Sketch cannot be edited

[kb9ydn]

In the attached part, when I try to edit sketch1, there is no "edit sketch" menu item for it when I try to right click from the browser tree.  I can create a new sketch and edit that one, but not sketch1.

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[innovatenate]

Are you importing a file?

Look in the timeline for a Base Feature. Try to edit the Base Feature first, then try to edit the sketch. 

I believe this forum thread may help.

http://forums.autodesk.com/t5/sketching-sculpting-modeling-and/trouble-editing-a-sketch/td-p/5394455

Hope that helps! 

Thanks,

[jeff_strater · Accepted solution]

This design has a couple of Base Features in it.  This particular sketch is actually owned by the second Base Feature, and so can only be edited if you first edit that Base Feature:

Then, you can edit this sketch:

I completely agree that this is very confusing, and not obvious.  We need to find a better way to distinguish these Base Feature sketches from normal parametric sketches...

Thanks!

Jeff Strater (Fusion development)

[kb9ydn]

Ok, I actually read that thread first but I'm still sort of confused about the base feature concept.  The way I understand things, is that there is a global workspace that is essentially the top level universe, which can have sketches and bodies in it as well as components.  Then each component has it's own self contained workspace, with other sketches, bodies, and components.  So if you want to edit something in a component, that component needs to active.  And then to edit a sketch or body in the global space, the root needs to be active.

By looking at the tree sketch1 appears to be in the global space, yet it's not?  You say that the sketch is owned by the second base feature, but if I edit the first base feature I can also edit sketch1.  And whatever I put in there is also visible when I try to edit sketch1 from the second base feature.  So where is it?

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[jeff_strater]

No argument with that.  You are correct, the Active Component and Base Feature concepts, as they are today, can be confusing.  I can try to explain some of it.

First, you are almost right with the "active component" concept.  When a component is active, any new objects (like sketches, or work geometry, or new components) will be owned by the active component.  So, for creation, yes, you have to activate the component to get a new sketch created underneath that component in the browser.  However, you do not need to activate the component in order to edit those objects.  Active Component is really only needed for creation.

However, Base Feature is another creature.  You can think of Base Feature as an island of Direct Modeling inside a parametric design.  When you create a Base Feature, you are put into a mode that is much like a Direct Modeling document - no history is captured in the timeline.  Things that you create while in that mode are also Direct Modeling analogs of the parametric features that live outside of that mode.  So, sketches and work geometry created while in Base Feature mode are owned by that Base Feature.  In that regard, Base Feature is like Active Component, you are correct.  The difference is that the sketches and work geometry owned by a Base Feature are not directly editable, unless you are editing the Base Feature itself.  And yes, you are right, the type and ownership of direct modeling sketches is not obvious from the browser - the icons look the same, and there is not a browser entry for the Base Feature, so there is no way to know that it is owned by a Base Feature.

Even typing that out, I admit, it is hard to justify the way it works.  In the original design, we struggled a lot with how to present this island of direct modeling in the UI.  We clearly have work to do in that area.  But, hopefully you can at least figure out how to use it.

Thanks for the input.  It does help, and we do take it seriously

Jeff

[kb9ydn]

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@jeff_strater wrote:

No argument with that.  You are correct, the Active Component and Base Feature concepts, as they are today, can be confusing.  I can try to explain some of it.

First, you are almost right with the "active component" concept.  When a component is active, any new objects (like sketches, or work geometry, or new components) will be owned by the active component.  So, for creation, yes, you have to activate the component to get a new sketch created underneath that component in the browser.  However, you do not need to activate the component in order to edit those objects.  Active Component is really only needed for creation.

Right.  So when you edit a sketch in a component, it will automatically activate that component if it's not already.  And then when the edit is finished, the activation returns to wherever it was before.  That makes perfect sense.

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@jeff_strater wrote:

However, Base Feature is another creature.  You can think of Base Feature as an island of Direct Modeling inside a parametric design.  When you create a Base Feature, you are put into a mode that is much like a Direct Modeling document - no history is captured in the timeline.  Things that you create while in that mode are also Direct Modeling analogs of the parametric features that live outside of that mode.  So, sketches and work geometry created while in Base Feature mode are owned by that Base Feature.  In that regard, Base Feature is like Active Component, you are correct.  The difference is that the sketches and work geometry owned by a Base Feature are not directly editable, unless you are editing the Base Feature itself.  And yes, you are right, the type and ownership of direct modeling sketches is not obvious from the browser - the icons look the same, and there is not a browser entry for the Base Feature, so there is no way to know that it is owned by a Base Feature.

Even typing that out, I admit, it is hard to justify the way it works.  In the original design, we struggled a lot with how to present this island of direct modeling in the UI.  We clearly have work to do in that area.  But, hopefully you can at least figure out how to use it.

