Sketch not able to be extruded?

ronnie_melao

I have sketched the Survivor logo, and now I want to extrude it. However, when I try to extrude, I can't select the sketch or any of the parts of it. The error for the extrude is: "Extrude did not regenerate properly: Select face or sketch region to extrude."

 I am pretty sure this is a bug or something, because I have done three logos just like this one and they all ended up fine. Also, sometimes when I play around with the sketch and extrusions, it starts to work. However, there's always something wrong, and when I fix it, I still can't extrude.

Thanks for the help!

https://cad.onshape.com/documents/a1bb823ab4a1bac3c5b99441/w/8a25ffe53e15dc1e222c3cce/e/ff0acb0ae244e6625e3f730a

philip_thomas

Well - since i was called out . . . . . 

Sketches are actually very complex things to solve.
In addition to the constraints that a user can see, there are MANY others that are maintained and passed to the solver.
If the solver fails, you get this.
What increases the chances of the solver failing?

• Large numbers of entities - this sketch would definitely qualify.
• Large numbers of very small (including zero length) entities. When we built the Onshape sketcher, we said that we wanted to handle zero length better than anyone else (super flexible, especially for configurations). We succeeded! The cost is that there are sometimes multiple solutions where you have a zero length entity. Minimize their use.
• Multiple entities on top of one another (as it turns out, this is the bugaboo here).

Keep sketches simple.
Dont have multiple entities one on top of another

Now to fix your sketch - it was ONE entity.
This one.




Delete it. There is another one directly underneath it!

Now can do whatever



Have fun!

owen_sparks

Hmm.

(a) I agree there is something weird going on here.  Enclosed sketch regions are not being recognised as such.

In this copy of your doc I've projected a small part of your existing (unedited) geometry onto a new sketch and it extrudes just fine.  I'd imagine you could continue this as a quick workaround.

https://cad.onshape.com/documents/2ca7040decda2e92da2b71db/w/d89b4ce08f22935733505586/e/8d9f7c4832ff37805cb31f86

Hopefully an OS person will jump in and comment.  @philip_thomas maybe?

(b) Just for future help if you could cut 'n' paste the link directly from your browser that would be helpful.  The read only link from the share options gives the helper an extra step of having to search for the real doc so they can copy it and try to see whats up.

Cheers and happy CADing,

Owen S.

MBartlett21

owen_sparks said:

(b) Just for future help if you could cut 'n' past the link directly from your browser that would be helpful.  The read only link from the share options gives the helper an extra step of having to search for the real doc so they can copy it and try to see whats up.

@owen_sparks
He has got a link, and it works too!

owen_sparks

@mbartlett21

Hmm, that's weird, I could swear that "make a copy" button wasn't there a minute ago.

Sorry for the confusion.

O.S.

philip_thomas

Well - since i was called out . . . . . 

Sketches are actually very complex things to solve.
In addition to the constraints that a user can see, there are MANY others that are maintained and passed to the solver.
If the solver fails, you get this.
What increases the chances of the solver failing?

• Large numbers of entities - this sketch would definitely qualify.
• Large numbers of very small (including zero length) entities. When we built the Onshape sketcher, we said that we wanted to handle zero length better than anyone else (super flexible, especially for configurations). We succeeded! The cost is that there are sometimes multiple solutions where you have a zero length entity. Minimize their use.
• Multiple entities on top of one another (as it turns out, this is the bugaboo here).

Keep sketches simple.
Dont have multiple entities one on top of another

Now to fix your sketch - it was ONE entity.
This one.




Delete it. There is another one directly underneath it!

Now can do whatever



Have fun!

bruce_williams

@philip_thomas

Could you please list best practices?  How far would you break this up into separate sketches?  The 'masks' are complex but look symmetrical to each other.   Would that be best as sketch of one side only and mirror feature?  etcetera.    I do a lot with imported geometry and sketches can be really challenging (use & offset)...

philip_thomas

@bruce_williams

Keep sketches simple.
Dont have multiple entities one on top of another



I have no idea how long it took the OP to trace this - mind blowing.
If I was facing this challenge, i would have made as many sketches as there were logical elements (eg 1 per (non repeated) mask).
This might have been 8 sketches.

These recommendations are just to reduce the potential for a problem - as you can see, the solver is perfectly capable of handling this as one sketch.

bruce_williams

 
Onshape handles so much it is easy (at first) to make over-complicated sketches. Good to know best practice of breaking up into logical simpler ones.