"Move Sketches to Component" tool to fix F360 component creation weakness

[mwoll]

I have been enjoying learning F360, but the way it handles activation of components is a major turn-off. New designers may not notice the problem right away; I come from a Solidworks background and do a lot od top-down design so the problem jumps right out at me.

F360 makes a big deal about how bodies can be changed to components at any time. This should be a big plus for top-down and concept design. But the resulting component winds up with sketches stuck in the top level of the model. The component cannot be used easily in other models. Even in the same assembly it may be hard to find the corresponding sketch for a component feature.

The way I can avoid this is to initially create a component and always activate it before doing any editing; this is shown in several tutorial videos. But it contradicts the more informal techniques shown in other tutorials. Also, if I even once forget to click the activate button while adding a feature to a component then I can no longer use "copy" to put it into another model, but only "copy new": the copy will be unlinked and missing at least one of its sketches.

Best solution:
Add a Move Sketches to Component tool. This turns any component into one that contains all of its own sketches. This approach works after-the-fact and so does not get in the way of early-stage creativity.

Notes:

1) I don't see a consistent name for a component that is "self contained" in the F360 docs. Ideas?

2) There are other possible solutions but this seems to be the easiest for the user. Maybe not for the programmers.

3) It would also be nice if a "self contained" component showed a special icon in the broswer for easy identification. Maybe add some lines to the regular component icon to indicate a contained sketch.

[mwoll]

Some more thought on my enhancement request...

1) What is really needed is not just to move all sketches to the component but to make the timeline of the component independent. This might be a messy programming problem but I don't really see how F360 can be  serious player without dealing with this weakness in its design.

2) Is there any reason why a component should ever not contain its own sketches? Maybe a simpler solution would be to make this automatic:

  a) When bodies are converted to a component also move all associated sketches into the component.

  b) When a new sketch is used to add a feature to a component, always move the sketch into the component.

3) If there is a specific reason to keep a sketch at the model level then a "copy sketch" tool, already requested by a couple of folks, would be handy. Make a sketch (stays in the model), copy the sketch (still in the model), and use the copied sketch to make a feature in a component (the copied sketch moves into the component while the original stays in the model). When copying a sketch there should be a dialog with a "link to original" checkbox. If linked then the geometry in the copy will have contraints to the original geometry (but no dimensions). If unlinked the copy will be identical to the original, including dimensions and external constraints.

[schneik-adsk]

Try this...

Create a new designs and create the sketches and features to model the part. Focus on one part for this test.

Now lets assume we decide we really wanted this to be an assembly and we want to create a few parts. 

All the sketches and features are at the root of the design we want them nested nicely under the first component....

Without rolling back, simply create a new component. You should see a component feature at the end of the timeline.

Now here is the trick. In the browser, Select the first sketch you created and drag and drop it onto the component in the browser. It will be below the bodies and sketch folder at the root.

Shazahm! All the sketches and bodies magically move into the component and you should see the create component feature in the timline now reordered to the beginning of the timeline!

So long as you are not creating features or sketches that span multiple components you should be able to retroactively restructure bodies and sketches into components and we will update the time line as needed. This is new functionality we added in the last few months so I am sure there are a few holes we need to patch but from the description of your issue it seems we might have a reasonable solution?

[mwoll]

Thanks for the reply.  I gave what you described a try and found that it works up to a point.

There are three issues:

1) It seems to be a bit flakey. I had to try it several times to get it to work correctly. Depending on the order of operations some additional sketches can get pulled into a component. These are sketches used to create bodies that wind up in other components.

2) If I follow the instructions in your note exactly I would pull the very first sketch into the component. But this has the effect of pulling all sketches and all bodies into the component. To make it work with multiple bodies (each one becoming a component) I had to work backwards. I looked from the end of the sketch list to find that last sketch that had created a new body. Then I dragged that sketch into the empty component. Then I repeated this for the remaining sketches in the list. This is tedious and error prone.

3) Given that issues 1 and 2 can be fixed, there is still the problem that this is a messy manual solution. I have to search for the correct sketches to go with the bodies, but this is something the program could do more easily. (Presumably) there are two-way links in the database between bodies and sketches. So if I select a body and make it into a component (or drag a body into a component) the program should be able to find the associated sketches and bring them in to the component automatically. This would be much faster and more consistent.

As I said a previous comment, it almost always is better to keep sketches with components, so why not make this automatic? Or at least semi-automatic. Let the software move sketches into components whenever a feature is added to the component (whether they are activated of not).
Another problem is sketches that are referenced by more than one object. Of course the better workflow in this case is for the user to create assembly level sketches and then make copies of these for use in individual features. This avoids messy dependencies. It would help here if F360 had a "copy sketch" tool that had an option to make either a complete copy or a dependent copy. (I'll write up a new suggestion about this.)
If the user has created multiple references to a sketch then it might be possible for the software to automatically make a copy of the sketch to put into the component, but this is probably trickier to implement.

