Sketches Driving Me Crazy....

[jagboy2013]

I'm relatively new to Fusion, but have used Solidworks for years, so familiar with the concepts.  I find sketching drives me crazy.  I am constantly creating sketches that appear correct to me, but won't do a cut or extrude.  I must be missing something, as I'm sure all the different colors that show up are telling me something, but I don't know what.  I typically Project features to get some sketch lines, and draw others.  My default assumption is projected lines are treated no different from sketched lines, but experience suggests perhaps this is not necessarily true.

I see lines and points change color from dark red to green to yellow to blue to black.  WTH does it all mean?  I understand blue is an unconstrained line, and black a constrained line, and projected features at least start out dark red, but what does it mean when they turn yellow or green?

If I have what appears to be a closed path in a sketch, but cannot select that area for a Push/Pull, HOW do I find the problem, other than just fumbling around in the dark until I hit on the right change?

Is this all documented somewhere?  This is my single biggest frustration with Fusion right now...

Regards,

Ray L.

[HughesTooling]

This thread has a few tips. Also make sure you have show profiles enabled in the sketch on the sketch palette.

Mark

[GrAndAG]

Green - line is fixed

Black - fully constrained

Blue - regular line

Orange dashed - construction line (it can't be used as profile contour)

Purple - projected line

Black dashed - projected line turned to construction

Yellow - warning (usually it's a projected line which lost its parent; so, cache is used)

May be it can be a red one - means error (again it's related to loosing relationship)

Also hollow (with white center) dots means unconnected ends. Connected dots are fully filled.

[TrippyLighting]

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@jagboy2013 wrote:

... used Solidworks for years, so familiar with the concepts.  ...

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Yes, maybe. I've not used SW in the last 5 years but before that I've worked with Solid Woks since 1998. I find that many users coming from other CAD systems try to use sketches the same way they are using them in their previous CAD system. In SW if you want to extrude something, your sketch profile must must reflect the outline of what you want to extrude. That results in trimming and a lot o other clean-up and cosmetic work inside the sketch

Fusion 360 allows you to select multiple segments from the sketch for extrusion and if they are adjacent, they form one solid body. While the sketch might look unorthodox and not what you might be used to, I've found that not having to do all this trimming etc. can save quite a bit of time.

On the other hand, the sketch engine in Fusion 360 needs some serious work so I can fully agree that sometimes it drives me crazy as well 😉

[jagboy2013]

That trick is definitely good to know, though it di me no good in this case.  However, I stumbled across the answer - it was a matter of what was visible, and what was being selected when I tried to select the paths for the extrude.  Though I could see the sketch, I also had another component enabled, and it appears the face of that other component was being selected, rather than the path I wanted.  I hid that component, and got the result I wanted.  Lesson learned: Probably best to turn off everything but the one sketch when making path selections for an extrude.

But, back to the rest of my questions:  What is the meaning of the white/green/yellow points and lines?  Magenta obviously indicates a projected line, blue a drawn line, and black a fully constrained line.  What about the rest?  An annoying thing, probably just a display resolution issue, when zoomed out, the points change colors!  Magenta points turn green when zoomed out.  Very misleading.

I have to say, overall I REALLY like Fusion much better than Solidworks!

Regards,

Ray L.

[jagboy2013]

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@GrAndAG wrote:

Green - line is fixed

Black - fully constrained

Blue - regular line

Orange dashed - construction line (it can't be used as profile contour)

Purple - projected line

Black dashed - projected line turned to construction

Yellow - warning (usually it's a projected line which lost its parent; so, cache is used)

May be it can be a red one - means error (again it's related to loosing relationship)

Also hollow (with white center) dots means unconnected ends. Connected dots are fully filled.

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Thanks.  That helps a lot.  I often see white points, and even if I make them coincident to other entities, they remain white.  If I try to add further constraints, I get warnings that the sketch is over-constrained, yet the points remain white.  What's going on there?

