Trying to merge Tspline surface with solid body

[Anonymous]

Alright, before I explain the difficulty I'm having, a little background on what I'm trying to acheive.

This is a painted foam model of the table foot I'm now trying to model. For the most part it's a straightforward solid modeling object, except for the top surface which is gently domed at the toe and transitions back to flat at the triangular pocket. I snapped a few quick shots with some side lighting so you can see the surface.

Now, I have finally managed to model the organic surface using the T-spline modeling space. I ended up doing it as a loft feature, and then tweaking it. Even that though has left it not quite perfect. I even used the Match tool to extend it  I am prepared to use it as a starting point though and remodel the rest of the foot to align.

I also tried the Edit Surface tool after going through the Create Base Feature process. The T-spline surface it makes though is registered on the long edge, which makes the sculpting assymetrical. I haven't been able to figure out a way to change the orientation of the base plane. Here some images of what happens. I quickly recreated the outcome so the dome is just roughed in, but you can see how it comes out lopsided.

Anyway, now I have an acceptable CAD version of the surface, but it's only a surface and I haven't been able to join it to the main body. In the sculpting environment I am not able to Fill Hole to close off the surface so it comes out as a solid. I've also tried just thickening it to convert it into a solid, but that doesn't work either. The Combine tool also doesn't work, combining a surface to a solid.  I've also tried some tools in the Patch enviroment, like the Stitch tool, but of course that doesn't let you combine surfaces to solids either.

I also tried creating it from a flat surface, and then sculpting it, but it was impossible to figure out the T-spline layout that when pulled and pushed would make the right shape. It always came out not quite right (and this attempt stays yellow for some reason). And it has the same joining problems too. 

So, I'm looking for some advice. Perhaps a way to join what I have to the main body, or how to get the T-spline surface from just a surface into a solid, or even a whole new approach.

Here's a link to the file if you want to take a look at it. http://a360.co/1L4cduw

Thanks for the help!

[jeff_strater]

One approach that can work in these cases, is to use solids to create a basic shape, larger than you need, then use TSplines to create some surface bodies for the sculpted areas, and use Split Body to trim away the portion of the solid that you don't want.

Take a look at this post, on modeling a carved top guitar body:  arch-top-guitar-model, for a step-by-step way to use this method.

It doesn't work in all cases, but I find it to be a useful technique.

Hope this helps

Jeff Strater (Fusion development)

[Anonymous]

Thanks for the link to the guitar body thread, that gives me some ideas.

As far as the method of making the contour and then cutting the profile shape, I thought of doing that but decided I wouldn't be able to control the perimeter thichness. Since I'm doming a rectangle the corners will be thinner than the sides as they are further from the dome origin. Perhaps I will try it on a test model though.

Bryce

[Anonymous]

So, I've tried a few approaches from the Guitar Body thread. One approach that I think could work is a lofted surface. I've gotten a surface shape that I'm really happy with, but I am unable to split the solid body with it for some reason. Here's what I've done:

First I drew all my sections. I wanted to make them all connected at the same center point, like in this example, but I wasn't able to get that to work. So instead I just spread them out a little and then patched the small hole. Perhaps my problem stems from this?

So I was really happy that I got to the shape I wanted. Then I extended the surface to protrude beyond the edges of the body and attempted to do a split body operation, but it is unable to "combine the geometry". It suggests checking inputs with the Validate Tool but it does not appear in the Inspect menu anyway. Plus I thought it was mainly for imported geometry?

Any ideas why the split body operation is failing? I'm thinking of trying to just build the whole thing out of surfaces and then stitch it all together and turn it into a solid if I can't get this to work.

Here's a link to this version. http://a360.co/1TN9asG

Thanks,

Bryce

[Oceanconcepts]

I had a similar problem I struggled with recently, trying to match an organically shaped lid for an electronics enclosure to the precise, planar edge of the rest of the case. I found the same problem trying to use the split tool. And using the Match tool destroyed symmetry. Come to think of it, that might be an idea station item- an option for the Match tool to preserve symmetry.  

What I recall is that I was able to either thicken the surface or add additional surfaces and stitch them into a solid. In any case, to get to a solid that I could use for a boolean subtraction from the base form. EssentiallyI used  t-spines for the shape, where I could incorporate symmetry, converted to a surface, converted that surface to a solid, either with thicken or additional surfaces, then used the boolean tools (which seem very robust in Fusion) to get the final form.  I don’t know if that will help, but for what it’s worth… 

This is the kind of problem that would be a great subject for a tutorial or webinar. Trying to incorporate the t-splines organic modeling with precise requirements of actual designs, and using t-spines, surfaces, and solids efficiently is a real challenge.  I know there must be many creative solutions. 

[jeff_strater]

Thanks, Bryce, for posting the model.

We will take a look at it.  However, my guess is that you are right -  the problems are with this patch where all the lofts meet:

You can kind of see, just from the model shading, that something is not quite right here.  But, if you turn on zebra stripes, you can really see that this is not kosher:

There are a lot of strange continuities here.  I still think that Split Body should work here, and the fact that it doesn't is a bug.  But, you can probably make life simpler for yourself (and the Fusion modeler) if you make this surface as a single loft, or maybe several lofts, but that meet without needing a patch.  Patch is a nice tool, but it sometimes generates wonky geometry that can affect downstream operations.

I will try to play with your design a bit to see if I can't get close with a single loft, or find a way to get the lofts you have to meet more cleanly.

Jeff Strater (Fusion modeling)

[Anonymous]

I actually also noticed the strangeness happening at the patch after making my previous post as well. I was looking at it with lines turned off and noticed the weird shading. It doesn't allow me to thicken the surface either, in fact it crashed Fusion. I really wanted to make it as one of fewer lofts, but wasn't able to get anything other than the broken up version I shared. I also noticed some of the loft surfaces are not tangent, but the loft errors if I turn on Tangent or Smooth.

Bryce

[jeff_strater]

Thanks, Bryce, for sharing this model.  It revealed a bug in our application logic that had not been discovered before.  I'll spare the gory details, but suffice it to say we were doing some unnecessary processing, and this is where the "problem combining geometry together" error comes from.  We didn't even make it to the split!  So, we will fix this bug, of course.  This case should succeed.

Having said that, I do think that you would be more pleased with the results if you can come up with a single loft to describe your dividing surface (or a TSpline surface).  The continuity of either of those surfaces are likely to be much higher than with one stitched together.

Jeff