Problem using loft - hollow shapes - need help

[simon.dyer]

In the photo below you will see my problem.  Thin sections appearing in the wall that create holes and other inconsistencies.

I started off thus:

- create sketches along the path of my shape

- loft them

- hollow them to a consistent wall thickness using the shell command.

Problem - shell failed, I think because the sketches defining the loft had different number of points, multi-use of splines, lines, fillets.

So I used method two.

2. I created an offset for each segment sketch, then made another loft through those offsets, which I cut from the outer shape using a Boolean.

I hope the offset loft would use the same algorithm, and produce a consistent offset.  It didn't and the wall thicknesses are all over the place.

Please suggest 'best practice' to achieve hollow organic shape with consistent wall thickness.

[jeevesme]

Do you have to use the Model environment? If not, you can go into the surface environment and create the loft you want then use the thicken command.

[michallach81]

Your initial way was the ONLY correct, which is to build solid shape (regardless of initial modeling method, through solid or surface modeling) and then use shell command. If a shell fails to do what it suppose to, then you must change your geometry. There might be some workarounds, but if shell fails then it means there is a geometrical problem with your part and it must be resolved not worked around. Under certain circumstances, you can try to thicken the outer surface instead of a shell, but first I would try to find reasons why the shell is failing.

[simon.dyer]

Hi @michallach81 I am fairly sure the problem is caused by the sketches at each profile position being wildly different shapes, needed to traverse a specific path -I dont see how I can change that to then enable shell to work.

I am not enough of a cad engineer to know the proper approach.

[simon.dyer]

@jeevesme - thanks I tried that but the profiles I have (like ribs along a plane fuselage) cannot be used to make a patch surface. I think that needs lines along a path, not what I have which is sections (aka profiles/sketches) along the path of how I need the shape to be.

[michallach81]

If so then try to build that channel with simple boxes, or if it must be "organic" try T-splines

[simon.dyer]

Many thanks @michallach81, -Splines are working much better for me than previous. Like 99% there.  It will even make a shell using splines of different numbers of vertices, if careful.  Too much twist on the shape and it wont work.

It wont work with a spline and a rectangle, even if vertices both equal the same (4), so joining an organic shape to a non-organic primitive directly cannot be done and will need to be made separately with a non smooth interface.  I cant see how to avoid that, at this stage. Im sure it can be done ( a square loft to an amoeba, with shell effect ) since we're limited only by our imagination, right?

[michallach81]

Discussion without specific example is too abstract and too academic. I can help if you have a specific question, or I can try to model something "nice" if you will provide the original file.

[simon.dyer]

I stand corrected @michallach81 - I can do shells in mixed profile lofts - here I managed circle->square->poly (4 & 5 vertex).  It has some limits on how wild the polyshapes can be, which I havent quite defined.

[michallach81]

It's too academic, and I have no time to argue. What you must understand is that lofting through several different profiles is the WORST way to articulate complex shapes. Do the same but in sculpt workspace (just loft Tspline).

[simon.dyer]

I hope I didn't come across as arguing the point. In just trying to understand how to make these shapes and do appreciate your suggestions.
I'll try the sculpt method next. Having been in there yet.

[designingberlin]

I disagree with your point.

1) Sometimes even surfaces that have to reason to fail in shelling do fail in shelling. I came across this very often.

2) Surfaces of bodies may be very complex and hard to offset. That's just how geometry works and self intersecting may be hard to avoid.

My current aprroach to shell complex objects is to generate all surfaces in the patch environment.

Offsetting the single surfaces usually works well in fusion and you can join them later in the timeline. or generate a boundary fill.

This may not work for all geomatries, but for ours it's fine.

@simon.dyerYou might have to add a loftguide. My approach would be to addd a plane in the object, create a sketch on that plane, project cut edges with the outer shape and offset the cutlines + some finetuning.

Best,

Stefan

[michallach81]

Hi Stefan,

As I said my argument would be an "academic", and proper explanation would take time.

Simon has a problem not with a modeling but with an articulation. He can't imagine how that part could look like, therefore he doesn't know how to approach it. Instead of fighting with shell/thicken/offset or any other tool, he should remodel that duct part. Without giving anyone a training, I can only advice to first draw that part on a paper. This way he can force his imagination to do what now seems to be impossible (while drawing, line after a line he will face numerous problems which he will have to solve, to progress).

Any attempts to work around this will eventually lead to more problems. 

Now about your points:

1. How do you judge that certain surface "have no reasons to fail"? In Fusion 360 we don't have tools to perform such analysis. If your judgment is based on your impression then you should re-evaluate your abilities (in fact our human abilities, not just yours)

2. "self intersecting may be hard to avoid", are you kidding me? This is CAD program and its purpose is to assist in designing manufacturable parts. If you manage to get a self-intersecting surface, then you must rethink how your part should look like.

