ambiguous - do you want to snap to it in 3D, or project it?
Auto project geometry on active sketch planes: Spot on here. We added this option recently, because having the extra geometry from the face can be a problem. It can slow down your sketch, especially if your face has a lot of geometry to it (for instance, a pattern of holes).
"When actually referencing the accessible geometry, the geometry is NOT projected into the sketch using the magenta color." Yes, you are correct. This was a first attempt to address the problem of geometry from the face being in your sketch. Fusion used to show these in the magenta color. But, some customers thought it was "too visually distracting", so we simply turned off the display of those geometries. They are still there, you can select them, dimension to them, etc, and when you do, Fusion will draw them in magenta.
"I am not sure how you would delete the dependency to that projected geometry if you ever needed to do that." Even though they are not drawn, they otherwise behave as any other sketch geometry. You can select and delete them. If you have a dependency to them (e.g. a dimension), deleting the dimension will break the dependency.
Hope this helps a bit.
Jeff
Hi
You never told, where this documentation can be found - if it can. If it can't, shouldn't there be a well defined reference documentation somewhere for Fusion 360?
@jeff.strater I´m sorry to bring this up again, but I stumbled over this issue when I tested an add-in I wrote.
Regarding the behavior of auto-projected geometry, you wrote
@jeff.strater wrote:
..............
"I am not sure how you would delete the dependency to that projected geometry if you ever needed to do that." Even though they are not drawn, they otherwise behave as any other sketch geometry.
.......
.......
Jeff
Well, they don´t behave as any other sketch geometry if you want to break the links of the invisible auto-projected geometry:
- even if you select an (invisible) element with click-and-hold and then right-click, there is no "Break Link" option in the dialog
image 1 - auto-projected sketch
image 2 - click-and-hold of invisible geometry
image 3 - right-click options for selected geometry -> no "Break Link"
So my questions are:
- is that behavior "as designed"?
- in my add-in I do break the links of these invisible linked sketch-geometry. Will this violate your "design-idea", and as result cause problems?
Thanks and happy holidays!
@Anonymous, yes, not being able to Break Link on the projected geometry from the face the sketch is placed on is "as designed". I'm not sure there is a great reason for this, but it is at least intentional. As to whether doing a Break Link via the API (where it might not be blocked) will cause any logic problems, I'm not 100% certain. Most likely, no, it won't cause any problems, if you can do that via the API. I can't think of any offhand. I know that you can delete that projected geometry. And, once a Break Link is done, there is no more memory that that geometry ever came from a projection, so I'm willing to bet nothing bad can happen from this.
Jeff
"regression"? How so? As far as I'm aware it has always worked this way - no Break Link on face geometry. If you think that you used to be able to do this, then yes, I'd agree.
You're probably right 
Can we redefine regression to mean 'this should be the way it works'?
Hi @jeff.strater - can you say where the full documentation of this is located?
... and aren't the names of the two options a little bit off - not really describing, what they do?
"Auto project edges on reference": Isn't it really: "Auto project on sketch" (since it is both bodies and sketches, edges, points, and surfaces that project and they all project to the active sketch and not to some "reference")?
"Auto project geometry on active sketch planes": Sounds more like what the first option does, but should maybe rather be: "Auto project sketch reference face to sketch"
Best
Hoegge
Furthermore, I'm still of the opinion that it should be possible to hide/show projected and non-projected geometries in sketches. Currently it is a mess.
@hoegge. Good questions. I did look a bit, and I could not really find a place where all of this is documented, unfortunately. It should be, I agree.
as to the names... Those names were the subject of a lot of intense debate among the design team. The challenge was to find a name that was both descriptive, but would still fit on the dialog. Here's a little explanation of what those names were intended to mean:
"Auto project edges on reference" - this one is relatively accurate. The "on reference" part was intended to show that this auto projection only happens when you "reference" (meaning click on) an edge (during curve or point creation). And the "edges" part here is actually accurate. This one does only auto-project model edges (it does not auto-project faces, bodies, other sketch geometry, etc). A more accurate name would be something like: "auto project edges on selection during geometry creation, when looking directly down the sketch normal", but you can see the problems with that... I have many opinions and commentary on this particular preference, but I'll hold those back for now.
