Fusion turns solids itself into non solid but stitched

[cekuhnen]

If u use a revolve surface tool you end up not with a solid

even when it is a solid.

clicking the part and hitting stich again turns it finally into a solid i the browser.

[AndrewSears]

Claas,

The revolve from the patch environment will not create a solid body.  It will create a closed volume with zero mass.

Section view will expose this to you.

Andy 

[cekuhnen]

That does not really make any sense.

In no other application I use would this happen to stich a water tight shell and not making it a solid directly.

Why does it not directly create a solid and not just a closed object?

[jakefowler]

Hi Claas,

Fusion 360, like many BRep modelling packages, has a clear distinction between solid and surface bodies, and this affects the tools that can be applied to those bodies (from my understanding this is one of the core differences between BRep and NURBS modelling: BRep kernels generally set their key assumptions based on whether a body is a closed solid or not). Given this, we allow users to create ‘closed surfaces’ as a convenience. There may be cases where you wish to use a surface modelling feature (e.g. Trim) on an enclosed shape (e.g. a sphere).  If enclosed surfaces were automatically converted to solids, this would inhibit this ability.

Are you encountering scenarios in which this is causing problems/confusion? Or do you feel this seperation of solids & surfaces is fundamentally flawed? I’m not sure I see major problems with this paradigm, but having ‘grown up’ with BRep tools my point of view might be a bit one-sided.

Thanks!

Jake

[AbdnAllHope]

All solid modeling programs offer a distinction between surface and solid. The ability to have a closed surface body that is not automatically a solid is a benefit. I have had a lot of occasions where I had to combine disparate bodies that came through from another app. Sometimes its easier to fill the open surfaces and make them solids to merge everything, and sometimes you want closed bodies to be surfaces so you can trim them that way instead.

I think the most important thing to consider is that a surface body has no mass and therefore no physical properties assigned to it.

Phil

edit. I must have been typing this for a long time. Looks like Jake beat me to it.

[cekuhnen]

Jake and Phil,

I come from Rhino Alias Cobalt approach of surface modeling where you can stich/join surfaces

to generate logical water tight volumes.

I assume based on your comparision of BREP and NURBS kernels there is a difference between

sticthing surfaces in Fusion together compared to joining surfaces in Rhino.

Essenciatlly in Rhino you can make a blend surface between two surfaces. When you have a poly surface

you can use the solid edge rounding tool and apply it onto multiple edges.

In Fusion you also have to stitch at least 2 surfaces so you can use the edge fillet command.

But it seems to be more the way like Rhinos Solid edge rounding because it is the same command

that you also have in solid mode, and it can work on more than one edge at once:

Essenctially when you stitch a water tight form in Fusion it presents it to you with the solid icon.

and you can in solid mode continue working on it with the tools present there.

Obviously in DM when you stitch a water tight shell Fusion bakes / removes the DM patch features:

open surfaces

Caped and stitched into a solid:

Unstiched / exploded solid into a polysurface:

For me as a designer the main difference between solid and surface is how trimming splitting will work.

When I work on surfaces I trim a surface, if I work with a solid I work with volumes.

This workflow is pretty much the same like in Fusion with Patch Trim and Solid Combine:

And exploded back into single surfaces

So I see lots of simularity between Rhino/Alias and Fusion when we deal with surface and solids.

This all makes sense and allows surface designers get comfortable with Fusion quickly, specifically

when they are Rhino users. The only problem is the drastic lack of tools in Fusion patch like a untrim command.

This makes the work in Fusion a one way street when in patch mode.

Anyway my main complaint however what started this thread was the when I create a revolve tool

and it is stiched, it is water tight, and Fusion with only show it as a solid when I hit stitch after revolve.

The problem with this is that Fusion uses the Solid icon to tell you if your shell is water tight.

If it is not water tight you see the open surface/patch icon in the browser.

That is problematic as this can lead to confusion.

I as a user really should not be forced to hit stitch again. The edge rounding tools in Patch are borrowed from solid mode

at least the icons are the same.

So maybe what might be a good idea is when doing a revolve give the user than an option to create a true solid

and not a closed shell.

If you think about the logic of the steps and not what a solid or surface modeler are just used to, I hope you will see the

problem here.

[AbdnAllHope]

A solid in rhino is a solid in name only.  When you make something solid in Rhino it is really just water tight.  There are times in the course of making a complex model that you might want or need a surface that happens to be closed to remain a surface and not automatically go solid.  Especially in a case when the surface is proprietary to an interm stage of the model.  Perhaps when used as a construction surface.

Up to a point surface vs. solid is really just semantics.  I'm not really interested in feature for feature comparisons or debating pros and cons.  The prupose of a 3D model is to record design intent.  

Here is my crude example.

What do you see?

I see 2 cubes.  That is all I know for sure.  What was the design intent?  I have no idea if this is a shelled cube, 2 surface cubes, or a solid cube inside another solid cube.  All Rhino knows is that 2 poly surfaces are selected.

Here are 3 fusion cubes.

Which one is which?

These 3 shapes are all identical but my actual design intent is recorded in version C.

To your point about untrim.  When there is no history or feature tree untrim is a vital tool (Untrim of course is a Rhino staple).  However with history and a feature tree (like in SolidWorks) not so much.  My verdict on whether I need untrim in F360 is still out.  

phil

[cekuhnen]

HI Phil,

That example makes sense, however as a product designer I never in my carrer encountered such a shape or volume surface problem.

If Fusion should not only be for engineers but also for designers the software should also take into consideration what we do and how we think.

