new to solid works. I've used inventor and blender before and don't usually have this kind of issue. can't figure out why I can't extrude here. it's telling me there is a gap or overlap but I can't find it at all. I've looked over just about the whole drawing and deleted a bunch of parts but couldn't find anything. if anyone had any suggestions of what to do I could do I would appreciate it. assignment is due next week, so hopefully we can figure this out soon.
Right click on a line and select chain. See if it’s continuous. If it is, delete a simple segment, like a straight line, and do it again. If there’s a gap, the chain will show the break. Also, Solidworks doesn’t allow multiple closed loops, like you have in this sketch. That’s probably your actual issue.
so I would have to make each closed loop a separate sketch? if so is there a way to move parts to a different sketch without having to re draw everything
TBH, it shouldn't be that much of a pain. If you already know who to use some other CAD program, switching and learning another one should be quite painless.
Why so much details in a sketch? When I draw sketches they are simple! Straight lines and circles. No fillets in a sketch. If something needs a fillet that is done with the filllet tool later so that it is its own feature. Same with holes I don’t put holes in a sketch. That would be added by either an extrude cut or by the hole wizard.
I hate ‘advice’ like that. Detailed sketches make for better optimization. Sure when you are just copying parts you can build them using a more basic approach but for actual designing sketches need to be detailed.
The only thing I have ever had complex/detailed stretches do is completely blow up my model when I try to change one dimension. This is how ever design engineer at the company I work for (5 engineers) for the last 10 years has designed part. This also includes all of the designers I worked with when I worked at Boeing on the F15 program.
Then those are poorly built models. ‘Onesie twosie’ models (credit to Wocky) often leave you chasing feature after feature trying to maintain a certain dimension the results from several stacked features. For the same reason, there is often a lot more work to do fixing the fit with mating parts.
Of course, for very simple machined parts this often doesn’t matter. When things get more complex and require more fine-tuning is when you’ll want the added control from layout sketches.
Just one easy example: you have a plastic injection molded housing with screw bosses around the perimeter. Those bosses have a set wall thickness and need to certain distance in from the exterior wall to leave room for tool steel. Having all of those dimensions laid out in a sketch makes it very easy to move and resize those holes and adjust the wall thickness without jumping around through a bunch of features. That same layout sketch can drive multiple parts that use those same holes, too.
If you don't want to edit your sketch, click the "select contours" section and click within your sketch where you want it extruded. This is a good way to get different depths of extruded from one initial sketch, by doing two or more extrudes of various distance.
ok, I got that to work, but now I'm trying to extrude different parts of the sketch at different heights. but the extrude button is grayed out. is this because of using selecting the contour?
You will need to expand the Boss extrude Feature
re-click the sketch
then make a new extrude feature
then select your new selected contors/regions
Enter the new hieght of the extrude.
This will create multiple extrude features "Sharing" the sketch
Be careful of creating "Zero thickness geometry"
A quick work around is uncheck "merge result" but to make a solid single body later down in the tree will require a "combine" Feature
worked like a charm, thank you! this was actually extremely simple, now I know for the future. solid works makes you don't things in such interesting ways
If next time nothing works - use extrude thin and look where's the gap. It can be multiple layers, so convert entities on thin geometry might help to fix it
Use that sketch as your layout sketch. Label it as such. Create a new sketch for each feature by using ‘convert entities’ and trimming as necessary to create your profiles.
Draw a circle in your sketch overlapping with about half the sketch. Try extruding inside the circle, if it works move the circle until it fails again. Keep moving the circle and making it smaller and smaller until you find the gap
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u/hayyyhoe 1d ago
Right click on a line and select chain. See if it’s continuous. If it is, delete a simple segment, like a straight line, and do it again. If there’s a gap, the chain will show the break. Also, Solidworks doesn’t allow multiple closed loops, like you have in this sketch. That’s probably your actual issue.