I have a sketch that would "have" more than one open outline, but I can't find it. I tried with the check sketch tool for the use of the function but it can't find it either... Is there another trick? (Solidworks 2012)
Thank you ;-)
Hi @ Sunn
Open your sketch and zoom in to see if all the points are coincident
you must have one (or more) missing segment in one place or another
post your file that we look at
Your completely constrained sketch must be black if you have laid all your sides
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Okay with gt22 you must have two right ends or other not connected.
Hello
I use the "selection of a channel" to find...
Right-click on a segment and then "select channel". Where auto-selection is interrupted is a bad coincidence.
Then just repeat until the selection is done entirely.
Good night...
3 Likes
Hello
It may be due to an extra segment in your sketch, a quick click can create a tiny segment that will generate this message (see image)!
So you have to find this end of the segment or use the outline selection to work in the interesting area
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esquisse.png
Hello
You can use the tool found in:
tools--> sketching tools --> repair the sketch.
This tool indicates where there are problems.
Kind regards.
I had checked my sketch, it forms a complete chain. In fact it's a bug in SolidWorks...
It's a rather complex sketch (aluminum profile), where I use differently oriented blocks. When I burst the blocks, he wants to do the extrusion. What is unfortunate is that it overloads and complicates the sketch even more.
Hello
It also happens that by modifying the "intervals less than", using the 2 arrows, we find an error that had escaped us.
In any case, good luck because sometimes, it's a bit complicated for not much!
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I had checked my sketch, it forms a complete chain. In fact it's a bug in SolidWorks...
It's a rather complex sketch (aluminum profile), where I use differently oriented blocks. When I burst the blocks, he wants to do the extrusion. What is unfortunate is that it overloads and complicates the sketch even more.
I don't really understand your sketch is created with several sketch blocks
if your blocks are completely constrained and closed sketches
by placing them on different planes you create a 3D sketch
if this 3D sketch intersects via your insertion of several blocks on offset planes
you end up with several closed contours
so SW won't find a single outline but several contours and SW doesn't like it at all
so no extrusion
who is moreover you can burst your blocks and then he agrees to extrude your assembly?
a visu will be welcome (screenshot)
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No, multiple 2D sketch blocks in a 2D sketch.
Hello
Is it possible to have the part file with your sketch? A drawing is sometimes better than a long speech... :-)
Hello
Have you checked for overlapping segments? It happens that a segment hides behind another identical one, in this case to check this you have to delete 1 segment, if it doesn 't disappear it's because there was another one on top, do that for each segment.
I know it's laborious but I don't have any other solutions.
Thomas
I can't give you my original file, I remade a "boat" model. But again, SolidWorks doesn't want to do an extrusion with combined blocks and sketching. They must be crushed. Unless there's a trick I don't know.
part2.sldprt
Indeed, the problem does not come from the fact that the sketch has an open outline. If you break up the blocks, it works without any problem.
I did not know that this was impossible.
Hello
With the COntour option selected and unchecking thin extrusion this works normally.
See attached file
Have a nice day
part2.sldprt
3 Likes
Great! Thank you very much ;-)
I did a test via attachment file
The one and only way I found was to make an offbeat shot of your sketch
Take the Convert tool on your new sketch and take all the segments on your basic sketch
once converted to this new sketch SW agrees to etrude
http://img839.imageshack.us/img839/6600/478n.png
hoping to have answered you as needed
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@ gt22, Mickael's solution is great.
1 Like
Thank you @ jmsavoyat
It's true that Mickael's solution is great
it didn't work for me the first time why will you know
so I opted for another solution a little + complicate
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