Solid loft that I cannot get to solve between the sketch and the end of the solid

Solid loft that I cannot get to solve between the sketch and the end of the solid

jagSJMV8
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Message 1 of 14

Solid loft that I cannot get to solve between the sketch and the end of the solid

jagSJMV8
Enthusiast
Enthusiast

I have a similar problem with a solid loft that I cannot get to solve between the scetch and the end of the solid.

Why can I not just click the end of the solid and the outer circle of the scetch?

3Y v3.png

 

@jagSJMV8 A new thread was created and the title modified for this post to increase findability. Original: Loft not possible?  CGBenner

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Accepted solutions (3)
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Replies (13)
Message 2 of 14

TheCADWhisperer
Consultant
Consultant

@jagSJMV8 

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

 

No islands in Loft.

Shell.

Undefined geometry should keep you awake at night.

 

TheCADWhisperer_0-1753804759421.png

 

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Message 3 of 14

johnsonshiue
Community Manager
Community Manager

Hi! I believe you will need to do it in two steps. First, create the Loft for the outer profiles. Next, create a Loft Cut using inner profiles.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
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Message 4 of 14

jagSJMV8
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Enthusiast

Sorry  - I thought I had exported it.

I have tried with shell extrude and thickening but it does not solve the geometry

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Message 5 of 14

TheCADWhisperer
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Consultant

@jagSJMV8 

 

Start a new part file.

Start a new sketch on the top plane.

Sketch a Construction Circle as shown below...

TheCADWhisperer_0-1753811997795.png

Now sketch a Vertical Construction Line to the left of the Origin as shown below...

TheCADWhisperer_1-1753812049806.png

Now add a Midpoint Constraint between the vertical line and the Origin...

TheCADWhisperer_2-1753812149577.png

Now add a 36mm dimension to the Vertical Line.

What do you observe about the color of the sketch geometry after adding the dimension?

TheCADWhisperer_3-1753812278829.png

TheCADWhisperer_0-1753814800810.png

 

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Message 6 of 14

jagSJMV8
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Enthusiast

Initially I have an orange dottet circle and a black vertical one

After pressing the coincident contraint I get black/black as you show - I have tried to do both a solid and surface extrude to it but cannot do the solid and surface only to the solid circle. I can surface extrude to inner and outer circle but not the solid - i include updated file3Y v4.png

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Message 7 of 14

jagSJMV8
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Accepted solution

After this I applied a patch which have solved the issue, but I don't know why the solid loft does not work. I can finish it with surfaces, but I would like to know what I am misunderstanding or doing wrong.

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Message 8 of 14

davebYYPCU
Consultant
Consultant

Using all of the last 2 sketches, solid Loft, as New Body.

Shell this new body 0.50 wall thickness.

Combine Join the two bodies.

 

Might help...

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Message 9 of 14

jagSJMV8
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Enthusiast

Thanks Dave, 

This method gives edges on the ID of protrution that does not get solved - I had similar results by edge shell and 0.5 thickness. What resolves right is to have two shell extrudes - ID and OD and then fill the space with a patch. I think I just have to accept that I don't understand why the solid does not work. 

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Message 10 of 14

davebYYPCU
Consultant
Consultant

What part of my file Loft - did not work?

 

toldb1.PNG

 

I did not continue with your double surface lofts (deleted) was far more work, to then Patch both ends, and Stitch to Solid, before Combining the new body.

 

Might help...

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Message 11 of 14

TheCADWhisperer
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Consultant
Accepted solution

@jagSJMV8 wrote:

Initially I have an orange dottet circle and a black vertical one


@jagSJMV8 

You should always fully define your sketch geometry such that it turns black and shows lock symbols in browser.

TheCADWhisperer_0-1753876039043.png

 

 

I think I just have to accept that I don't understand why the solid does not work. 

 

See Attached file.

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Message 12 of 14

jagSJMV8
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Enthusiast

Hi Dave, 

The wall of the side tubes comes in at 45 degree which means that if the section analysis is done from the top it does not fit as the wall due to the angle is about 0.7 thick if projected on the XY plane but 0.5 on the other two planes

3Y v4db2.png

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Message 13 of 14

TheCADWhisperer
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Consultant
Accepted solution

Shell (at right time in history) returns consistent wall thickness.

TheCADWhisperer_0-1753878028802.png

 

If you want the tapered ends to be shelled too - change the history.

Message 14 of 14

johnsonshiue
Community Manager
Community Manager

Hi! There are multiple ways to do this. Here is a more compact design with a ball joint at the intersection. However, the pressure profile would be totally different than the original design .CFD Analysis is highly recommended.

 

johnsonshiue_0-1753894613414.png

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
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