"End Face Cannot Terminate Extrude Feature"?

SOLIDWORKS How To Questions
1

Hi all,

So in the attached part file, I’m looking to use “SKETCH Top Piece_Arc Wall” to make an extrusion offset from a curved surface. The error in the attached screenshot pops up when I try to do so.

Any ideas? All help is appreciated :slight_smile:!

Thanks in advance,



image.png
image.png

2

That error means that if you project the sketch onto the surface you selected, the sketch overlaps, outside the boundary of the surface, so the end condition is not really clear.

3

UPDATE MORNING 6/7:

I did some inspecting, and I’m now certain that the area of the selected surface totally encompasses that of the selected sketch.
This is the only cause of this error that I’m aware of, so I’m just not sure how to proceed…


P.S. I can’t find an option to edit the post, sorry, lol.

4

The reason it’s not working is because the surface selected for “Cut Up To” is not planar. It does work when using Blind, Through All, or Up To Surface for an end condition. It’s the offset that’s giving you trouble.

If you check the “Translate Surface” box it will approximate the offset but it may not be the desired result since the software doesn’t know which direction to measure. You could try creating an Offset Surface and cutting up to it.

With Solid Edge the solution is simple… :mrgreen:

5

You keep trying to do things the wrong way. I’m not sure what you’re trying to do, but maybe a lip? SW has a Lip and Groove function. Also, you might consider using a swept cut.

The reason this offset won’t work is that when you offset the face, the sketch doesn’t project within the offset.
image.png
Ways to proceed:

  • use the "translate surface
  • you’re probably meaning to include “reverse offset” to add a lip
    image.png
  • you could also eliminate the Cut Arc Wall feature and use a cut sweep instead


    Also, you’ve got a zero thickness corner in here. Dude, you need some help. Do you have a teacher?
    image.png
    You could do this more simply and it works:
  • extrude box
  • shell
  • add groove feature
  • create bottom of curved lip as an extruded surface
  • cut up to the surface


    Plus, I gotta say, you have to learn to use tangent arcs for sketching. Both of your arcs were totally unconstrained. Keep working at it. You’ll develop better instincts if you see how other people do some of this. Remember there are many ways to accomplish the same thing. Your job is to find the most efficient and most accurate way.
    image.png
6

UPDATE 6/8:

I tried selecting “Translate Surface” and got an error for zero-thickness geometry…

7

Yeah, I showed you where the zero thickness error is. Don’t do it that way. Use the technique I showed you with the shell feature. Fewer features, more correct geometry, better workflow, less messing around with sketches.

8

1.) When you say “extrude box”, do you mean to just create an extrusion from a rectangular shape?

2.) I’ve never used the shell or groove tools (I’m still pretty new to SW, to be honest).

3.) In what way would this cut be applied?


P.S. Thanks for being so helpful/thorough :slight_smile:!

9

[quote=Ballfreak10 post_id=7880 time=1623170494 user_id=162]
1.) When you say “extrude box”, do you mean to just create an extrusion from a rectangular shape?
[/quote]

I mean take your original sketch and extrude it like this:
[attachment=0]image.png[/attachment]

[quote]
2.) I’ve never used the shell or groove tools (I’m still pretty new to SW, to be honest).
[/quote]

Ok, movie time:



https://youtu.be/KTmY8burkDo

[quote]
3.) In what way would this cut be applied?



P.S. Thanks for being so helpful/thorough :slight_smile:!
[/quote]
hope that helps

10

[quote=matt post_id=7884 time=1623174276 user_id=49]
I mean take your original sketch and extrude it like this:

image.png







Ok, movie time:



https://youtu.be/KTmY8burkDo





hope that helps
[/quote]

WOW, this was so overly helpful I just…I don’t know what to say! Other than thank you, of course, haha!