I didn't design the autodesk way. How do I unscrew this?

[i-make-robots]

I designed a few parts in a project (set A); moved them into position in an assembly; designed a few more parts *in that assembly* (set B); then tried to tweak dimensions of the original parts.

The new part sketches did NOT update correctly, and the components depending on those sketches are bonkers.

Save Copy As... doesn't import the sketch on which the set B parts are built, so I can't modify them.

Pictured here the black servo controls the parallelogram motion of the grey nozzle.  The blue component was modelled in place.  When I adjust the arms of the parallelogram the blue component breaks.

How was I supposed to do this?

[jeff_strater]

Hi @i-make-robots, can you share your design?  It will be a big help in figuring out what the problem might be.

One question:  You mention Save Copy As.  Did you Save Copy As of the parts in set B, then reference it as an external component back in your original design?  Or is the entire design in one Fusion design?

Thanks,

Jeff Strater (Fusion development)

[i-make-robots]

I used Save Copy As and then tried to edit the copy, but no sketch was
available in the copied part.

The problem part is a component in the assembly sketch.

http://a360.co/1OhTXfL


--
Dan Royer :: Marginally Clever::Raising Robot Literacy :: +1.604.916.2281

[jeff_strater]

Thanks for posting the design.

Next question:  What edit are you making to which parameter, and what is the desired outcome?  I tracked down the length of one arm to an edit in Sketch2 of parameter d40, an the other to editing parameter d47 in Sketch4.  Are those the dimensions that you are editing?  What values are you choosing, and what is the expected outcome?

Thanks,

Jeff

[daniel_lyall]

one big thing the parts are not components, I am going to have a play and see if I can make the parts into components.

if you do all your Models as components it save a lot of problems down the line, something just work better if you use components.

[i-make-robots]

d40 and d47 are the two values I am trying to change.
I am trying to make them 24mm.
Sketch 10 is the one that doesn't respond well.

--
Dan Royer :: Marginally Clever::Raising Robot Literacy :: +1.604.916.2281

[i-make-robots]

@daniel_lyall That's how I would have done it in SW because SW is funny
like that.
I can see how moving one of the dimensions at a time would be wacky, but
once both are changed (or by changing both at once) it should understand.
Eh, the relationship node graph must be insane.

--
Dan Royer :: Marginally Clever::Raising Robot Literacy :: +1.604.916.2281

[daniel_lyall]

I had a look some of you sketches they have become disconected from there body's sketch 7, sketch2 and 1.

all your imported models where easy to fix.

[daniel_lyall]

the reason they are going na na it's projected geometry changing sketch demented 47, effects other bits,  it is something that happens with projected geometry. well that's what it look's like to me I have had the same problems before.

you could try re drawing the sketch and delete the projected geometry from the last projection to the first, this works sometimes I am going to play some more my self to see if I am correct or not, if I am wrong Jeff will say, what one good thing about this forum you will get told you are wrong and be given the correct info in a nice way.

[daniel_lyall]

the blue part is the problem it was the fillet's I had to delete what you will see in the pick. 40 seem ok now 47 some times. 

 http://a360.co/1O5MxR5

[jeff_strater]

Thanks, @daniel_lyall, for looking into and fixing this model.  I had a look at the original, and found some problems, but have not completely worked them out.  I think the root of the problem is that, in that blue component ("little finger parallelogram"), there are several overlapping geometries.  In the picture below, there are 3 circles over top of each other in sketch10.

One of them is the projected edge of the other part.  There may be two projected edges.  Now, this, of course, should be OK - they are constrained to be concentric, as near as I can tell.

But, when I change d47 to 24 mm, it updates like this:

You can see that one of these circles has not updated correctly.  I need to look further into why this is.  It's clearly a Fusion problem.

I was able to get your design to work better to delete some of the duplicate geometry, but there are other problems.  Some of these may be that this sketch does not have enough constraints to hold it in place on update of the other component.

