creating an aligned component to another compound angled component

[Anonymous]

This might be a curly one.... I am working on a chair brace located at the top of the chair. The 2 side frames of the chair are both inclined in toward the center slightly, as well as reclined toward the back. This creates a compound angle that the brace needs to align to. The brace consists of a curved back that is attached to 2 circular steel rods that fit down inside the tops of the frames. I need to make the brace such that at the points where it fits down inside the frames it must be aligned parallel to the axes of the frames on each side, as well as be perpendicular to the frames when viewed from the orthogonal side views (left and right)

I have constructed an arc and then extruded it, but it is incorrect. What it actually requires is a loft through 3 profiles. The 2 ends need to be aligned to the axes of the frames, while the middle profile needs to ensure it perpendicular orientation to the frames when viewed from the sides. 

I hope I have explained that ok.... Would love some help.

[davebYYPCU]

A Loft, yes, but top to bottom, not sideways, I think this is what you want, followed your sizes and settings 

Your intent and order of operations could do with some work,

(make half and mirror at the end, dependent on the end goal)

I

would also consider joining the internal rod to the brace, then cutting all that from the outer pipe, if I have actually figured what you wanted. (you don't need the drilled hole, and then make the "Cylinder" to fill it, Avoid primitives until you get more experience)

Check the time line, I have only fixed the brace, and deleted the internal rods, for clarity.....

Happy to answer the questions I generate.

Might help....

[Anonymous]

That makes more sense, thanks so much.

I am a little unclear on how you determined the sketch points for the lower arc of the loft. One thing I am finding hard to find in Fusion is locating the centers of objects (like this circular chair frame) to snap to in order to be able to create an accurate sketch. I have resorted to projecting the sketch to the sketch plane, but here I can only get the top and bottom profiles of the frame and not the section profile at the offset sketch plane where I need it. I have tried to recreate your arc but am not able to. Are you able to run through how you found the center like you did?... Sorry to have to ask.

Also, can you tell me why using primitives is not recommended here. I don't quite follow what you mean here about the cylinder:

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.....you don't need the drilled hole, and then make the "Cylinder" to fill it, Avoid primitives until you get more experience....

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[TrippyLighting]

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@Anonymous wrote:

Also, can you tell me why using primitives is not recommended here. I don't quite follow what you mean here about the cylinder:

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.....you don't need the drilled hole, and then make the "Cylinder" to fill it, Avoid primitives until you get more experience....

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The primitives in Fusion 360 are a relic from the early days of Fusion 360 when it was a pure direct modeling software. As such they are only semi parametric. For example if you snap a primitive to a sketch point, it will not remain attached to that point if you change the sketch. At least that's been my experience in the past.
This only applies to the primitives in Fusion 360. Other applications handle this differently.

[davebYYPCU]

Ok, I found that you made the brace curve, extruded down but the lower edge did not flare along the upright centre line, as was your original intent.

I made the offset plane the depth of the Extrude.  Your upright centre lines would pierce the sketch plane, so you use Project > Intersect, to place the end Point, (Purple Point).  Edit the height of the brace with the offset plane position and all will update.

At the time you made the brace, and editing that component one of the uprights had not been made yet, so I did half and mirror to get the other side.  The short tangent lines are construction, for accuracy.  In the second sketch that construction line is Projected.  The second sketch is a tangent curve to the outer purple end point.

Primatives, just to add to Peter’s comment, when you have more experience, you will not use them in elaborate models, anyway.

[Anonymous]

Great thanks for clarifying. Awesome 🙂

A couple of things have come to mind from your comments. Firstly, once the projected centerline point of the frame is on the sketch plane and used to create the bottom curve, does it stay along the centerline when the offset plane is extended downward? 

I also notice I am unable to adjust the top curve that is attached to the original plane. Is there a way to bring that down so the brace is below the top of the frame as in my original file?

The left frame was made using a centerline, but when I tried to mirror it about a midplane the sketch did not go with it. This makes it difficult to get a center point to draw the full curved sketch to. Is there a way to retain the sketch when copied/mirrored to allow making sketches to the copy snap to the centerline if its not there?

[davebYYPCU]

Last things first, I expected to see the centre line in both components, and at a loss to explain that, when it wasn't there I had the work around for a half / mirror to fall back on. @jeff_strater would be interested in that.

