Unable to extrude blue sketch

[davidK82P7]

I am making a microSD card holder for myself in Fusion 360.

I downloaded an STL model of a microSD card, imported it into F360 as a mesh object, scaled it appropriately, and converted it to a solid. Then, I projected the solid onto a new sketch plane, without the "linking" option.

There were a couple missing lines around the projected sketch, but I added lines to close it off. When I double click on any line in the sketch, the entire outline is selected, so it does infact appear to be a closed sketch. Example:

I've read in other forum posts that the shape needs to be fully constrained - but how can I do that with such a complex shape? When I select the entire outline, it is a total of 148 objects - primarily because the round corners are not actually arcs - they are a bunch of small straight lines.

This is the model I downloaded and imported as a mesh:

https://grabcad.com/library/micro-sd-card

I've attached my F360 file in case anyone would like to take a look at it. But, all I'm really trying to do is project the outline of the microSD card model onto a plane, then extrude the outline of the card via the "cut" mechanism so I can create a microSD card shaped hole in the surface. Hopefully that makes sense.

Thanks!

David

[HughesTooling · Accepted solution]

The only reason the sketch in blue is because you have auto project on, personally I'd turn it off as it adds a lot of clutter to sketches.

As you can see with the other sketch hidden you get the outline of the face you've sketched on. As for your problem, the white dot is a giveaway for the problem, try dragging the point.

[jeff_strater · Accepted solution]

Sketches do not have to be fully constrained to have valid profiles.

The problem is in the lower left corner:

there are 5 sketch point stacked up here:

I deleted some of the small arcs to the bottom of this point and re-created them, and the result is OK

Also, don't pattern sketches.  You are much better off extruding and then patterning.  As it is now, this sketch takes a very long time to solve

[HughesTooling]

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@davidK82P7 wrote:

I downloaded an STL model of a microSD card, imported it into F360 as a mesh object, scaled it appropriately, and converted it to a solid. Then, I projected the solid onto a new sketch plane, without the "linking" option.

I've read in other forum posts that the shape needs to be fully constrained - but how can I do that with such a complex shape? When I select the entire outline, it is a total of 148 objects - primarily because the round corners are not actually arcs - they are a bunch of small straight lines.

Thanks!

David

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To answer the question about constraining, don't waste time with STL conversions. Just scale it to the correct size then create the sketch yourself by tracing over the mesh.  You could try creating mesh sections but doubt you'll save any time.

Mark

[davidK82P7]

Thank you!! I don't know how I didn't see the white dot, but that did it!

[davidK82P7]

Thank you! Great point about extruding first, then patterning. For this case though, I needed the sketches on the plane so I could get the length of the overall design just right. But, I will absolutely extrude first, then pattern the extrusion. 🙂