Problem lofting complex surface

[Anonymous]

Hi all,

I'm having issues lofting a surface from contour polylines drawn on 'elevation' workplanes. See IPT attached.

Lofting either fails (unable to solve) or I end up with strange bulges and other geometry that doesn't make much sense.

I'm trying to get a solid with a smooth surface, similar to the attached image.

Am I doing something wrong, or is inventor not the right tool for this task?

[johnsonshiue]

Hi! Inventor was not designed to create terrain survey shape. It was designed to create the ideal digital twin, which you will make in real life.

Loft is more like a freeform tool. As long as the resultant shape passes the sections (and G1/G2 continuous), it is considered a legitimate solution. You may try Boundary Patch with guide rails to see if you get a better shape. May I ask what you want to do with the surface?

Many thanks!

[jhackney1972]

Your part contains some very complex "open" geometry.  If Inventor can loft all these sketches together is very doubtful because they are overlapping in places and as I said very complex.  You will only get a lofted surface because they are open sketches.  I lofted seven of the splines together to form a surface and then thickened that surface to 1 mm thickness to make a solid and it took Inventor 10 minutes to do it.  I received some bulges in the surface but the thicken command worked those out.

If you are going to do it, you will need a hefty workstation, and lots of patience.

[Anonymous]

Thanks for the replies. It sounds as though Inventor is not the right tool for this task. I'm designing a structure to be placed on the terrain, the structure is all bespoke components so I would rather model it in Inventor than Revit.

Perhaps the best workflow is to export this drawing to another program, create the solid body, and then import back into inventor. What would be the lowest friction way to do this? Revit?

[PaulMunford · Accepted solution]

You could do the terrain map in Revit and then open the Revit project in Inventor?

[johnsonshiue · Accepted solution]

Hi! I took a look at the part. The sketches exceed the valid model range. Inventor geometry has to be bounded in a cube to +-100m in XYZ. Each single piece of geometry has to be smaller than 100m. I think you will need to us AutoCAD or Revit to do that. Like I mentioned before, the geometry created in Inventor is meant to be made in real life. Another tool you may consider is 3D Max. You can make mesh based on these curves (export as IGES and import to 3D Max).

Many thanks!

[WHolzwarth]

I've played with the topology, too. Here's what I noticed, not every comment is new stuff in this topic:

- Some bulges were visible in Inventor's loft here, too

- Trying to add all sections into a single loft slows response time more and more with each line

- The last line is closed and can't be added easily. But there are ways to go

- Trying a loft over all lines (except the closed one) in Rhino was rather quick, but bulging appeared there also

- Therefore creating several Inventor lofts - each with only two curves - seems better. But even then bulges appeared

- Remedy seems to be manual adding of transition points. Much additional work would be needed

I'm not very experienced with 3ds Max, but I'll try to get a result there. I'll report, If I'm having success.

I've seen Johnson's comment about 100m limitations. I'm convinced, that scaling down this geometry doesn't change anything. Longest dimension in this sample is near to 300 m.

[Anonymous]

My interpretation of the documentation regarding the 100m limitation is that it’s not a hard limit, however beyond this distance some precision is lost due to the way coordinates are stored internally. I’m guessing these are either 32 or 64bit floating point values. The end result is that tolerances can’t be guaranteed beyond 100m.

I agree that the scale is probably not going to make much difference. I’m close to giving up and redrawing it all in Revit - I haven’t been able to get dwg import to work... the model imports in the wrong orientation, as in Inventor, the XY plane is designated as the Front view, while in AutoCAD it is designated as the Top view.

[johnsonshiue]

Hi Guys,

Indeed, even if the sketches are scaled to within valid model range, the loft would not look nice. Like I explained earlier, Loft is more like Freeform. The geometry is under-constrained. As a long as the G2/G1 surface passes the sections and follow the rails, the solution is legitimate. Also it is a mapping technology, meaning the vertices from one section need to be mapped to the next. Inventor uses an algorithm to do the mapping. It is based on the number of vertices, the relative position of given vertices, and the curves. You can manually override the automatic mapping.

For this particular case, another option is to use Boundary Patch with Guide Curves. You can create two separate splines on each end to close the loop. Then create a Boundary Patch -> select the inner curves as Guide Curves. Sometimes, it provide a better alternative solution when vertex mapping becomes out of control.

Regarding the valid model range, it is strict. We do have customers modeling outside the range without problems. However, it is case by case and it may not work for every case. Also, the behaviors outside of the range are unpredictable.

Many thanks!

[WHolzwarth]

I've tried it now in 3ds Max, both 2017 and 2018.

Terrain creation is rather quick, but not as it should be. This seems to work well only in ascending regions. Valleys are neglected.

Look at the right side of the picture. Lines are extending from one hill top to the opposite one.