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Loft between 3D sketch and normal sketch

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Message 1 of 42
wolterh6
7892 Views, 41 Replies

Loft between 3D sketch and normal sketch

I have a cylinder on top of a curved surface; I want to make the cylinder land adaptively to the surface, so I projected the circular face of the cylinder in the surface, which ended up being a 3D sketch. I tried to loft a solid between both curves, but it always gives me errors. Some examples are:

  • The attempted operation did not produce a meaningful result. Try with different inputs.
  • Multiple disjoint loops found in a profile section.

I have attached a test case.

 

I have had success when trying to do the same thing with curved surfaces in two dimensions only (e.g. extruding a 2D curve), but I think the error is produced since the curved face I am trying to use belongs to an elipsiod.

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41 REPLIES 41
Message 2 of 42
JDMather
in reply to: wolterh6

I don't understand.  A loft would simply create a cylinder.  So why not extrude the circle To or To Next?

or

If you really want a loft Split the sphere face with the 3D Sketch and then Loft.


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Message 3 of 42
wolterh6
in reply to: wolterh6

Wow, now I feel really dumb. You did understand, but I thought those extruding methods could not adapt to surfaces 😛 

Your answer will be marked as solution.

Message 4 of 42
razortje777
in reply to: JDMather

Hello everyone, I am new here but I've got exactly the same question. But in my drawing I need to make a loft between a 2D and a 3D sketch.

 

Unfortunately the topic starter solved his (same) problem at another way but in my example that's not possible.

(the previous answer that you can manage this with the option 'split' was not really clear for me...)

 

I am looking forward for your answers.

(I hope it is not a problem, that I put my question in his topic, but I thought it was ok cause of the relevance..)

 

Problem_with_loft_3Dsketch_to_2Dsketch.png

 

Message 5 of 42
JDMather
in reply to: razortje777

You would probably be better off using the 3D sketch to split the face and use that in your loft.

Find the red End of Part marker at the bottom of the browser.
Drag the red EOP to the top of the browser hiding all features.

Save the file with the EOP in a rolled up state.

Attach the file here.


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Message 6 of 42
razortje777
in reply to: JDMather

Thank you for your answer.

I don't understand yet the solution with the Split function, but I try to search it again on the internet.

 

I prefer not to publish my part on the internet yet, besides it is very big (14mb).

But in the beginning of this topic is a perfect example with an 'egg' ( Test case.ipt 212 KB )

When it will work there, then I guess it will work too with my drawing.

 

Hope you can explain it too with the 'egg example' to me.

 

 

 

Message 7 of 42
JDMather
in reply to: razortje777


@razortje777 wrote:

I prefer not to publish my part on the internet yet, besides it is very big (14mb).

 


Looking at your picture - I could make up a simple example concerning only the loft.   (looks like engine cylinder ports)

You should be able to attach a simplified example that exhibits all the behavior of your desired feature.

In the process of creating the example - you might even figure it out yourself.

 

You are going to need some guide rails or centerline curves and your profiles will work best if you have the same number of entitites in each.  For example a filleted rectangular profile has 8 enitities - the 4 lines and 4 fillets.


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Message 8 of 42
razortje777
in reply to: JDMather

I have got allready some rails (made unvisible in the drawing...), and it works fine when I connect the area at the bottom with the green area inside the cylinder.

But now I want something to connect with a 3D sketch area (yellow aera).

 

So that's the whole issue I think, because adding rails will work I hope. But for now... I only need to connect those 2 area's but Inventor will not allow that.

 

I have watched dozens of tutorials in youtube, but all of those have 2 straight 2D-sketches... none of them uses a 3D sketch area.

 

Meanwhile, I will try to simplify my drawing an upload it.

 

Thanks for the help allready! I appreciate that!!

Message 9 of 42
wolterh6
in reply to: razortje777

I don't know if this is the correct approach - and if it isn't, I hope I get corrected - but lofting between a 3D sketch and a 2D sketch has always been impossible for me, I work it around my making another 3D sketch on the same plane as the 2D sketch which is simply a projection of all the curves that matter in the 2D sketch to the plane. In other words, is like converting a 2D sketch into a 3D sketch.

 

Then I loft and it works fine. 

Message 10 of 42
razortje777
in reply to: wolterh6

I have tried it your way but I then I discover several problems. How do you deal with those?

