Face Vase Modeling Help Needed!

suzi_grossman

I'm trying to do a kind of tricky model and I think I'm on the right track with a loft along a guide curve, but it's not quite working. I have two complex profile sketches from imported dxg files that are on the same plane 180 degrees apart. I want to do a rotation, but also morph from one to the other as it rotates.
 
Here's how it looks with just a normal rotation with one of the profiles, which is what I want, just plus the morph.

I tried making a circle as the guide path to loft between the two profiles, but I think I must not be understanding something because I get some pretty funky results. Here is the circle:

And here are the results. It looks like it is making a weird shape inside that's confusing things?

Any ideas on how to solve this? Thanks!!

glen_dewsbury

You mention 'Loft'. Why not a revolve of one half?

eric_pesty

I don't think a circle is enough to guide it. Also by definition if the profiles are different then the guides aren't going to be circular arcs...
I think you are going to need multiple "guides" along the the way at least one at the top as well probably a few intermediate ones.
You may also have to add an intermediate "section" at 90deg (you could do that by superimposing the two sketches and getting a "midpoint" line although I'm not sure there's a way to do this automatically so it would be really tedious with the number of points you have!

There is a slight possibility it could work "as is", have you tried enabling the "match profiles" (or whatever it's called), it looks like that could be part of the issue from the bottom image...

EvanReese

If you can share your doc that will help. If the import is actual tangent continuous curves, you could use the fit spline function to make each profile into a single curve, which would make synchronizing the loft a lot easier. You've got the right idea though!

EvanReese

@suzi_grossman

I have this thing where I see a CAD challenge and can't stop thinking about it in the back of my head even if I want to... so I have an update for you, haha!

I see now that your import seems polygonal (made of lines, not curves), so you can't use fit spline to combine all of the edges to help with lofting. You could, however, still use the fit spline tool and select each point one-by-one in order to make a smooth curve through them. I'd only do the parts that are unique (so focus on the faces), then use the normal sketch tools in onshape to sketch the rest of it. You could make the inside of the vase smoother by re-sketching it anyway. Once that's all set up, I think lofting with a path should work. This is the slow "get it done" solution, but if you're doing this kind of thing a lot I'd take time to find a better workflow.

_anton

I was curious how well this would work, so I conducted an experiment: https://cad.onshape.com/documents/f3053e99941819d7ec94b74b/w/04331cef9037dd871b1ffa62/e/6301b090a4159fdaf8ce5a9a

I greatly simplified the sketch, drew fit splines between corresponding points, and did a loft.

steve_shubin

suzi_grossman said:

I'm trying to do a kind of tricky model

https://cad.onshape.com/documents/10bab0a12ed2b6c1759fb694/w/2c3dc803bdf42011023ca227/e/68e1e2ff435e8a7040639cde

Maybe I’m missing something

EDIT — and I really was missing the point

And it finally came to me. See my 2nd  post below this one

steve_shubin

Oh by the way

I think Anton has the best little logo or whatever you call that

Every time I see that little hippo with the beady eyes, it just cracks me up

S1mon

@steve_shubin

I think the whole point is that there are two different profiles of two different people. As the surface revolves around it morphs from one person to the other.

The recently added loft connections might help with this problem.

I would also recommend sketching one side with some splines and mirroring them, removing the mirror constraints and then tweaking the positions of the control points of the mirrored version to match the second profile. When you have similar splines, you’re more likely to get a loft which behaves better.

steve_shubin

Yeah my slow gray matter finally put two and two together and figured that this has to be some existing piece of artwork or what not

anyway if that were the case, it seems that you’d want to put this on a turntable with one of the new iPhones on a tripod and use the LIDAR, but whatever

whatever the case, here’s my loft version

Although it could probably do with some cleaning up

And I did exactly what you talked about doing Simon. To draw one side and mirror and then remove the constraints and adjust. And this kept me from having to play with any type of connections

https://cad.onshape.com/documents/c8df6fa178c4bef62de18087/w/72d3fb6d5ac6f22ef4484a80/e/dbb90e6a6914fc348c152472

MichaelPascoe

Ohh, I see it now!

suzi_grossman

Thanks for all the suggestions and ideas everyone! I originally had curve splines when I made the profiles in Photoshop, but it doesn't look like I can import into Onshape while maintaining the curves since the files formats they accept I think only do straight lines unfortunately. Since this is a one time project through I'd be willing to redo the curve splines in OnShape so that's a good idea to simplify the shapes. I haven't done splines in OnShape before, I'll have to learn about those. And Steve that looks great!! Very much what I am going for. Thanks for the test! It looks like you used a circle at the top of the vase as a guide? 

suzi_grossman

In case anyone is interested, both of the profiles are actually me! I had jaw surgery (for medical reasons, but it changed how I look) and they are the before and after. I've been doing art in a number of mediums about the process and as a way to reconcile with my altered appearance. Here are the photos that the profiles were traced from:



And these are the single profile vases that I've 3D printed:

steve_shubin

@suzi_grossman

I like how the vases turned out !!

Yes you’re exactly right. Sketch 3, was a circle that I split in half. So at this point it is a 180° arc. And yes, it was used as a guide.

