need help extruding from sketch
The layered lines seem to be confusing the fusion in terms of producing a profile. if you delete the shorter segments, or at least a few of them, the profile becomes available for extruding. This seems like a bug, but it's also not good modeling practice, so avoidable. you also might just delete the spine, as that also allows the profile to be available-
@Phil.E -what do you think? buggy?
In case your wondering about those phantom profiles, they are caused by this setting-
which projects the lines from faces you create sketches on, but keeps them invisible. but they are there, and they highlight when you mouse over them, and you can constrain geometry to them or delete them. you use to be able to break the link to them, and make them visible, but that behavior seems to have changed. (on second thought, this may be what causing the double line situation illustrated above, hmm)
I'm at a loss as to why someone at AD thought this was a good idea at all, and worse thinks it should be the default behavior. I highly suggest turning it off.
next, the spline with a kagillion control points is problematic. you always want to use as few points as possible, other wise you end up with curvature like this-
which is extremely bad. This curve could have been produced with probably 5 control points.
but i'm not really sure what the purpose of the curve is. it looks like you where trying to reproduce the edge of the face the sketch was on. if so it, would be better to just "project" the edges into the sketch.
@laughingcreek Yes technically a bug. Would you say it's fair to describe it as "splines drawn on top of existing sketch curves causing profile to not compute"?
Regarding the underlying default behavior. This case is a good example. The auto-projected face is intended to be used, at least judging by the attempt to manually draw the same shape.
For reference, here is the help section for "how to" in Sketch.
http://help.autodesk.com/view/fusion360/ENU/?guid=GUID-48A0A48C-CBC3-404E-9212-889DF4D776AE
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
To reduce the clutter. Needlessly placing visible lines that the customer doesn't care to see or use is avoided.
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
Glad to look at any cases where this causes trouble.
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
2 examples I've had to explain to new users where because there was this invisible line there you can't see that was causing the confusion-
Then there is this thread, where the OP didn't realize they were tracing over a line that was already there because they couldn't see it.
These forums are full of post from new users confused by behaviors that are a direct result of this functionality.
I'd be curious to know how many users, once they discover this setting, leave it turned on.
Auto Project has caused problems for years, from people projecting a face again so ending up with duplicates of everything to overloading the system when sketching on a face of something created from a imported svg\dxf. Can even be a problem sketching on a face of a gear with a lot of teeth. Always suggesting people turn it off and only a couple of times has anyone complained about manually project what they need.
Other solid modelers I've used seem to do this without projecting or if they are they do it's to a layer that's totally invisible. Might be nice to have an option in preferences to create as normal projected geometry and let people have a choice, or even create as construction lines.
Mark
Mark Hughes
Owner, Hughes Tooling
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Tracing the edge of a part is unnecessary and prone to error.
To avoid using auto projected profiles, use Sketch > Create> Project/Include > Project. Select the face and the edges of it will be projected into the sketch.
Using Fusion default settings, the workflow is as below. In this case, the auto projected profile provides what appears to be what is needed. Am I missing something about the shape you want, or does this show the desired result?
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
@Phil.E -Sorry, I just can't help it. just a few minutes ago you posted in a different thread a PDF on stable projections.
Got it. You are correct. After looking very closely at the model it's clear there are small mis-alignments where faces come together, all over the model. Unfortunately these are within the tolerances Fusion uses for manufacturable surfaces, meaning they cannot be ignored by the modeling kernel. Errors will happen when using geometry built this way, and features like sketch projections are also going to pass these mis-alignments onto the next feature.
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
@laughingcreek you mean this post:
https://forums.autodesk.com/t5/fusion-360-design-validate/avoidance-of-loss-of-projections-best-prac...
"Avoiding lost projections", advice for someone seeking to use stable reference sources in parametric design.
The image is a paragraph written by Jeff Strater from here: A sketch master class written by Jeff Strater for AU a couple years ago.. Page 47-56 is about stable sketch references.
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
@mark -sorry, we've hijacked your post to debate something your probably not interested in. anyway, back to regular programming-
@mark wrote:
> it looks like you where trying to reproduce the edge of the face the sketch was on.
Yes, the original edge was corrupt. I couldn't do anything with it. Any operation gave me an error.
I create broken models all the time. It comes from free-handing. I usually fix them by undoing to before the problem but it wasn't feasible in this case. (I consider broken models to be "bugs" of F360 but in other threads I have been told it is my fault).
It's hard to say what made that edge "corrupt". this model looks like it could have been split and half and reassembled (badly) at some point-
close up of 1, showing short non-tangent segments on the face. I don't know what operation you wanted to perform here, but this would cause filet (and other things) to fail-
close up of location 2, illustrating odd geometry, and the reason I suspect it was split and re-assembled-
As I was trying to duplicate an existing edge I thought the more the merrier.
When drawing splines, more is not the merrier. You end up with a wavy surface.
As a beginner I am assuming you mean to delete control points. Otherwise I don't know what deleting segments means. I clicked on dots and deleted many of them but no profile appeared. You showed a menu (with tabs of Objects and Parents if I remember correctly) with items circled and said to delete, but I don't know how to bring up that menu. I have seen that menu at seemingly random times and have tried to play with it but it never seems to do anything.
No I meant the segments that had been auto projected from the face (I originally thought you had drawn them). If you hold the left mouse button down, it will show a list of everything under the mouse pointer. you can then scroll through the list and pick the thing you want. Useful in a multitude of cases.
here it is showing that invisible projected line-
META: Not letting me see the thread while creating a reply is a major pita. I can't refer to users or things shown to me because I don't have perfect memory. The hint telling me to use @ is useless since the list it brings up does not help me figure out who to reference.
yes. agreed. My current workaround is to duplicate the tab first, so I can switch over to it for reference. not great, but something.
...Try to offset the thin face around the whole object. You will get error saying something about not being able to delete a fillet. There are no fillets...
there are some very small arc shaped faces that it is interpreting as fillets,
... I assume the edge is broken by slight misalignments caused by free-hand operations I performed in creating it. This happens often to me. I have been told in other threads I need to change how I work. I personally feel that this should not happen and is due to some bug(s) in F360.
yes, probably the free hand operations. I think it's less a matter of changing the way you work, and more a matter of understanding what is happening. Fusion isn't a free form modeler. It's an engineering tool that's used to create rather exacting geometry that you wouldn't be able to achieve in a free form way. That's one reason why it's less forgiving when things aren't exactly right. but you can still do things in a free form way, but you would need a deep understanding of the ramifications of the resulting geometry to be particularly successful.
That said,I would still suggest changing your approach. You can achieve so much more, so much faster, once you drink the cool-aid and model in a way that keeps fusion happy.
what operation is it you where wanting to perform on the edge of that part?
