Resolve "Warning: Detect some position features may result downstream features fail after restructure."

[Doubletop_]

In another post I have been made aware of RULE #1 so thought now is the time to tidy things up a bit. I've learned that once a component has been created the associated sketches  can be dragged from the top level folders to the component folder.  That includes the initial sketch and any created having missed activating the component.

That is sometimes, other times  I get the "Warning: Detect some position features may result downstream features fail after restructure."  I've looked here to see what is required to resolve this and can't find any definitive answer.

By way of an example the attached file creates a series of bushes, no relationship whatsoever with each other. Some of the bushes I've managaged to shift the associated sketches and other I get the "Warning: Detect some position features may result downstream features fail after restructure." and the sketches refuse to be moved.

I had the problem with the "general bush" so deleted all its files and started again. Three simple sketches. First sketch in the top level folder, extrude "make component" activate, second sketch and extrude, third sketch and a hole. Drag the initial sketch to the component and the "Warning: Detect some position features may result downstream features fail after restructure." message. (BTW I have the first sketch tied to the zero datum, the problem occurs with or without doing this.)

It doesn't seem to be related to the order of creation either. The Wet Header bush was done first (error),  Turret, Top Feed, Dome, (No error), Safety (error), General (error), and so on.

Why is this? 

What is required to fix it when it occurs?

What is required to avoid it happening?

Thanks in advance

Pete

[etfrench]

Change the order of your operations.

1. Create new component.
2. Make the new component's origin visible.  (Hide the main origin first if it's visible.)
3. Create sketch on one of the components origin planes. 
4. Create geometry on the origin, not out in space.
5. Extrude.
6. Use a joint to position the component to another component.

If you're making a library of parts, either make each an individual file or make each a component following the above steps.

To create these bushes you only need one sketch per bush.

[etfrench]

p.s. The above only answers the third question 🙂

[davebYYPCU]

First Component in the file.  Would likely be like this, Origin is sensible, one sketch, because the rear extrusion is from object.  Bolt holes are blind so the joint face is in the right place now.

You came across Rule 1 fairly late.

You are not using the Origin for Symmetry, then the object is made with 2 sketches but not on the same plane and material both sides of the origin.

So at the time you make the second extrude - join , you have set it for New Component.  The 2 sketches made on the back face will drag into the component, but the sketches before the second extrude are not dragging for me.

Make each component on the document origin in a sensible location of the part, for later Joint snap points to work nice and let Fusion do most of the work.

Hide each component when built, before making the next one.

Might help....

[HughesTooling]

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@etfrench wrote:

Change the order of your operations.

1. Create new component.
2. Make the new component's origin visible.  (Hide the main origin first if it's visible.)
3. Create sketch on one of the components origin planes. 
4. Create geometry on the origin, not out in space.
5. Extrude.
6. Use a joint to position the component to another component.

If you're making a library of parts, either make each an individual file or make each a component following the above steps.

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Add to the above.

You can also create a joint between a component origin and a feature on another part if you need references you can only get with the component in place.

Mark

[Doubletop_]

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@etfrench wrote:

Change the order of your operations.

1. Create new component.
2. Make the new component's origin visible.  (Hide the main origin first if it's visible.)
3. Create sketch on one of the components origin planes. 
4. Create geometry on the origin, not out in space.
5. Extrude.
6. Use a joint to position the component to another component.

If you're making a library of parts, either make each an individual file or make each a component following the above steps.

To create these bushes you only need one sketch per bush.

---

Thanks, espectally for the tip about one sketch, I'd wondered why it couldn't be done this way and had developed the habit of layering up sketches. Now I realise that was purely because the sketch is made not visible after the first extrude.

This definately works

1. Create new component.
2. Make the new component's origin visible.  (Hide the main origin first if it's visible.)
3. Create sketch on one of the components origin planes. 
4. Create geometry on the origin, not out in space.
5. Extrude.

will mean the sketch is held in the component folder

Whereas

1. Create sketch at main origin
2. Extrude
3. Make Component from Body
4. Do futher extrudes

Does not allow the sketch to be subsequently moved to the component folder and gets the "Warning: Detect some position features may result downstream features fail after restructure".

However, this is not consistent as I have managed to move the sketches for some components. In fact, in my multi sketch components moving the first sketch results in all the related sketches being moved. 

I tested this using your example on a completely new drawing and only the one simple component. To rigidly have to follow the step of creating the component first to circumvent the message and the problem being inconsistent. Is this a bug? 

.