I think I get it now.  And I see now how it ended up like it did.  I keep forgetting that imported files always start out with the design history turned off, so I didn't turn it on until after that sketch was created.  So the sketch ended up in a base feature by default.  (I think I even submitted an enhancement request for having design history enabled by default for imported models)

So from my limited experience so far, it seems like this "island of direct modelling" exists independently of component activation?  (Like an editing mode as you say)  What I mean by that is, when you're in this direct editing mode, are all base features available for editing (from any component), or just items within a particular base feature or component?

Coming from Solidworks, the idea of direct editing (without a history) is honestly quite foreign.  And mixing that with parametric modelling I would imagine is a major challenge.  I guess what I would say in terms of making it easier to understand, is that the browser tree needs to show base feature objects, and any entities that exist within that base feature need to be shown as such (leaves on the base feature branch).  Parametric features should have their own tree entry also (branch), with the items as leaves.  I know this could make the tree rather complicated but I think it would be less confusing than what it is now.

Anyway, I appreciate you taking the time to help me understand this.  I don't think I'll be switching over from Solidworks any time soon, but I do need to understand Fusion well enough that I can use it for machining fairly efficiently.

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[jeff_strater]

Yes, much of what you say I agree with.  The "islands of Direct Modeling" is a bit of a challenge to figure out, and is not very discoverable.  We were trying to find a way to mix direct and parametric.  I'm not sure we have settled on the right answer...  I like your suggestion of having some kind of Base Feature representation in the browser.

Having design history for imported designs would be nice, but right now we are not able to read design history from, say, Solidworks, so we are left with just the "dumb" solids.  Now, most of the time, this particular problem won't exist, because users won't create sketches inside the Base Feature geometry.  But, it's not that difficult to forget that you are editing a base feature, and accidentally put one in the base feature.  We've talked about making all sketches parametric, and available outside the base feature, but it gets a bit tricky to specify how that will work.  We'll keep thinking about that, though.

Thanks for trying out Fusion.  Maybe we'll convince you to switch over some day.

Jeff

[kb9ydn]

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@jeff_strater wrote:

Yes, much of what you say I agree with.  The "islands of Direct Modeling" is a bit of a challenge to figure out, and is not very discoverable.  We were trying to find a way to mix direct and parametric.  I'm not sure we have settled on the right answer...  I like your suggestion of having some kind of Base Feature representation in the browser.

I was thinking about this a little more yesterday.  Since it it more of an editing mode (direct vs parametric), maybe in addition to having direct edit features represented in the tree, you could also alter the user interface in some way to indicate what mode you are in.  For example, when in direct mode, have all direct modelling features highlighted in the tree, and all parametric features translucent, or something like that.  This way the features that are editable are made more obvious, and the ones that are not are left in the background.  Or you could use colors too, although that could have issues in terms of accessiblility.  Anyway, I think some sort of significant change in the interface would help to reinforce the separation between direct and parametric modelling.

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@jeff_strater wrote:

Having design history for imported designs would be nice, but right now we are not able to read design history from, say, Solidworks, so we are left with just the "dumb" solids.  Now, most of the time, this particular problem won't exist, because users won't create sketches inside the Base Feature geometry.  But, it's not that difficult to forget that you are editing a base feature, and accidentally put one in the base feature.  We've talked about making all sketches parametric, and available outside the base feature, but it gets a bit tricky to specify how that will work.  We'll keep thinking about that, though.

Thanks for trying out Fusion.  Maybe we'll convince you to switch over some day.

Jeff

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Actually I wasn't thinking about reading the existing history from imported parts at all. (That woud be awesome indeed, but likely not practical)  What I meant was simply having design history capture enabled by default for imported parts.  There is a setting in the preferences to enable design history capture all the time, but it doesn't work for imported parts.  You have to manually enable it for each imported file.  The default units also don't work for imported parts either.  They always default to metric.

I can see how fusion could someday be a SW killer.  But I think it has a ways to go in terms of general usability and smoothness of workflow.  SW has been around a LONG time and they've done a pretty good job streamlining it.  Like any large and complicated software, it has it's warts and a significant learning curve.  But once you learn the basics it's very easy to use and it doesn't get in your way.  In contrast, I learned Mastercam at the same time with Solidworks (about 5-6 years ago), and I absolutely hated MC.  It's a very powerful program and has a ton of features, but the interface is (or was back then) a complete disaster.  In some cases it looked like parts of it were created by two completely different teams that never talked to each other.  I felt like I was constantly fighting with it to make it work.  So when HSMXpress for SW came out I was SO happy!  The ease of use and integration with SW is exactly what it should be (and it's free!).  And now that Fusion has HSMWorks for cam (at a ridicuously low price) I have very high hopes for it.  Throw in some basic simulation capability and it will be unbeatable for entry to mid-level CAD/CAM.

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