Why I can't use sketch on lofted part

[ziga.bacnar]

So basically I created a loft by using two sketches. Between them was created a solid just like I wanted to. But the problem is that on this solid's face I cannot create another sketch. Red arrow is pointing towards the lofted part

[SBix26 · Accepted solution]

If a face cannot be selected for a new sketch, then that face is not flat.  Not mathematically flat, that is.  Loft is not a precise tool for creating well-controlled geometry, so it is not surprising to me that it didn't create flat faces.

If you're allowed to, please attach your file here and I expect someone can show you how to model this without Loft and producing flat faces.

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Sam B

Inventor Pro 2023.1 | Windows 10 Home 21H2

[johnsonshiue · Accepted solution]

Hi! Sam is right. The face may look flat but it is not flat. It could be a spline face. I suspect there could be some minor deviation between two section profiles. Here is what I would do.

1) Turn on the visibility of the two section sketches.

2) Measure the angle between two matching lines (from both sections). They should be parallel. If not, add constraints to ensure they are parallel.

If they are parallel, the lofted face should be flat. Otherwise, it will be a bug. Please share the ipt file here. I would like to take a closer look.

Many thanks!

[cadman777 · Accepted solution]

In addition to what's already been said...

When you have two edges that can't make a flat surface with any of the 'easy' tools, then you make it a sheetmetal part that consists of triangles that have a press-formed seam across the shared edge. Usually you run a diagonal line from lower to upper corner and build a box around the whole thing. Then you can use the sheetmetal tools to make the face.

[Cris-Ideas · Accepted solution]

@johnsonshiue 

Actually it is not strictly the case.

Face can actually be mathematically flat and still it may not be possible to define sketch on it.

It happens if it is created by operation that is not registered as producing planes, like loft in this case. 

As loft is interpolation by default it is describes as approximation and although result can actually be actual plane it is not recognized as plane by Inventor as it is not defined as plant, and therefore it is not available for direct creation of sketch.

There are also other "edge" cases when produced object is actually a plane, in strict mathematical conditions, but is not recognized as such object.

Fun fact. Two axis defined in 3D, that actually cross (they have a common point) are not recognized as coplanar by Inventor. In fact mathematically, as they cross they produce a plane that they both fit in, so in fact by definition they are coplanar, inventor however sees it differently.  

To make a sketch you need to define  work plane and sketch on this plane.

[ziga.bacnar]

Thank you so much, I totally understand the problem now. I am going to attach the file, to help you see the part where the problem occurred.

[SBix26 · Accepted solution]

Yes, I see that the edges used to create the loft surfaces are not coplanar.  The resulting surfaces cannot possibly be flat.

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Sam B

Inventor Pro 2023.1 | Windows 10 Home 21H2

[johnsonshiue]

Hi Cris,

Many thanks for your feedback! Your comments are very interesting. Some are not consistent with my understanding. Let me embed my reply to your comments.

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@Cris-Ideas wrote:

@johnsonshiue 

Actually it is not strictly the case.

Face can actually be mathematically flat and still it may not be possible to define sketch on it.

It happens if it is created by operation that is not registered as producing planes, like loft in this case. 

As loft is interpolation by default it is describes as approximation and although result can actually be actual plane it is not recognized as plane by Inventor as it is not defined as plant, and therefore it is not available for direct creation of sketch.

[JS]: The way Inventor Loft works is that if an analytical face can be created, Inventor should do it. If not, it is a bug. The only exception is that the section profiles are straight spline as opposed to a true straight line. If you have an example showing that an analytical face is possible but the Loft generates a spline face, it will be a bug. Please share the example.

There are also other "edge" cases when produced object is actually a plane, in strict mathematical conditions, but is not recognized as such object.

Fun fact. Two axis defined in 3D, that actually cross (they have a common point) are not recognized as coplanar by Inventor. In fact mathematically, as they cross they produce a plane that they both fit in, so in fact by definition they are coplanar, inventor however sees it differently.  

To make a sketch you need to define  work plane and sketch on this plane.

[JS]: I also want to see an example here. Two coplanar lines in a 3D sketch should be recognized as such. Please share an example that exhibits otherwise.

Many thanks!

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