Inventor won't let surface be used as a sketch plane

Hello,

I have a loft with two profiles which defines a ridge feature. The top surface of the loft (on Front view) needs geometry to be defined to continue it, but Inventor does not allow a sketch to be created on that surface. Presumably because the 4 points are not coplanar - but I can't understand how that can be:

* Loft is made of two triangles

* The "top" vertex of both triangles is defined the same lengths from model "ground", in direction perpendicular with model axis

* The "bottom" vertex of both triangles lies on a flat surface perpendicular to model "ground".

* Triangle bases are coplanar with model ground

* This means a surface containing two top points of both triangles and two bottom points of both triangles as its 4 vertices is a plane...?

The intended modeling operation is to:

* Create a plane on top surface of the loft

* Create a top-view design of ridge continuation on that plane

* Extrude down, to next face

This would create a continuation of the ridge which was lofted.

Does anyone know why this can't be done this way, or what is the recommended way to proceed?

UpperArmShoulderNew2.zip

I might see geometry a little differently - but it is obvious to me that face isn't planar without even doing any inspection.

But go to Inspect>Surface, click Autorange and Apply.

or

any plane can be defined by 3 points.

Start the workplane and pick any 3 of those 4 points - you cannot create a plane that will go through all 4 points.

I have not had time to offer much on this one, but I am fairly certain that I would not likely be using Loft features for any of the features created so far.

BTW - in solid modeling we refer to the "Faces" of a solid body and "Surfaces" are geometry that have no volume (infinitely thin).

If you go to the top of your browser you will see a folder for Solid Bodies and one for Surface bodies. You have one solid body made up of several Faces. You have two surface bodies in your file. Those surface bodies are quilts comprised of several stitched Surfaces.

And yes, an easy way to check to see if a face or surface is planar is to simply try to select it for a 2D sketch. Inventor will only allow selection of planar geometry for 2D sketching.

"[...] I am fairly certain that I would not likely be using Loft features for any of the features created so far. " (JDM)

I see that you have a few pages with tutorials, including items in "read before you post" thread in this forum. Getting through all of these non-selectively could take a long time. Can you suggest specific ones that apply to the problem of creating these features your way?

I think most (if not all) of those tutorials deal with more complex geometry. (Except for maybe the Inventor 101 which is too simple for this problem.) So I guess this one is a sort of "middle ground" that I haven't documented anything that would be of any help.

I re-created the features using "surface extrusion and plane" approach; defining the top profile on one plane, extruding as surface, and then slicing off the top with another plane. This has the advantage of the top surface being a guaranteed plane, simpler process, easier to modify, and it seems like more intelligence is built into the model.

For anyone who might be interested, I am attaching the completed model (excluding the diamond tread cross geometry, which runs file size over limit, but it's done the same way).

UpperArmShoulderSmall.zip

....which runs file size over limit, .....

To dramatically reduce file size - find the red End of Part marker at the bottom of the feature tree.

Drag the red EOP to the top of the browser hiding all features from the graphics window. Save the file in this rolled-up state and zip.

On the other end - the user will simply drag the EOP back down (it is the graphics, not the geometry definition that explodes file size).

Thanks, I will remember that for the future! Too bad I didn't see this note in any of this forum's pinup threads, perhaps I missed it.