Conclusion: I appreciate your solution but will not "accept as solution" at this time because it seems still buggy and because a more automatic approach would be much more user-friendly.

[mwoll]

(also posted to forum) Thanks for the reply. I gave what you described a try and found that it works up to a point. There are three issues: 1) It seems to be a bit flakey. I had to try it several times to get it to work correctly. Depending on the order of operations some additional sketches can get pulled into a component. These are sketches used to create bodies that wind up in other components. 2) If I follow the instructions in your note exactly I would pull the very first sketch into the component. But this has the effect of pulling *all* sketches and *all* bodies into the component. To make it work with multiple bodies (each one becoming a component) I had to work backwards. I looked from the end of the sketch list to find that last sketch that had created a new body. Then I dragged that sketch into the empty component. Then I repeated this for the remaining sketches in the list. This is tedious and error prone. 3) Given that issues 1 and 2 can be fixed, there is still the problem that this is a messy manual solution. I have to search for the correct sketches to go with the bodies, but this is something the program could do more easily. (Presumably) there are two-way links in the database between bodies and sketches. So if I select a body and make it into a component (or drag a body into a component) the program should be able to find the associated sketches and bring them in to the component automatically. This would be much faster and more consistent. As I said a previous comment, it almost always is better to keep sketches with components, so why not make this automatic? Or at least semi-automatic. Let the software move sketches into components whenever a feature is added to the component (whether they are activated of not). Another problem is sketches that are referenced by more than one object. Of course the better workflow in this case is for the user to create assembly level sketches and then make copies of these for use in individual features. This avoids messy dependencies. It would help here if F360 had a "copy sketch" tool that had an option to make either a complete copy or a dependent copy. (I'll write up a new suggestion about this.) If the user has created multiple references to a sketch then it might be possible for the software to automatically make a copy of the sketch to put into the component, but this is probably trickier to implement. Conclusion: I appreciate your solution but will not "accept as solution" at this time because it seems still buggy and because a more automatic approach would be much more user-friendly. Michael Wollowitz

[promm]

@mwoll,

Based on the reasons that Kevin gave, this idea is being changed to solution provided.  There are three things to take away workflow wise.

1. You can drag and drop a sketch into a component or from one component to another.

2. If you drag and drop right after a sketch is created, we do not add it to the timeline.  This is a new enhancement that helps customers who forgot to activate a component first.

3. Create a component, we now activate it so that a sketch should be put into the component.  This also was done to help customers who forget to activate components.

Thank you,

Mike Prom

[sgraves]

I object to this "solution".  I have an assembly that I failed to properly activate the components.  Now I have a bunch of sketches at the root.  I am trying to move the sketches to their proper component.  I have not been able to move a single sketch.  Every single sketch gives me a "Warning: Detect some position features may result downstream features fail after restructure."  This can't be a solution if it doesn't work.

[sgraves]

After a little more thinking about this, here is my 2 cents.  I would like a way to leverage work I have already done.  It could be because I screwed up or because the design goals changed, I got educated, any number of reasons.  Ideally each component has a "recipe" to create it.  There are several ways the recipe is captured and presented to us.  The tricky thing is when we are creating an assembly, we are creating dependencies between components that may not be obvious.  I know it may not be possible to create a standalone recipe for a given component, but I should be the one to decide how to handle those inter-dependencies.  In other cases, when I make a change that impacts something down the line, Fusion 360 allows me to make the change and flags the areas in error.  I can go and fix the problems.  That may mean restructuring things, etc.

I would like the same functionality here.  Let us assume I have the design I want in the giant recipe that is the assembly.  In the assembly timeline, I should be able to change which component gets that step of the recipe.  If that breaks something down the line then so be it.  I should have the opportunity to go and fix that problem.  The program should not say, "I will not let you do this because it will break something"  I, the human, am very likely to see why it broke and how I can structure it to not break.

I do not have the intimate relationship with Fusion 360 that I have with other programs.  I suspect I am missing some nuances, for example Fusion 360 may have to organize things at the assembly level when there are inter-dependencies.  I hope I have conveyed what I want.  It would be great if it is already there and it is my lack of education that is the problem.  If so, please educate me.

Thanks,

Steve

[TrippyLighting]

@sgraves

Yes, you are missing a nuance 😉

It's called Fusion 360's R.U.L.E #1

As you are coming for Solid Works, be aware that when you select a face, edge or vertex of an object, and use the move tool, you are actually moving the body within the component, not the component. To move a component you can just drag it or if you want to use the move tool, you need to double-click on the object. The highlighting in the viewport will be different as well as the highlighting in the browser

[sgraves]

@TrippyLighting

Thank you for the response.

