can't select sketch for loft

[Anonymous]

Hi!

I use the following tutorial:
https://www.youtube.com/watch?v=cBW782jzs3M

At 1:50 the author creates loft

I follow the tutorial, but I can't create loft, I just can't select the sketch.

This is image before loft.

In order to make loft I need to draw the marked line, then it works,

but the author doesn't have these lines and it works.

What do I miss??

Thank you!

The files are attached

[tschaeferZNBXX]

Worked fine for me.

Be sure that your lines are attached to the projected geometry of the block face.  If they are not then you have an open loop which will not work.

[Anonymous]

Yes, I have an open loop

The marked line is missing.

but in tutorial this line is also missing

Thanks

[tschaeferZNBXX]

In the tutorial they are attaching the lines to the projected face line at the top.

When you are selecting your faces are you using the browser or trying to click the model? I did it just how they did (using the browser to select the sketch) which worked just as shown.

[mdavis22569]

@Anonymous

Had the same issue ...we fixed it on his post ...

I can't find his post ..but if he can click it it might help

[Anonymous]

-Make sure LOFT area is closed. You can make sure by using EXRUDE command.

-When LOFT command is active click on the border line.

[tschaeferZNBXX]

I did not have to create the additional line at the top.

I projected the face of the block and then attached the lines to the top edge of the block just like the tutorial. There are many ways to close the loop but by doing this we limit the number of dimensions needed.

[Anonymous]

From my understanding I realize that lines created by PROJECT GEOMETRY is merely a reference line. It cannot be considered as a GEOMETRY line. But some times it will work when an area is enclosed by reference line only.

If area is enclosed by assorted lines you may have problems.

[tschaeferZNBXX]

I have used ever since I started Inventor in 2003. I have never had an issue with it or had them as just reference lines. Maybe I am wrong but I do not believe they are just reference lines and can be used as actual lines.

I think the problem is that the top line goes outside of the two lines that create the loft and that is why the sketch was selected from the browser instead of selecting the sketch in the model. Since the top line does not end at the end points of the other two lines Inventor has an issue knowing what you want. When you select the sketch from the browser then can figure out there are two areas possible.

[tschaeferZNBXX]

Another thing is be sure that before you try to select the sketch you have the "Remove" material selected not the "Add" material for the loft.

[mdavis22569]

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@Anonymous wrote:

From my understanding I realize that lines created by PROJECT GEOMETRY is merely a reference line. It cannot be considered as a GEOMETRY line.

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Nope ...not true ...

Look at your loft exercises you've done. You've projected geometry and extrude in those exercises.   

[JDMather]

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@Anonymous wrote:

From my understanding I realize ....

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I have used Projected Geometry for 15 yrs.  The behavior hasn't changed.

They are not "reference only" unless you change the linetype to Construction.

My preference though, is to exactly that  - change them to Construction and only use for reference.

That way if something "goes sick", it is much easier to fix the problem in my experience.

[Anonymous]

Problem is if all GEOMETRY line all the end points will be clear. If a PROJECT GEOMETRY line there is no end points, only highlight of a line if you miss that you will not get a closed area.

[tschaeferZNBXX]

There are end points and the new sketch becomes adaptive to the existing GEOMETRY.

The tutorial clearly shows the dimension to the end points of the new lines added and they are attached to the top projected edge.

[Anonymous]

Yeah!!!!!!

It works!

The problem was that the top line (projected geometry) was set as construction line,

after I removed construction option it works fine

:)))))

Thanks for all your replies

[Anonymous]

I made an account here just to answer this question.

Right click the sketch in the feature tree and click show. I had the exact same problem, struggled for way to long of a time, and then tried this and it instantly worked. For anyone else that finds this post, here you go.

[kelly.young]

Hey @Anonymous thanks for taking the time to create an account and share your experience, that's awesome!
Welcome to the Autodesk Community!

When making a Loft feature I would draw the triangle explicitly with the Project Geometry of the face edge(s) as construction.

Unless you are actually cutting through something to find an edge I would not use Project Cut Edges as that has a greater tendency to become sick in advanced situations in my experience.

You can use the projected line, but as good practice I like my lofts to have independent closed loop lines defined and constrained.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[johnsonshiue]

Hi Guys,

Just to add to Kelly's reply a bit, Inventor Loft command probably has the most sophisticated selection behavior. It is because Loft allows you to select an edge, a face, a closed or open loop in a 2D sketch, a closed or open loop in a 3D sketch, a sketch point, a workpoint, and a vertex. It is very versatile. As a result, the selection behavior can be a bit confusing. If you have multiple loops in a sketch, you will need to select the sketch first and then select the loop. Otherwise, Inventor does not know what you are trying to select.

Many thanks!