Does it stay along the centre line when the offset plane is extended downward?   Yes, edit feature and change the distance.

I also notice I am unable to adjust the top curve that is attached to the original plane. Is there a way to bring that down so the brace is below the top of the frame as in my original file?  Yes, sorry I missed that somehow.

Realign the first curve, and the second curve will simply update, 

Construct both sketches / curves with the Project > Intersect, and Project commands, and there is no need to extrude the top section.

Might help...

[chrisplyler]

I have not corrected the other stuff you did that is... not necessarily wrong but... not the best workflow. But I did remake the brace. I think, from the file you posted, that the incorrect bit is just the fact that your extrude didn't widen as it follows the side posts down? How about something like this?

[Anonymous]

Thankyou so much for taking the time to make the screen cast. 

Sorry for the confusion, the actual issue was that I was not able to align the ends of the brace to the centerline of the chairs frames (pipes) making it difficult to insert the brace with rods attached down inside the frames...

[jeff_strater]

@davebYYPCU , @Anonymous , I haven't taken the time to fully understand the problem in this thread, so I'm just addressing a fairly narrow question about mirror component:  "I expected to see the centre line in both components, and at a loss to explain that, when it wasn't there I had the work around for a half / mirror to fall back on. @jeff.strater would be interested in that."

This is, for better or worse, as expected.  Mirror component does not mirror sketch geometry.  The main reason for this is that Mirror component only mirrors the "output" of the component:  Primarily bodies, but also includes work planes, axes, etc.  Yeah, it arguable whether the work geometry items are inputs or outputs.  But, the real reason for not including sketches is a transform issue.  Fusion only supports right-handed coordinate systems.  If we supported a mirrored sketch, the result would be a left-handed coordinate system in the mirror instance.  This would require a significant amount of rework in the sketch environment.  However, use cases like this make an interesting case for trying to support this in the future.  This would require some kind of a non-editable sketch, since you would not want to allow a user to edit the mirrored sketch.

So, I won't say "never", but that's not how it works today.

[davebYYPCU]

Thanks, Jeff, I think I forgot the mirror - sketch syndrome, which was all that I intended you to check out, as soon as I read the response it made sense, but before, in a situation that I needed the sketch.  I almost went with the Circular pattern, but half mirror was first option.

[Anonymous]

If I may interject here, I can understand why Fusion (rightly or wrongly) does not allow the sketch to be copied. But I still do not understand why when drawing a sketch between the center of a component and a copy of that component, fusion does not allow you to automatically snap to the center of the created body when the originating sketch is not there.....thus making it super difficult to get where you need to go...... Mmmmmm.

This goes back to why Dave had to do a half sketch and mirror it to get to where he needed to get to. This is a workaround at best to an issue that requires fixing don't you think?

While I'm on the topic of half sketches, and the need to HAVE TO use them in this case, why is there not a symmetry axis function in the model environment to cover this, and every other requirement for half sketches for symmetric parts? A symmetry axis would simply, and automatically draw in the other half of the sketch for you so you can actually see the entire part, negating the need to perform a mirror at all.... Does that make sense?

If Fusion is 'right-handed', simply make it work for right hand sketches..... Perhaps I'm oversimplifying it, but it seems like a great evolution for Fusion as opposed to what it is currently, and for very little effort....

[TrippyLighting]

@Anonymous different workflows don't necessarily mean that there is something wrong that needs to be fixed.

These are just different workflows to look at a problem from a different perspective.

If @davebYYPCU's workflow solved the problem then that's fine. In the end that got the job done. So did @chrisplyler's screencast I believe. I can think of other workflows all resulting in the same end result.

[chrisplyler]

Fusion (rightly) doesn't include a component's sketch/es in its mirrored copy, because that mirrored copy must remain symmetrically inverse with the original. If the sketch/es were included, some dolt would try to change a dimension in the copy, and it would fail to be a mirror.

If you want to snap to one or more positions (center or otherwise) in one or more components while you're sketching for another component, use one of the Sketch>Project tools to capture that/those desired position/s from the geometry, not from a sketch.

[Anonymous]

Thanks again Chris for your time and patience to make another screencast for me 🙂 Some very helpful insights in there.