Yes, I understand Rule #1, but I have to retrain myself.  Can't I fix the problem when I forget to activate the proper component without redoing all the work I have done in the wrong context.  It seems to me that one should be able to move the sketches and timeline operations to the proper component.  I have been unable to do that.  I haven't even been able to copy and paste a sketch from one sketch into a new sketch.  It is very frustrating to realize that at any time I could be painting myself into a corner.  It is making me paranoid!

At a minimum I would like to copy or move a sketch.  I must be doing something wrong!  It has to be possible.  I can't imagine a system where a sketch can't be replicated in another place.

Thanks,

Steve

[etfrench]

I agree.  The inability to copy a sketch in timeline mode is one of several reasons why I prefer direct modeling mode.

[daniel_lyall]

@etfrench you can copy and paste in time line mode, there is a way to do it that works I will post a screen cast soon

[daniel_lyall]

@etfrench @sgraves Here you go

[etfrench]

@daniel_lyall It looks like you're just using the line tool to create a sketch on the face of an extruded component/body.  Is there a difference between using the line tool and just selecting the face and creating the sketch?  In any case this seems to only pick up the extruded features in the sketch.  Construction lines and other non-extruded items don't exist on the new sketch.

It's puzzling why there isn't a Copy Sketch command.  The new sketch doesn't need any references (nor should it have) to previously extruded features from the original sketch.

[daniel_lyall]

I am use the line tool to start the sketch that's all I could of used any sketch element to start the sketch, Each coped Sketch is a new sketch.

Its Sketch those 3 squires, extrude, make 3 components drag the first sketch into the first component after activating it,

Open the first sketch again select all stop the sketch

Activate component 2, start a sketch by selecting the line tool draw a sort line anywhere

Stop the line tool put the cursea on the line right click and select paste, ok the position then stop sketch and extrude. rinse and repeat in component  3 useing the sketch from component 2

The sketch when you first paste it, it just goes to where it was started from in X, Y and Z  on the faces that was selected. ( there is a if with this)

It could of been a construction plane offset from the new components origin, it just pastes the same as if you selected a faces.

The IF

If it's a offset plane from a faces it does not goto the same X, Y and Z as the original sketch it goes to the center of the original faces on it's construction plane the off set was done from. (Don't do it this way)

But you can move it to where you wont it to be, once it's where you wont it to be you ok the move tool, then do what you like with the sketch.

Each copy I did is from the sketch before, Its a all new sketch with it's own parameters. 

[TrippyLighting]

@etfrench

I direct modeling mode you can copy a sketch from one component to another by simply dragging the sketch from one component to the other while holding the ctrl key (CMD key on mac).

I timeline mode that does not work, however, sketches or to be more precise, the contents of a sketch can be copied in in timeline mode from one sketch to another.

So while you cannot drag a sketch from one component in the browser into another, there is a way to copy a sketch even in timeline mode.

@sgraves

Under certain circumstances a sketch can be moved into a component.

If for example you forgot to create a component in the first place and the the sketch and body show up in the top level folders for sketches and bodies you can still create a new component and drag the sketch for the top level folder into that component and that will pull the body that was created with this sketch with it into that component. If you are too far down the road, then, yes, you'l have some re-work to do. For example if you've gone so far as to creating joints between components than dragging sketch in not possible anymore.

Also, when reorganizing components, for example you have created several components already and then decide that these should better be in an assembly you can simply drag these components into that new assembly. The most common error when users report that this does not work is that they don't have the timeline marker rolled all the way to the end.

[sgraves]

@daniel_lyall(and @TrippyLighting)

Thank you both for your help.  Thanks to you, I am making great progress toward resolving my concerns.

Daniel,

Thank you for the animation.  Turns out ctl-C does not copy the sketch.  In your animation you used the right mouse click and that worked for me.  In fact, the ctl-C next to the right mouse click in the context menu was grayed out (go figure).   So now I can transfer the basic geometry in my sketches to a new sketch created in the proper component.  I can also move a blank sketch.  I have really screwed up my project (really my first doing it all in one assembly), previously I was making individual parts and making an assembly like I would in Inventor.  It is a gear train and is certainly easier (if done right) as an assembly.  I still can't move sketches that break the structure some how, but copying sketches gets me most of what I want since they have the majority of my work.

Thanks,

Steve

[daniel_lyall]

Anytime You want to know how to do something just ask, This is the Fusion Advanced Help area They called this forum that, Its also a professional forum as well, so no rude Aholes trolls or anything like that.

What helps to get a good reply is a screencast, a copy of what you are working on, and a well written what you would like to do.