Probably is mostly useless. Maybe there are still some cases of needing to share a sketch that Inventor does not do automatically? I can't think of any off the top of my head, but maybe there are some, and it was deliberately left in for those.
Still have trouble seeing what's so confusing about it though. Two processes that have the same result - It doesn't matter at all which you use, so you can just ignore whichever one isn't your preference. Personally, I forgot that it even did the automatic sharing until this question reminded me, because I was used to prior versions.
It's confusing because when new users (like me) see two options they assume there is a difference, and try to understand it, spending time testing, exploring the documentation, and asking in the forums.
It's bad also because the user interface should be as clean as possible, and show you only the useful items.
Smaller programs (like Wordpad) have just a few buttons, and they keep them always visible.
Larger programs (like Word) have many more buttons, and they show only the ones useful in the current context.
Inventor does a good job (better than Word) with the ribbon: when you work on a part, you don't see the projected drawing view button, and while editing a feature, you don't see the sketch constraint buttons.
I guess this it just a little error on an otherwise very good interface.
I guess I can see that. My suggestion to a new user would be to continue to assume that there is a difference until you find out otherwise, but to be aware that sometimes there isn't one.
Again referring back to my example of constraints, it's possible to turn off the constraint persistence and inference, and manually add all of the constraints yourself. That could be looked at as two options as well. You'll probably find a lot of cases like that as you learn more about the software.
Sometimes there's a legitimate reason why you still need access to both techniques. Sometimes it's just a legacy from some older workflow that hasn't totally been eliminated yet. Try not to worry too much about it if two things seem equivalent, because sometimes they are.
And when two ways to do the same thing like this have you frustrated, just be thankful you're not using AutoCAD, where there are 10+ ways to do almost everything. . . .
There is a difference between manually adding all the constraints to a sketch and getting them automatically inferred. In one case you have more control of the situation, in the other you need less clicks to get the same result.
There is no difference between making a sketch shared or visible. The same number of clicks to get the same result.
If you think as a user perhaps it doesn't bother you much.
But try to think as the guy who makes the decision about what to put in the interface: you would never decide to put duplicated items like "circle" and "round shape", or "extrude" and "sweep", because the result would be a crowded and unusable interface. One button for "circle" and one button for "extrude" do the same job.
My opinion about the Inventor interface is very positive. But the fact that the quality of the rest of the interface is very good doesn't make this error any less an error (again, unless there is a meaningful difference that I don't know.)
Maybe this is the root of the confusion - Visible and Shared do NOT mean the same thing. Visible does exactly what it sounds like - it puts the sketch back on the screen. It does not necesarily allow you to reuse the sketch. Shared allows you to reuse the sketch, but does not necessarily mean it is visible. These are two seperate attributes of the sketch.
When you attempt to perform a second extrude using the sketch(which must already be visible to allow you to select it), it is automatically setting it to a Shared status. It is simply bypassing the step of manually setting it as Shared (which was necessary in prior versions). That's the reason I used auto/manual constraints as a comparison - it is automatically adjusting a setting which can also be changed manually. It is that automatic change to Shared status that allowed you to reuse it - NOT the fact that it was Visible.
Even though you aren't having to set it that way yourself, that sketch is becoming Shared. Try this - make a sketch with two profiles. Extrude one. Then turn visibiity back on for the sketch, and extrude the second.
Note that the sketch now appears as an item on its own in the browser, as well as being listed under the extrusions. This only occurs for sketches that are considered Shared.
Now delete the second extrusion. Then, right-click the sketch, and note that there is an "Unshare" option. This only appears on Shared sketches as well, since you can't Unshare something that was never Shared.
Hopefully that makes things a little clearer. The button for Sharing the sketch may be somewhat obsolete, since the sketch now sets itself to Shared when you try to reuse it. But the concepts of "Visible" and "Shared" do have distinct meanings that are independant of each other, and are both still necessary.