"Auto project geometry on active sketch planes" - I agree that the "active sketch planes" part is not the best-worded bit. Your suggestion, IMO, is better. It really is whether the edges of a planar face that is selected for a sketch are automatically projected into the active sketch. Even the "projected" here is a bit misleading. There is no "projection" here. Or, rather, the projection is a null projection. But, that's a small point, I guess. Maybe: "include edges of selected face in a new sketch" would be fairly accurate. The whole thing about these curves being invisible is another whole topic...
Oh, one last thing: You'll be happy to hear that we are adding the ability to hide/show projected geometry in a sketch in an upcoming release. I will admit to mixed feelings on this, but the demand was fairly high, and it was not difficult, so it's going to go in.
hi @jeff.strater - that sounds great - but only if you can also hide/show other ("non-projected") geometries / sketch parts too. Otherwise there is still no way to easily see projected geometries to clean them up and break links. Is that included to and if not - could you make a push for it?
Best
hoegge
@jeff.strater - thanks for the explanation. I think then, what makes the first one confusing is that it is not obvious that "reference" is a verb and not a noun. So renaming to "Auto project edges on referencing" would probably help a lot.
This led me to think the project dialog could also be improved a bit then, since it meant that a sphere could not be projected, since it has no edges and I saw (never used it before), that you can select between "specfied entities" and bodies:
where bodies makes perfectly sense, whereas "specified entities" seems weird. Selected bodies are also specified entities. So maybe it should be "edges" and "bodies" instead?
@jeff.strater tried out a bit more and it seems like the "auto project geometry on active sketch plane" does only project the profile and not the edges of the profile, which seems a bit weird. Why would you do that? If the profile / face of a body has a hole inside extruded by another sketch, this hole is not subtracted from the face, but both are projected as profiles (assume a profile cannot have holes). You can select the edge of the profile by hovering over it but apparently not use it for anything (except snapping to it). I think it is a little weird this kind of "projection", or? What is the rational behind doing it like that and not projecting the edges? Is there a use case?
https://knowledge.autodesk.com/community/screencast/9bed5aec-1262-4877-8c7e-c064ab0756e9
BTW: Thanks for being very responsive. It is people like you who makes Fusion 360 a great program. Then let's hope the web / community development people catch up at some point
@hoegge wrote:
.....
.....Selected bodies are also specified entities. So maybe it should be "edges" and "bodies" instead?
mmhhhhh.... edges?.......you can also select (and project) vertices and faces and construction-geometry and even geometry from another sketch....
Those edges are really projected. They are just not explicitly drawn. This is a decision that was controversial, at best. The idea was that all that purple geometry would clutter up your sketch, so it's better not to draw it. But, the curves are definitely there - you can snap to them, constrain to them, dimension to them, everything but SEE them...
"mmhhhhh.... edges?.......you can also select (and project) vertices and faces and construction-geometry and even geometry from another sketch"
That is true for the Project command itself. But, this preference only applies to auto-projection, which is a related, but different mechanism. Auto-projection during curve creation only applies to model edges. Nothing else.
Yes - that is for sure a strange choice @jeff.strater - and pretty inconsistent. If we get the ability to hide/and show projected curves AND hide/show other curves (to see only projected), this would make even less sense.
Thanks
yes - you're right ("you can also select (and project) vertices and faces and construction-geometry and even geometry from another sketch").
Also understand it is different mechanism - but maybe not very "smart" to have a different projection mechanism, when it is "auto".
Well - now a least I understand it - wonder how many never finds out
Please: also hide/show non-projected - to be able to clean up in projected geometries
thanks
Hoegge