 

1) I can not copy every 2D Sketch with a 3D Sketch because you only have 3 drawingtools: arc, line and spline. I can't draw a circle with it

2) How let I follow a 2D-curve with a 3D-curve? How can you make them exactly the same?

3) Even if I have two 3D-sketch area's... it still says an error that it is not possible to connect those two..

 

Isn't it possible to copy in someway a 2D sketch to a 3D sketch? If yes, then I have solved problem 1 + 2...

 

Thank you for sharing your option, but I hope there is, in someway, a better solution possible with Inventor 2012...

Message 11 of 42
JDMather
in reply to: razortje777


@razortje777 wrote:

 

Isn't it possible to copy in someway a 2D sketch to a 3D sketch? If yes, then I have solved problem 1 + 2...

 


 

Include Geometry command in 3D sketch (think of it as roughly the equivalent of Project Geometry in 2D sketch).

 

Not sure this is your best solution though.  Post the stripped example.

 

Port.png


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Message 12 of 42
wolterh6
in reply to: JDMather

Indeed, I forgot to mention how to project the curves 🙂 The post above describes what I was thinking.

Message 13 of 42
razortje777
in reply to: wolterh6

Thank you for your answers!


 

This is indeed the solution because with two 3D Sketches you can make a loft between it.

But... this option works fine with the 'egg example' but for some reason it doesn't work by my cylinder... it keep saying an error....

 

I hope I can solve this last piece too because I really near to the solution 🙂

 

here it works.png

 

faillure_1.png

This is indeed the solution because with two 3D Sketches you can make a loft between it.

But... this option works fine with the 'egg example' but for some reason it doesn't work by my cylinder... it keep saying an error....

 

I hope I can solve this last piece too because I really near to the solution 🙂

Message 14 of 42
razortje777
in reply to: wolterh6

and here is the other picture, where it doens't work...faillure_1.png

Message 15 of 42
JDMather
in reply to: razortje777

I don't think you even need the 3D sketches.
Split the face.

Attach example file here.


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Message 16 of 42
razortje777
in reply to: wolterh6

Actually I've discovered inventor is really complicated and a lot basics I do not really know. So lot of basics I don't know and that's why this drawing is a big mess and should not be as it should be.

But last time I used Inventor was 4 years a go (I drawed a Bugatti Veyron engine, well some parts of it...)

For example, I don't know how to use the Split face and lots of other basic tools.


For now, I have tried to upload the file because I have not other option and the errors made me a bit desperatelly.
But it is 15mb, and I can't make it any smaller... well I don't know how../
Hope someone could help me.

Message 17 of 42
JDMather
in reply to: razortje777

See response #5.

In addition to rolling up the EOP, after saving in a rolled up state right click on the filename in Windows Explorer and select Send to Compressed (zipped) Folder.  Attach the resulting *.zip file here.

 

Looks like it would be pretty simple to create an example file.
Just a cylinder and a couple of sketches.  Don't need all the stuff out of the image frame.


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Message 18 of 42
ipi
Advocate
in reply to: JDMather

Let me jump into the fray:

 

I am having the same issue in that I cannot loft between a 3D sketch and a 2D sketch.  As was suggested, I created a 3D sketch and the included the geometry from the 2D sketch, but I still cannot crate the loft.

 

Please see the attached file.

David Hassan

IP Illustration
www.ipillustration.com
Message 19 of 42
JDMather
in reply to: ipi

Your 3DSketch1 is not symmetrical?
What are you trying to make?

Maybe a trim would be a better solution.
Why not have the origin at the center of this object?

How did you create the 3D spline - did you type in the points or import Excel points?


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Message 20 of 42
ipi
Advocate
in reply to: JDMather

Please refer to the 2 images I have attached for a visual explanation of what I am trying to accomplish.  Essentially, it is a cone whose small end begins to curve inwards and is wavy.

 

To create this shape in Inventor, I first drew the the profile of the 2 curves in AutoCAD and then arrayed them (see capture 2). Then, in Inventor, I created a 3D sketch and imported the DWG (attached) into the 3D sketch and used the endpoints to create a closed 3D spline.  I then created a 2D sketch to draw the circle that represents the end of the loft.

 

There is no good reason why the origin is not in the center of the array.

 

Many thanks in advance for your input.

David Hassan

IP Illustration
www.ipillustration.com

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