And how does a line get to be fixed?  I've never used the Fix option, yet I find projected lines turning green by themselves...

Regards,

Ray L.

[TrippyLighting]

This is a link to the Autodesk University handout Jeff State and I prepared for out Class at AU last year. It has a section called "What do all the colors mean". And lists most of the colors you find in the sketches.

As someone coming from solid works it would be a good idea for you to go through the entire  document 😉

[jagboy2013]

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@TrippyLighting wrote:

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@jagboy2013 wrote:

... used Solidworks for years, so familiar with the concepts.  ...

---

Yes, maybe. I've not used SW in the last 5 years but before that I've worked with Solid Woks since 1998. I find that many users coming from other CAD systems try to use sketches the same way they are using them in their previous CAD system. In SW if you want to extrude something, your sketch profile must must reflect the outline of what you want to extrude. That results in trimming and a lot o other clean-up and cosmetic work inside the sketch

Fusion 360 allows you to select multiple segments from the sketch for extrusion and if they are adjacent, they form one solid body. While the sketch might look unorthodox and not what you might be used to, I've found that not having to do all this trimming etc. can save quite a bit of time.

On the other hand, the sketch engine in Fusion 360 needs some serious work so I can fully agree that sometimes it drives me crazy as well 😉

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That difference I picked up on right away, and doesn't really cause me any problems.  And, that has the advantage that a single sketch can be used for multiple extrusions, which is nice.  You can't do that in Solidworks.

Some things I miss from Solidworks: The ability to copy sketches (quirky though that feature is in SW), and most especially the ability to re-order the timeline!  I find I often make changes to a part which breaks other features, and there appears to be no way to "repair" this, without re-creating those features from scratch.  Even worse, I have had sketches or extrusions which simply STOP working entirely, and CANNOT be fixed.  Even deleting all entities from the sketch and re-creating from scratch will not result in a good extrusion.  It became necessary to delete the sketch entirely (which deletes all down-stream features!), and recreate all from scratch.  This has hit me 2-3 times already.

Regards,

Ray L.

[jagboy2013]

Perfect!  Thank you!

Regards,

Ray L.

[TheCADWhisperer]

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@jagboy2013 wrote:

  And, that has the advantage that a single sketch can be used for multiple extrusions, which is nice.  You can't do that in Solidworks.

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Of course you can.  I do it every day.

[TheCADWhisperer]

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@TrippyLighting wrote:

 In SW if you want to extrude something, your sketch profile must must reflect the outline of what you want to extrude. That results in trimming and a lot o other clean-up and cosmetic work inside the sketch

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Don't need to trim up the sketch in SWx.

Simply use the Selected Contours.

[jagboy2013]

Only if you want to extrude the ENTIRE sketch, which is quite limiting...  With Fusion, I can create a single sketch, and extrude several DIFFERENT profiles with it.

Regards,

Ray L.

[TheCADWhisperer]

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@jagboy2013 wrote:

Only if you want to extrude the ENTIRE sketch, which is quite limiting...  With Fusion, I can create a single sketch, and extrude several DIFFERENT profiles with it.

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Wrong.  

In SolidWorks I can create a single sketch, and extrude several DIFFERENT profiles with it, just like Fusion, just like Inventor.

This isn't my first rodeo.

[kb9ydn]

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@TheCADWhisperer wrote:

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@jagboy2013 wrote:

Only if you want to extrude the ENTIRE sketch, which is quite limiting...  With Fusion, I can create a single sketch, and extrude several DIFFERENT profiles with it.

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Wrong.  

In SolidWorks I can create a single sketch, and extrude several DIFFERENT profiles with it, just like Fusion, just like Inventor.

This isn't my first rodeo.

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I feel like more recent version of SWX (in the last 5 years or so?) have gotten a little more flexible with this, especially around what you can do with open contours.  I haven't done a side by side comparison to older versions but it seems like it used to be more strict about making you use closed sketches for extrusions.  Either that or maybe it was just a lot more buggy or not as easy as it is now.

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