That's all I had time for today, unfortunately.  I'll try to get back to it tomorrow.  Let me know if either of you makes more progress.

Jeff

[daniel_lyall]

Hi @jeff_strater I worked throw the drawing deleting the wrong way, sketch 11 and  the 2 fillets keeped being the fail point. I keeped doing this to I got to sketch 11 I was undoing as I went.

I deleted the 2 fillets and worked from sketch 11 forward editing the sketch removing the double and triple sketche's so all that was left was the non projected sketch, and if there was only a projected sketches I removed them if they where a line or circle, the sketch fillets seem to be OK if they where projected.

the last thing I did was re organise the time line so a sketch was with it's press pull and fillet, A lot of stuff was out of order. 

you are very correct about the constraints and most driven demeans where bad, some still are sketch 47 will fail then you undo and redo the change and it will work, 40 was fine 

it was a combination of 2 many double and triple projections with new sketche's as well, projections in the wrong place and a re projection to other spots have a look at sketch 2 and 12 and sketch 1 and 4. sketch 13 and 16 are fine. 

so there is a couple of bug's in the sketch what made sketch demented 47 fail, the two fillets with sketch 11 are bad and sketch 11.

It was a good exercise for the mind working my way through the sketch, it helps me in the long run.

[jeff_strater]

OK, I spent some more time with this today.

There are multiple ways to do this type of design, and I think eventually you will find a path that works for you.

I focused again on Sketch10, because I think that at least some of the problems are revealed there.

Some of the problem is that your sketch is not very well tuned to accept updates such as you gave it by lengthening the lifter finger or lifter finger assistant.  Some of this, unfortunately, does kind of require a sense of how the tool works.  For instance, the way that projected edge geometry works.  When a sketch updates, the first thing that it does it to update the projections, and then it updates the rest of the geometry that may reference that geometry.  Second, you will need dimensions to control the distances to the references so that your sketch updates in a predictable way.

For instance, just taking one example.  In this design, if I start just looking at sketch10, this is the starting point:

if I update d40 to 24 mm, the following happens:

I assumed that you really wanted this sketch to update.  So, I looked at the sketch, and the cause was that the circles here were not projected edges.  So I edited the sketch, deleted the circles, projected edges and completed the circle.  

Then, I can edit d40 to 24, and I then get this:

So, we are closer, but as you can see, we still have problems, because, while the circles now update correctly, the rest of the sketch does not.  So, I undid the parameter edit, and went back in to make some more changes:

I had to hook the vertical lines to be coincident to the points on the circle, and add some dimensions.  Now, I get much better behavior on that side of the sketch

Now, however, I looked at the other side.  Here we have a problem.  This side does use projected geometry, both to "lift finger assistant" and "Rotation mount".  So, when I update d47 to 24mm, I get this:

Mostly, it updates as I expect.  That one circle puzzles me, and may be a Fusion bug.  But, the main problem here is that this sketch references geometry from the "Rotation mount" component, which does not move when d47 is edited.  So, now, the geometry of the component being built from sketch10 is going to be a bit wonky.

This is where there are a variety of design approaches that could be applied.  If you can get the geometry in "Rotation mount" to move with d47, then this approach can work.  Or, you can build components in a different order.  The idea here would be to build the "lift finger" and "lift finger assistant" components, then this component (I think it becomes "lift finger parallelogram"), and then build "Rotation mount" from that geometry, by projecting edges from "lift finger parallelogram" into "Rotation mount", so that you have a chain of dependency that works well together and tolerates updates.  All of these are kind of "top/down, model in place" approaches.

Or, you can use a different approach entirely, and create components not in place, relate them with joints, and use Combine to do things like cut out the notch in the "lift finger parallelogram" where "Rotation mount" fits in.

Anyway, the net takeway is that some of this takes time and experimentation to get right, and a bit of planning.

So, good luck with your designs!

Jeff