I was using the project to sketch tool early on, but the one I didn't look at was the sketch - intersect tool, that projects to the offset plane I was using... Silly me! Dave was gracious enough to set me right there.

My discussion about the having symmetry axes and planes for the model environment was concerning the workaround Dave had made use of to make the brace, and about not being able to see the whole part whilst constructing it, and then having to do a mirror function as well. 

For situations like this and many others, the ability to use symmetry axes and planes (in the model environment) saves a HUGE amount of time (projections/translations and mirroring) and makes adjustments to both sketches and bodies a pleasure. It is a progression in parametric modeling to be sure, and one I feel Fusion would benefit greatly from. The Scuplt environment uses it to some extent to edit T spline objects, but it definitely needs to be adopted into the Model environment too.

A diversion from the original post I know, my apologies, but it did come up as a result of a solution.

[chrisplyler]

Hmmmm. So...copy the sketch into the mirrored copy, keep them linked, and allow edits to either sketch, with those edits being propagated either direction?

Okay, I'll buy into that idea if you want it. I don't see any negative side effects. But I also don't see how it saves any time. If you can edit the mirror's sketch, you can just as quickly edit the original sketch.

Or...wait...maybe I'm starting to see your vision.... You want to edit the original half of the pair and see the changes in the mirror in real time? So that you can see the results of every change happen without waiting until you've finished editing?

Okay, I'll jump on board with that. Personally, I'm able envision the results in my mind's eye just fine, and so don't feel that I need such a thing, but it couldn't hurt.

Have I understood correctly?

[Anonymous]

Or...wait...maybe I'm starting to see your vision.... You want to edit the original half of the pair and see the changes in the mirror in real time? So that you can see the results of every change happen without waiting until you've finished editing?

Yes, that's the basic gist of it. When working with a symmetry axis or plane you would only draw half of the sketch and the  other half is generated for you. Any edits are done to the side you have drawn and as you say, are updated in real time.

So, if you are having to get projected sketches from both sides to make the new sketch, working with a symmetry axis negates that need to do that, and also for the need to mirror the sketch after it is complete. When working with curves, although I can visualize it also, the whole sketch can provide instant feedback that you might otherwise miss in a half sketch. You can of course turn the symmetry axis off if you need to, and add/subtract something to only one half when required.

In cases like this especially, when parts of the new sketch are curved and you want to apply constraints to link to the reference sketch to follow its axis when edited (because of the compound angle), the originating sketch is the ONLY place you can do that currently. A half sketch can take care of that (as a workaround) but then has to be mirrored. Dave had to adopt this method in his earlier posting when confronted with these issues.

A symmetry axis just makes the process easier and smoother. Editing is where its true time-saving potential comes in. If you have played around with the symmetry tool for editing T-spline objects in the sculpt environment you will know what I mean.

[TrippyLighting]

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@Anonymous wrote:

A symmetry axis just makes the process easier and smoother. Editing is where its true time-saving potential comes in. If you have played around with the symmetry tool for editing T-spline objects in the sculpt environment you will know what I mean.

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Unfortunately the sketch engines in most mainstream CAD software systems just don't work that way. In fact, mirroring and patterning in sketches is rarely a good idea. I most cases for overall performance reasons it is better to mirror geometry than sketch items.

[Anonymous]

That's very true. I have used it in SpaceClaim and it is fantastic, but then it is a direct modeler...

I noticed the use of symmetry axes/planes in the sculpt environment which works very well, so had hoped it could be easily adopted into the model environment as well. 

Jeff Stater mentioned earlier that it could be done in Fusion, but at the cost of significant re-work to the engine. Having used the function personally, I find going back to the traditional method slow and tedious. I thought Fusion users would benefit greatly from it.

[chrisplyler]

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@moovmedesign wrote:

I thought Fusion users would benefit greatly from it.

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Some might, I suppose. So I won't stand up and say it's a bad idea.

But for me personally, I can't imagine that real-time mirror edits would have any significant impact compared to updated-when-you-finish mirror edits.

Besides...isn't what I show in my Screencast video below effectively real-time edits anyway? At least, for dimensional changes. Doesn't work if you need to actually Edit the sketch to add or remove geometry, but it works for dimensional changes. It's something at least.