How to begin create this model?
First issue: You've used a Control vertex spline for the curve. Delete it, and use an Interpolation spline instead. Expand the spline menu for that.
Another way can be editing Sketch10, right-click on the spline and Convert to Interpolation, but time will be the same as above, because of new point placement is needed.
IMO, Interpolation spline should be the default option in Spline menu
Walter Holzwarth
Well, I tried the Convert to Interpolation Spline option. It can be done, but it's worse than creating a new Interpolation spline with only 3 points. I had to delete most of the converted points.
For point matching, you need to project 3 points from bottom circle, intermediate eliipse, and top curve into Sketch10. After that you can place coincident constraints with the spline, and adapt the spline shape by Activate handles and placing an orthogonal constraint at the bottom.
Now to 2nd issue: Your top circle is incorrect. You need to create a 3D intersection curve with this circle and the side view radius instead.
New intermediate file attached.
Walter Holzwarth
Both rails were not ok, because of the top end section.
This top end must be created as an 3D intersection curve of ircle 600 dia (=R300) and circle with 200 dia.2 Points (left and right) must be included
After that new 2DSketch11 and two guiding lines (15°), starting at these points.
Then another 2DSketch10 with projections from some lines of 2DSketch11, where a new outline spline can be set (Tangent to 15° guiding line, rectangular versus bottom line.
Now do similar for a right outline spline.
Walter Holzwarth
You can use only one sketch, but things don't get easier in this special situation.
I've made further steps, but I think @Anonymous should look at this..
I couldn't get the Loft completed with 3 sections and 4 rails. Some working around was needed.
Walter Holzwarth
This is no easy task for beginners, and it seems to be a general problem for lofting with Inventor 2017.
That's the reason, why I notified Johnson from Autodesk QA
Walter Holzwarth
Hi,
All that lofting and those splines are pretty annoying and not really the core of what Inventor is made for.
Anyways, I worked a bit on the latest model I could find in this post.
Building a loft can be annoying, as they fail often. I suggest to first make a loft of the horizontal circles (adapt the splines for that) and then cut out the upper part. You can use 'Split' for that. Then it didn't want to shell (which you should) so I used 'delete face'.
We've used 2 rails now, according to the excecise you should put 2 extra lines in, perpendicular to the ones you have. Given the shape, you probably need that. The combination of splines + lofting is just trial and error, I suppose that is also why they do this kind of excercise.
But we're good on track I guess.
Good luck!
asiteur schrieb:
.. But we're good on track I guess.
I don't think, that this attempt will succeed. My latest file does better, and it's only a short way for completing the task.
I'll do that now, but I'm afraid, that eas03 can't understand, what's been done. Some experience is needed here.
Walter Holzwarth
Hi,
Unfortunately Embossing only works on single curved surfaces. This is a complex surface and then you can't use emboss.
Extruding will work best, if you want to keep a single height for the letters, you can cut extrude using an offsett of the body, but that, in this case won't be very easy.
I've made an extrusion, because emboss doesn't work with 3D faces like that. You've seen by yourself.
Walter Holzwarth
Hi Walter,
I don't think Inventor Loft ever support same 2D Sketch in section selection. It is because the selecting different section profile within the same 2D sketch can get ambiguous. Also Loft is usually a protruding operation. Coming back to the same sketch may be rare. The same restriction does not exist in 3D Sketch section or 2D/3D rail selection. Please feel free to report it on Inventor Ideas.
Many thanks!
