Any idea why Inventor is not resolving this sweep with a defined curve?

[chris]

Inventor 2023 doesn't seem to be able to resolve this sweep with an included curve past 180º, if it was created at an angle less than 180º, Also, within a sweep being defined by 3D Sketch, it seems to work when using a slider to define the angle, but it doesn't work when the dimension is hand typed to a direct number, (180º)

See Video

[Scott_Parker]

Inventor 2d sketch tries to maintain the "Chirality" in the sketch.  So if geometry is constrained to a line and lies on one side of the line it will try and keep that geometry on that side.  In this case the arc is constrained to the line.  It lies above the line.  It will solve to maintain the chirality and keep the arc above the line.

[chris]

@Scott_Parker   Major design drawback... that ability or lack of, limits the design process and in my case, it limits me from creating a template that allows for the option of 4 different designs in one file to have to create 4 files. That's not the only shortcoming, it also causes issues with trying to use the array to a path command.

IMO, this is something that needs to be fixed or at a minimum allow the user to define for themselves. Letting us define the curve by the curve length would solve the 3 limitations that IV2023 is causing on my current design. The simplicity of this handrail design should have only taken me a few hours to model and configure, but because every "work-around" I try to get around IV's limited capabilities in this one area, I've been on this design for over 5 days now.

I'm not a new user, I've been using Inventor since R4, I know the design I want to make, but IV is not allowing it, instead, it's forcing me to manage 4 template files instead of allowing me to make one, well maybe 3.

btw, same thing happens in Solidworks, so don't feel bad Autodesk

[pcrawley]

If you're looking for a workaround that isn't quite so involved, try creating the sweep path from your construction geometry, then using a fillet to build the appropriate curve between the two line segments.

It works using slider-driven values and typed values.  You might notice the fillet fails at 180 - and that's expected because a fillet between two colinear lines would be meaningless.  You can use conditional suppression of the fillet if it troubles you:

 

[chris]

@pcrawley Yep, already tried that... well yours looks different... are you creating the fillet with a surface? I tried to open your part but it only opened a derived version, was yours created in IV2024? Can you show your example of a conditional suppression at the 180's

[pcrawley]

Two lines constrained with an angular dimension (later driven using the iLogic slider).  Extruded as a surface:

Fillet the two surfaces - adding the conditional suppression by right-click > Properties on the Fillet feature:

Create the sweep path using "Project Cut Edges" and it creates the sweep path through the filleted surface:

Add a workplane on the moving end of the path, sketch the sweep profile, sweep, done!

It's not 100% bullet-proof if you are too quick with the slider increasing the angle beyond 180°.  But you go back and drag the slider more slowly, it rebuilds itself nicely.

Sorry I can't post a 2023 version.  If only there was a SaveAs previous version... 🤤

[chris]

@pcrawley thanks! Testing now, I totally forgot that the feature had those properties, thank you for the reminder (duh)

[pcrawley]

I'd normally do the suppression with a line of iLogic because it's quicker to set up (and change) multiple suppression conditions.  In this case though, only 180° causes the problem.

If Angle = 180 Then Feature.IsActive("Fillet1") = False 

 or (you may have already found this) - this shortened version of creating the boolean appears to be more reliable and faster to solve (or it's just my imagination!)  It' is less typing 😉

Feature.IsActive("Fillet1") = (Angle <> 180)  

[chris]

@pcrawley Okay, even when I try your method of creating the radius between the planes the result is the same when the angles are set to 180º... they break. The reason for this, I believe, is that I'm projecting the edges of the 3 planes and two radii, so even though the properties of the radius are suppressed at 180º, it also means it suppresses the projected surface edges, which is what is driving the sweep profile for the tubing. (see video)

 

[pcrawley]

Does a "Rebuild All" fix it?

If so, add the following two lines to your iLogic code:

RuleParametersOutput()
InventorVb.DocumentUpdate()

[chris]

@pcrawley No, rebuild-all does not yield any results, just an error message about not being able to resolve the projected curves...? 

[pcrawley]

I've modelled something similar - I see your problem...

I'll let you if I find a solution!

[pcrawley · Accepted solution]

The problem with the model is that the 3d sketch.  It can't handle having segments deleted.  As soon as you hit 180, the arc in the 3d sketch fails because it is a point of nothing - and once failed, it stays failed.

My 'cheat' is to create a 2d sketch to form the top rail (red feature) - then two 2d Sketches to create the ends (yellow features).  Hope it makes sense from the pictures:

 

(I do still break it by dragging the slider too fast.  Time for a faster computer!)

Someone is bound to have a more elegant solution!

(2024 model attached)