As a product designer it is quite common for me to first think about the A-surface and for such a task not only Rhino every surface tool has untrim.

Working on A and B surfaces in a surface modeler allows me to work efficiently on the detail level of each part as nessesary.

An example is a 3d texture sturcture on A but a flat along B.

Once both are done, they are joined and can be passed down the workflow.

Not needed a an untrim would also only make sense if the toolset of the design timeline would be radically improved.

Currently the DM mode is very basic and follows more the idea to execute a blueprint but not use it conceptucally to explore design variations.

The design timeline allows a certain type of freedom to explore ideas as long as you can build you desing out of solids and that is a drastic limitation to my workflow.

It was my understanding that Fusion should be a bridge between designer (surface approach) and engineer (solid approach) currently however it feels heavily being

solid modeler with its pros and cons.

[cekuhnen]

Thinking about your post of not needing untrim brought up the memory of cases where the model has problems features need to be removed, nurbs surfaces were untrimmed to get back the original hard edges or surface intersections and then the design was rebuild.

[AbdnAllHope]

I feel I need to say that you are not the only Product Designer on this forum.  Nor are you the only person who has taught 3D to students.  Sculpting, Surfacing, and Solid Modeling are important concepts that are software agnostic, and I have never prescribed to the idea of teaching to the software.  Rather bending the software to one's will.  My previous comments should in no way automatically label me as an engineer, nor should there be anything wrong with that if I was.  I have used many of these 3D programs extensively and at times exclusively.  I find a way to make the 3d model look like the drawing or better.  I don't always get to choose which programs I use, and there is often no point in complaining about it.  I do the best I can with the tools available even though the best tools may not be available.  When I am asked for my opinion I give it.  When I have a choice I choose.  Otherwise I just do the work.  Further more I summarily reject the idea that Industrial Design and Mechanical Engineering are somehow mutually exclusive.  Product Development is the very definition of skills overlap.  It takes a lot of disciplines to get the job done.  The best firms, designers, and engineers do this well.  I have learned to be flexible with my tools and with my approach to modeling.

[AbdnAllHope]

Solid modelers do this kind of operation just fine.  You can select fillets, and other features like protrusions and delete them to get the old sharp edge, or smooth surface back.  You can also edit the fillets or move and change the protrusions.  Thats direct modeling 101, and all the major players in solid modeling can do it.  Fusion 360 can do it too.  I'm not saying untrim is useless.  It's just not as critical to a solid modeling workflow.

[cekuhnen]

Phil,

what provoked you to write this if I can ask:
"I feel I need to say that you are not the only Product Designer on this forum. Nor are you the only person who has taught 3D to students."

I am also pretty sure I did not label you an engineer, or did I state that designers and engineers are mutually exclusive.

I was providing counter points to your argument but in reflection to Fusion and what Fusion 360 tries to be or who they try to target.

[AbdnAllHope]

I may have taken some of your comments a little out of context from the point you were trying to make. I think this is because we have different experience, and views on the subject matter. I realize that my comments might appear to be a little defensive. I apologize if I have offended you since that was not my intent. I was only trying to articulate my point of view in an effort to contribute to this discussion.

Phil

[cekuhnen]

All good.

I guess after all this talk, maybe Fusion should have three icons:

open shell

closed shell

solid

Regarding untrimming, if you design like in Inventor, than what you said of course makes very much sense, if

Fusion will also have a dedicated and feature complete parametric design history, which is somewhat I feel does not have (I come from SolidWork).

What I find interesting about Fusion besides TS of course is that from the start they promoted the software with a vision of bridging surface designer

and engineer into one workflow. While there is overlap they still have unique requirements and workflows which propably also evolved overtime into

what we see today. Rhino and SW are good for what they stand for but for a fluid workflow cannot be things improved. That is what caught my

attention with Fusion.

The engineers I work with would love to work on one and the same file meaning they can do their engineering stuff and have the tools they need

for their tasks and I have my surfacing toolset to generate what I want but both in one environment.

I actually do not mind mixing both ideas because I see the value in them. Working with constraint sketches and features is as great as working

with surfacing commands and profile inputs like in SolidThinking. but I can see that a hybrid of both worlds could be taugh to make and make even usable.

So I am very curious about the upcoming improvements to the design timeline and as it looks also Autodesk realized that in certain parts Fusion currently

falls short - well software development also takes time.

Regarding our previous discussion about untrim here is a screen recording in how I can do this in Fusion and in Rhino.

https://drive.google.com/file/d/0Byzv_NlyKp_2bHRadGFnMW5yVm8/edit?usp=sharing

Untrim can be done in Fusion via the Extend surface and that actually pretty well

Surfaces bend along two directions can also work while then it gets a little hard to control the extend and model can get

a bit messy.

That why with just a mouse click an untrim would be nice to have as well so the surface is reset to its orignial.

I think from my standpoint appreciating each method/workflow how engineer and designers work I am also curious if

the evolved workflows or approaches could not be done better and thats where I see Fusion's potential to provide 

a combination of both worlds in one interface.

I hope I was more clear and easy to understand now.

[AbdnAllHope]

Here I think we see eye to eye. I have used extend to get bits of a trimmed surface back in SolidWorks many times. My secret weapon though has always been Offset with 0.00 distance of a surface or group of surfaces before the trims or filleting. Kind of putting a spare in the bank so to speak. Gets dicey for the next guy who tries to follow your tracks though. SolidWorks has had un trim for a while now but old habits are so hard to break.

Phil