I used 180° arcs for both the path and guide. I did this because I wanted to extrude the two main profiles off of the front plane so I would have some faces to use for the MATCH TANGENT at the start and end of the loft. So if I have extrudes that are NORMAL TO the front plane, and both 180° arcs start and end on that front plane and are coincident to the profiles, we’ll that will allow me to use match tangent in the loft

So below is a picture that shows how the outside faces ended up being tangent as a result of that. No crease where the front and back came together upon doing the mirror of surface

But notice how the inside is not tangent, and there are creases on the inside

So on the inside, I got lazy. I did not make extrusions for match tangent on the inside loft. But that certainly could be done

I also was a bit lazy on the main sketch of the two main profiles.

I first sketched the right side and then mirrored to the left. But notice that there are some blue curves on the left.

Well, after I removed all of the mirrored constraints on the left, in order to move the curves into place, like I said — I got lazy, and failed to fully constrain them by using the fix constraint. Of course it can be done. So as is, you have to be careful not to move any of those blue curves

steve_shubin

WOW !!!! it took me a long time to get what was going on here

Well for starters. Even though it was titled FACE VASE … The word face didn’t register with me at all. I saw vase and I thought — OK, here we go

Then I read Simon is referring to these profiles as persons — and I thought — ‘maybe that’s the way some mechanical engineers refer to a technical profile’ — as a person.

Then I see some artwork by Michael that looks kind of like some type of foliage or what not spilling out of a vase. And then I looked down and I see his artwork was voted up four times. And I think — ‘I guess everybody really likes his artwork’. And I know I did because I think I was the first to vote it up

And then I see Suzi post 2 pictures of herself. And I thought – ‘well that’s interesting that Suzi would share that with us’. And the thought passes through my mind — ‘I think one of my nieces might’ve had some kind of TMJ surgery or whatever it was’. But I still didn’t get it.

So I figure you guys should all have a good laugh on me because I’ll tell you what, I sure had a good laugh once I finally realized what was what. Slow as all get out — I FINALLY SAW IT. Belly laughing out loud 

suzi_grossman

@steve_shubin Too funny!! And so helpful even without knowing what was going on lol!

suzi_grossman

Ok I think I'm getting really close to getting it to work. I redid the profiles using splines. No matter what I did with the inside it still wanted to connect the inside to the outside which created an impossible shape, so I switched to trying to make it work as a solid. It looks to me like it's doing exactly what I want, but it is still giving me an error "could not create loft with given information." I tried it with both a semi-circle and a full circle and seem to be getting the same issue. Maybe I'm missing something essential about how lofts work?

Here is the link to the project. https://cad.onshape.com/documents/514325f5a53490ec0db47b5d/w/01774faf8c8be8fb8c264ba1/e/6e505c9402efa307b5706d78?renderMode=0&uiState=64150579fa9ad113ece4ed5b

It doesn't show up initially since the loft isn't working, double click the loft to see it. It looks like it should be doing exactly what I want, I'm not sure what the issue is, any thoughts? @steve_shubin ? Thanks!! (And sorry it took me so long to get back to this, I got distracted by modelling a capybara lol)

Here's a screenshot:

glen_dewsbury

Had a little time on my hands today so I thought I'd give this a go.
It was a bit of a challenge for me.
https://cad.onshape.com/documents/9b7aa1ef7fed9cdc1f9226bb/w/3bdb142e3d9fb68f5e68f87c/e/279ed955883c65d69b0266fc

suzi_grossman

@glen_dewsbury Interesting! You're defintiely using some techniques I haven't learned yet. I think I'm confused about the difference between a guide vs a path for a loft. How are they different?

glen_dewsbury

Take a look at part studio 2 and you will see the difference. Guides will give individual paths that can each be modified to produce a shape. A path in this case is a single curve that can modify the shape. When you have a shape that is prolematic to loft guides and path can help. Note that I also went through the original profiles to give them the same number of segments each. Odd numbers of segments can be less effective, like square to triangle. There is a way to make it better but not as precise. 
https://cad.onshape.com/documents/9b7aa1ef7fed9cdc1f9226bb/w/3bdb142e3d9fb68f5e68f87c/e/7b4e231438db3ad37cf776c6

BTW The last surfice put in has no path or guides. If loft will get you what you want without, then less overhead.

Ste_Wilson

@glen_dewsbury really helpful little demo there!

suzi_grossman

I did it y'all! Turns out the trick was that I need to have the same number of spline points for both profiles. And I just hollowed out the center by removing a rotated shape. I'm excited to see how it prints!


And thanks for the great guide and path tutorial @glen_dewsbury !

glen_dewsbury

Looks good.

suzi_grossman

Here's the 3D printed version! Thanks for all y'all's help and encouragement!

Starting position:


Rotated 90 degrees:


Rotated 180 degrees:

Paul_99

Great job of keeping on track! You might grab one of these turntable things (I'd cover up the lights and mirrors in this case but they are cheap and strong) and about the right size.

 https://www.sciplus.com/revolving-multicolor-led-pedestal-50690-p

Mainly because I want to see a video of it spinning and the profile changing back and forth!