[etfrench]

Once you make a component out of a body, you won't be able to move the related sketches.  

If you extrude a body, then create a new component, you can move the sketch used to extrude the body to the new component and the body will follow to the component.

[Doubletop_]

I've done some tests and have come to the conclusion that the problem is resolved by Rule #1. Creating components from bodies is to be avoided. The problem isn't helped by the default extrude being "New Body" so easy to miss and there's no way to recover.

The tests. For test 1-4 a new drawing for each test to ensure nothing else created the problem

Test #1

1. Create component
2. Draw sketch
3. Extrude #1 & #2
4. Create hole

Sketch created in component file

Test #2

1. Draw sketch
2. Extrude #1 and create component
3. Extrude #2
4. Create hole

Sketch can be moved to component file

Test #3

1. Draw Sketch
2. Extrude #1 and create Body
3. Convert Body to Component
4. Extrude #2
5. Create hole

Move sketch into Component folder gives “Warning: Illegal restructure. It will cause bad dependency.”

Test #4

1. Draw Sketch
2. Extrude #1 and create Body
3. Extrude #2
4. Create hole
5. Convert Body to Component

Move sketch into Component folder gives “Warning: Illegal restructure. It will cause bad dependency.”

Test #5

Tests 1,2,3,1,2 and 4 in one file the same results were experienced

Test #5

Tests 1,2,3,1,2 and 4 in one file. This shows why some of of the components in  my example could have the sketches moved into the component folders and others not. Once you've gone past the creation of a new body in the extrude there is no way back as the create component oprtion is removed. Not very fail safe really and easy to screw up

I'm also guessing that the message "Warning: Detect some position features may result downstream features fail after restructure." I'm getting is a result of some other misdemeanour of mine which is shrouding the “Warning: Illegal restructure. It will cause bad dependency.” message.

Pete

@etfrench @HughesTooling @davebYYPCU 

[Doubletop_]

.... and of course none of this answers the question what does "Warning: Detect some position features may result downstream features fail after restructure." relate to? and How can the problem be resolved?

Fixing of the problem of Body's converted to components and the component not accepting its original sketch. is a completely seperate issue Is it a bug?

[Doubletop_]

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@etfrench wrote:

Once you make a component out of a body, you won't be able to move the related sketches.  

If you extrude a body, then create a new component, you can move the sketch used to extrude the body to the new component and the body will follow to the component.

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Isn't that what my test #3 did and I got the “Warning: Illegal restructure. It will cause bad dependency.” message?

[davebYYPCU]

Don't be reading too much into this warning 

 "Warning: Detect some position features may result downstream features fail after restructure."

It says may - and if you get yellow icons down the line, a quick edit will normally fix it, so not a bug, just a warning.  When you understand Fusion, edits early in the timeline then displayed warnings will be inevitable, (because of the edit) but so is the fix.  Edit Feature and reselect the problem bits.  Design and problem dependent, can't cover all examples with general statements.

Only the author knows - if I do this - then - that will break, so fixing it will be needed,

(I'm Ok with that cause I know why)

Might help....

[TrippyLighting]

In essence, restructuring objects in the browser only works under specific circumstances.

In many cases, it would theoretically be possible, but the code to allow it has not been developed yet, and Fusion 360  limits what is possible.

I find that unfortunate.

This is one of the core modeling areas I would value more development as opposed to say rather costly manufacturing extensions.

[Doubletop_ · Accepted solution]

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@davebYYPCU wrote:

Don't be reading too much into this warning 

 "Warning: Detect some position features may result downstream features fail after restructure."

It says may - and if you get yellow icons down the line, a quick edit will normally fix it, so not a bug, just a warning.  When you understand Fusion, edits early in the timeline then displayed warnings will be inevitable, (because of the edit) but so is the fix.  Edit Feature and reselect the problem bits.  Design and problem dependent, can't cover all examples with general statements.

Only the author knows - if I do this - then - that will break, so fixing it will be needed,

(I'm Ok with that cause I know why)

Might help....

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I'm coming to the same conclusion; it is the way of IT applications. You never get the coder to write the test spec. Over time users gain expertise and a way of working that avoids the pitfalls. The beginner, like me, has to fall into these traps as part of the learning process. They either find their way through the minefield and develop their own expertise or walk away disillusioned. RULE #1 and #2 help, if you know that they exist.

So where do we find RULE #3,#4 ...... etc?

Thanks for your help guys, I'll close this one out

Pete

@davebYYPCU @TrippyLighting @etfrench @HughesTooling