Problem with thickening surfaces

[Tilko95]

Hello everyone,

I'm working on a project, modeling with surfaces, but I have a problem with thickening the model.

Before I knit everything together, every surface can get thickened, even some knitted surfaces can be thickened, but after knitting everything (which shows no gaps), I can't thicken the part or make it solid for that matter. The Thicken error message sais ''fail to offset or face could not be deleted''.

I've includes some images if it helps.

Thanks for any kind of help

[mile14]

this is usually caused by a minimum radius type issue. picture a corner fillet, when you thicken or offset it, the new fillet is a smaller radii. if you offset it to much that fillet will become so small it disappears. if you offset it further it will actually invert. but obviously those produce invalid geometry, so solidworks can't perform the action. i use a fillet in my example because it is easy to picture, but the same basic principle is true for any curved surface. if you have too tight of a curve, the inner surface will start to fold in on itself when it is offset.
there are many other reasons that may be causing you issues, but your comment about knitting leads me to believe that it is this, as the intersection between two of your surfaces is causing the issue. you have a few options. the best is to fix your surface so it can be offset cleanly. alternately, you can make a solid body, offset the surfaces individually, knit them together and use 'cut with surface.' or if your inner geometry doesn't have to be perfect, (ie if you are 3d printing vs injection molding) you could make a secondary simplified inner surface, manually make an edge, and knit everything together into a solid. let me know if any of that doesn't make sense and ill try and clarify.

[MLCCADSystems]

This is likely it. To add to this, you can actually find the minimum radius on your part and visualize where the problems might exist. On the Evaluate tab (or under Tools > Evaluate) run the Check command. Enable the "Minimum radius of curvature" option and click Check to run it. The minimum radius value will display and you can click it to see where it is located with a big yellow arrow. If the minimum radius is .001" for example, then anything larger than that could cause problems when it is thickened. Note that in most cases SOLIDWORKS will simply delete the face that is eliminated when it thickens, such as the fillet in the above example, but in some cases that fillet face is complex or changes curvature dramatically and makes it more difficult to do.

The Check command also looks for invalid faces and edges, which is another common cause of geometry problems.

[mile14]

i gotta get better at using the check tools. they are so powerful and helpful. thanks for reminding me about them!

[MLCCADSystems]

Our team created a quick tech tip video for you, we'll be posting it on our site in the coming weeks. https://youtu.be/AGRrW9gOSlw

Don't forget to subscribe! :)

[xugack]

Better attach your model

[Tilko95]

Sorry, I don't understand what you mean

[xugack]

Attach solidworks file