My sketch includes blocks, and the sketch is fully defined, but when I try to extrude, it is forcing a thin feature. How do I close the sketch properly?
I do not want it to be a thin feature, but it won't let me deselect this. Help?
block sketchblock sketchblockdefinition thinfeature
i just did this with your file:
Try exploding the blocks and constraining the entities.
Can you click the "Selected Contours", click inside your shape, and then deselect the "Thin Feature" option?
What are these lines circled above? They look extra lines, either delete them or make sure they are construction.
My mistake the circled area in red on the right is not an extra line., only the two on the left.
Tom dunn wrote: What are these lines circled above? They look extra lines, either delete them or make sure they are construction. My mistake the circled area in red on the right is not an extra line., only the two on the left.
Tom dunn wrote:
I believe those are leader for the relation icons, not actual sketch lines.
Will SolidWorks allow you to Contour Select the area inside the geometry & blocks? Or won't it allow that either?
EDIT: My post was being moderated for some reason.
I believe this is something in the sketch, but without the file, we're just guessing.
Can you upload your file?
For assistance with this, see: How can I attach a file to a forum post?
One of Two things...
Thing One... = Double Lines - one on top of the other, no they will not propagate.
Thing Two.... = A small gap in the lines somewhere
Seems to default to Thin Feature when theres blocks in the sketch, just need to select the contour. Thats fast for anyone to test. Of course there could be something actually wrong with the OP's sketch too.
Sketch is screwed up, I use blocks a lot and they never ever are Thin Feature by default.... Unless it's the same as my original answer - Thing One - Thing Two
This is what I'm getting:
Maybe theres a better way to do this?
The fact that the entities of your contour do not all have the same weight indicates you have overlapping entities.
The three lighter gray lines are the BLOCK in the sketch, the same way OP is using blocks in their sketch. Blocks mixed with regular sketch lines.
My mistake, I have never used (or seen) blocks used in that manner. Sure enough, closing an open contour block with a separate sketch entity results in a default to a thin feature, which can be overcome by using ' Selected Contours'. I don't know if this is a feature or a bug.
Teemu Jääskeläinen - Sure there is a better way... You have overlapping lines - Explode the Block and select a line and delete it, if another line shows then that is your culprit, if not hit undo and check another line, till you get around the entire sketch..
Run "Check sketch for feature". Then select Boss Extrude from the drop down and hit Check. See what it says.
Did a little more testing- extruding the sketch as a thin feature results in separate bodies. SW is seeing the contours as separate even if they together make a closed contour. Interesting.
Thanks for your help, everyone. The part is attached.
I did find this link online, which suggests I can only do a "select contours" or create a separate sketch on top of the sketch with the blocks in it & then convert entities: https://www.reddit.com/r/SolidWorks/comments/3dn4qb/solidworks_block_thinks_it_has_an_open_contour/ Note: see "WorkDodge" comment:
"Option 1: Select contours. Option 2: Use the sketch that include a block as a reference sketch. Create a new sketch and convert entity of the reference sketch. I believe both of these accomplish what you're after. Both are acceptable solutions."
I also performed a Check Sketch for Feature command, and it claims the sketch is multiple disjoint closed, and that there is an open contour, but I can't find the open contour.
I tried to do an extruded boss using the Select Contours tool, but that was both tedious & it didn't work.
BUT! I then tried creating a separate sketch on top of my other sketch, performed a "Convert Entities" on the entire sketch, & that worked perfectly. This just seems like a ridiculous work around for something that should work in the original sketch. Does anyone know of any SPRs on this?
Teemu - I noticed that & it looks like it should work, but when I clicked the check mark on extruded feature, it gave me a rebuild error.
Thanks, Dan! I think that works for me!
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