Visible does what it sounds like. That's clear.
What does Shared do, other than making a sketch visible and reusable, which is exactly what Visible does?
And what does Unshare do, other than... nothing?
You can set a sketch Shared and not Visible, but... why?
You can delete the second extrusion and decide whether unshare or not a sketch, but... why?
Is there a reason to unshare that sketch, after deleting that second extrusion? Or not to?
As a beginner (beginner with Inventor, I have been working with other 3D tools for 25 years) I understand why I should make the sketch visible in order to reuse it, in fact that's what I do, and it works.
Then I find the shared option, and... I can't figure out what is for.
It's a relic of a previous life, and it should be removed.
Again, Visible is not making the sketch reusable. An implied, automatic "Shared" setting is making it reusable.
Unshare removes the ability to reuse the sketch (admittedly, this now does very little since reactivating the Shared status is automatic). It also removes the seperate browser item for the sketch, as this only exists for Shared (or unused) sketches.
Setting the sketch Shared and not Visible is very common. When you're done working on the sketch, you don't want it cluttering up the view anymore, so you turn the visibility off. That doesn't change the fact that it's shared. Similarly, setting a sketch to Visible but not Shared is also common - you may need to be able to see it for reference, but have no intention of actually reusing the sketch.
The reason to unshare the sketch after deleting the second extrusion would be to clear that sketch entity from the browser, since it is no longer needed. It's a cleanup function more than anything else - not doing so won't harm your model, it just leaves an unneeded item in the browser. Also, I think there are a few functions (though I can't think of what they are at the moment) that won't accept a shared sketch, so you would need to Unshare it to use one of those features.
My point was that Visibilty is not what is replacing Share, and you should not equate the two. Automatic application of Share is replacing a manual one. Share and Unshare was previously more important of a concept than it is now, but the automatic behavior doesn't quite cover everything yet (like unsharing something that no longer needs to be shared). Until it does, the options for it will still be needed for special cases that you haven't run into yet (and probably some I haven't seen either).
they are not the same...
I don't understand what is different following the original OP's two workflows.
The question was not about the difference between shared sketch and visible sketch.
stop trying to pick fights...i dont care that you insist on trying to degrade my posts...give it up already...help or dont help its your choice
i will give you some comprehension assistance as you obviously are struggeling to understand
i replied to stefans comment:
"I understand, they just decided to put two items on the context menu just to confuse the user and clutter the interface."
I replied as he is mistaken in thinking that they are the same and therefore redundant
both options ARE required at different times independantly of each other therefore they are not redundant and are not there to 'confuse users' and imho they do not clutter the interface
This is a rather academic discussion but I wanted to jump in nevertheless.
Removing the share context menu might give us a cleaner user interface but would you also then like us to remove the drag and drop capability (you can now create a shared sketch by dragging it in the browser above the feature it is initially consumed by). Some users like to use the context menu, others like the drag and drop and yet others like to have an automatic sharing capability. We satisfy the 3 tastes today.We are walking a fine line of not scaring new users with complexity while at the same time not taking away too much functionality that "older" users have gotten used to over the years.
Besides I wanted to give another example where "visibility" and "sharing" are decoupled.
You an create a loft to an invisible but shared sketch. So in that case the share command has still a reason of existence and you don't HAVE to use the visibility flag on the sketch if you want to consume that sketch by more than one feature.
I finally see one difference between a shared sketch and one not shared: a consumed sketch is visible in the browser only under the consuming feature if not shared, it is visible as a root for a new branch if shared.
That would justify two items "visible in graphics" and "visible in browser".
Giving two ways to perform the same action is good (drag and menu item), but it's bad when they are duplicated (two menu items whose only difference is a text).
Bob, I don't understand your second point when you say you don't have to use the visibility.
If the sketch is visible you can reuse it. No need to share it.
If the sketch is not visible you need to make it visible in order to reuse it, sharing it would make no difference.
Am I missing something?
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