I've mentioned that "lofting" through several profiles is the WORST way to articulate complex shapes. The main reason is that our imagination fails to understand the relationship between each profile, therefore, we never know what relation we do create when drawing them.

Below is a screencast where I create a simple example:

My main argument is that middle profile don't match relationship that is defined, between first and last profile, by the rail. In my example, nothing is yet bad, but you should see already the difference. I've created also gif showing underlying geometry:

[simon.dyer]

@designingberlin

I have discovered the sculpt environment, and Im finding it more tolerant of the crazy shape Im trying to do.

(I tried the patch environment but having trouble making it work - wont loft my closed profiles, wont use rails if I add them)

Sculpt however will use my profiles, BUT it creates seperate bodies which can be thickened but dont overlap.

Please see below.  How can I force it to create one body when I loft my profiles?

[simon.dyer]

@michallach81 Thanks for the video showing how to build patch from scratch.  Please be assured I do know what Im trying to build.  There are two openings from other items, and I want to build a 'pipe' between them, turning and shaped so it does not hit the other objects.  I have 3 or 4 profiles defined.  I just want to loft/patch/sculpt/whatever between them with the pipe forming into the end openings (rectangle) and have a 1.4mm thickness.  I dont know how to do it in Fusion.  The method you show goes back to using little sections of wall.  If its computer aided design then I want it to aid me and make the tube how Ive defined it wikthout the need to patch it all together from little sections.  Clearly I don't have the experience that you have.
You asked earlier for a file.  Here it is attached.  Ive set it up to display only the regions I am stuck on.  There are two fan ducts. At the fan end, the pipe needs to slip over with 0.25 clearance(created in profile)
At the other end, the pipe will be combined with the body parts.
Any comments on this specific example are welcome.
Im not asking anyone to do the job for me.  Just how to encourage Fusion to make this clearly defined pipe. 

[michallach81 · Accepted solution]

Hi Simon,

The first thing to say is that the way you've built the file will cause more problems. There are too many warnings in the timeline. Also, your use of components and bodies is inconsistent.

I wish that current position of fans is somehow intended and not just random, but I'm guessing you can place them a bit better. Now it is very tide and we have to drive duct through very narrow "corners". When I was speaking about bad articulation I was talking not only about bad profiles but also more general. You should consider redesigning at least how fans are placed.

Now a bit academic question, how did you find placement for construction planes for your ducts? You were guessing, and that's bad. You should drive that form already existing data, like the position of inlets. For example, you can create a path from an inlet to an inlet, and use that path to create construction planes at least at a right angle. That path could also be helpful in loft command.

Here is my simplest approach, I don't consider it as a good practice, but the good one would require redesigning big parts of your printer (?):

[simon.dyer]

@michallach81 many thanks for showing me many techniques in that video. And it created the shell without issue.  So in short, it looks like my method using profiles along the path was actually making the whole loft more difficult.  I was intrigued to see how it created the shell right through from end to end even including the extrusions you did at each end and the loft between. (I thought they we separate bodies)

Anyway Im going to take your advice and move the fans into a more ideal position.  They behave oddly when I move them, asking me to 'capture the position'.  Is that because they were converted into components?  I'll also try your projection method from the openings - hoping the bodies I create will move if I tweak the fan positions.  Currently they do not.

You might have guessed I did not create the original model of the printer.  Just adding my fan ducts.  No one else uses twin radials on e3d thats Ive found, so looking forward to seeing the results.

Thansk again for your effort assiting this newbie in my first more organic design.  And Phew - I can learn patches another day!

[Anonymous]

Good how-to-do videos guys !

I was experiencing the same/similar problem in message 14 of 17, simon.dyer in reply to Rankstefan, but I am a total beginner and I am still learning the tools and what they are used for. Unfortunately, I learned the hard way before reading this & found out myself via experimenting with the Sculpt environment that the Sculpt managed to do what the Loft command was not, even though a complete beginner, I could not get the Loft to work, however, the Sculpt did what I required the Loft to do.

I used the Sculpt for the narrow nozzle below to join the nozzle only to the curved tube...

[TrippyLighting]

@Anonymous Looking at your design, its really all over the place. Your timeline rally looks like a mine field with all those move operations and yellow highlighted sketches. Yellow and red icons in the timeline indicate warnings and the root causes for these need to be addressed soon rather than later.

[Anonymous]

Thank you for the reply and advice!

I have no idea what those errors mean, I just try to get through by basic trial and error, total beginner ! I am slowly learning though as I play more with fusion 360, but I never expected software to be so advanced yet so effective.

Perhaps I should check out some videos on youtube to learn more on certain tools and errors 

PS : When you use the sculpt command instead of the loft tool, I noticed that you cant combine and export the body as an stl file, any ideas on how to counter this ?