Strange behaviour - Faces are not parallel

[Anonymous]

I found a strange behaviour that i think might be a bug. 

While I was designing this part i found out that: 

- Two faces that should be perfectly parallel are not. (One of them, which should be collinear with another face, has instead an edge that should exist)

- While using the "Midplane" command on these two faces, the plane that is created is not in the middle. 

I don't know if these two odd things are related or not. Any advice? Did i make some mistakes in modelling the part? 

[TheCADWhisperer]

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@Anonymous wrote:

Did i make some mistakes in modelling the part? 

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Can you File>Export and then Attach the *.f3d file here that exhibits this behavior?

[Anonymous]

yeah sure

[TheCADWhisperer]

Are you working from a book drawing?

I would expect to see Tangencies in these locations, especially 1 and 2.

I would have modeled with symmetry about the Origin.  Now on to the rest of the problem...

[TheCADWhisperer]

Hmmm, well this is a strange one.

I will have to remodel from scratch anyhow - utilizing the BORN Technique.  Back in a bit.

[Anonymous]

No i'm just learning using Fusion and i'm working my way up some drawing exercises taken from a book (good eye!). 

You are right about the tangent constraints: if that was a real part they should be there, but the model i'm following has actually that shape.  Anyway, it's just an exercise..

[Anonymous]

What's the BORN technique, out of curiosity? 

I think I'd be able to remodel it myself to do it right, but i'm curious in why this is happening to avoid doing the same mistake in the future. 

Thanks! 

[TheCADWhisperer]

I have to leave for work, but for others to take a look I boiled it down a bit. (see attached)

[chrisplyler]

Just eyeballing that picture...they sure look tangent to me.

[Beyondforce]

Hey @francesco.buonamici ,

I hope this video will help:

Cheers / Ben
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[HughesTooling · Accepted solution]

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@TheCADWhisperer wrote:

I have to leave for work, but for others to take a look I boiled it down a bit. (see attached)

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The angle problem starts in the sketch. If you delete the vertical constraint, move the line end point then reapply the vertical constraint the angle error goes away. Just deleting and reapplying without moving the line endpoint doesn't fix the problem. I've seen these problems a few times in Fusion's sketches but they are not something that's repeatable. @jeff_strater  can you take a look?

Thanks Mark

[Anonymous]

Well, in the lateral view you can clearly see the edge, that is visible. Moreover, a diametral tangent line would be perfectly vertical. 

But that's not the problem anyway

[HughesTooling]

The picture above is from @TheCADWhisperer 's  file, in @Anonymous  original there are parallel constraints and the question is how did you get those? If I redraw Fusion create perpendicular constraints not parallel.

Here's a screencast demonstrating the error in the original file.

Mark

[TrippyLighting]

Here is a link to the paper that explains the BORN modeling technique.

What you are describing looks indeed like a problem with precision and I am wondering if it is the result of using projected geometry from a sketch.

Looking at your design, you make good use of constraints and your sketch is fully dimensioned and constrained. That's a good start.

Given that this part is symmetric across one axis I'd have located the sketch origin at the symmetry axis. That usually helps simplifying things and often eliminates the need to create auxiliary construction planes.

It is also generally a good practice to break more complicated geometry into several sketches, but in this case I would have put everything onto one sketch that is still pretty simple.

For the rib I do use projected geometry. However I am not intersecting faces, but select the body option in the UI as that is a a more stable reference than a face an edge or a point.

It does create more projected geometry though, which is not always welcomed.

Look at the the timeline:

[chrisplyler · Accepted solution]

Weird. I reproduced the same thing - although I only used one Sketch and four Extrudes - and my sides are parallel and produce a Midplane exactly in the center.

I am able to correct your part by editing your Sketch5 and replacing your geometry with a 3-point rectangle. Then of course I had to edit the Midplane and re-select the sides.

[Anonymous]

Thanks for the effort but this was not was I was asking. That model has a strange problem with the way two faces have been created. As I said in the previous message, the problem is that the two external faces (left and right - rectangular) are created with a small angle while they should be perfectly parallel, as the used sketch/feature combination imposed. 

This probably caused also some problems on the definition of a MIDPLANE between the faces, which results different from a midplane evaluated on other features. (Multiple central planes that you saw in my model were created to show the discrepancy). 

I get that there are multiple strategies (probably better ones) to achieve the same result, but it's not the main issue here. BTW, the base sketch is composed by lines that are not tangent. That IS the design intent. 

[Anonymous]

Thanks for all your answers. 

It seems clear that it was a bug that originated in a sketch due to an incorrect imposition of a vertical constraint on a line. Although the constraint was imposed, its effect was not correct. 

Thanks for all the modeling advices.