How can I extrude surfaces between my sketch lines?

Aero_Modeler

Hi!

I've created a sketch of a top plate for a drone off of an existing design. However, when I attempted to extrude it into a part it was only extruding the sketch lines and the places I have circles and slots. Is there any way to essentially flip what is being extruded so that it is everything between the sketched lines, circles, and slots?  

matthew_stacy

@Aero_Modeler, I would strongly encourage you to sketch less.  A large complicated "masterpiece" sketch like you are working on can be challenging to troubleshoot and fix, like trying to find and close gaps as you are doing now.  Follow this example to see how you might break the model into small, bite-size pieces.  Step through the feature tree line by line to follow the progression.

I started with a single wedge comprising only an eighth of the final part.  The sketch is just a 45 degree triangle.  Then make another sketch defining just the slot.  Then mirror that part, resulting in a quarter wedge of the final part.  When ever possible pattern (or mirror) PARTS, or if necessary FEATURES.  Mirroring or patterning sketch entities is a last resort, and should be avoided whenever possible.

It can also be advantageous to create chamfers and fillets as parametric feature rather than sketching them in. 

In summary, sketch much less of the part and then mirror and/or pattern the part itself.  Make more, simple sketches that focus on a very small number of features.  Don't sketch geometry that can be more readily created with model features.  It's called parametric-feature-based CAD for a reason.  There are some great tutorials on these topics in the Onshape Learning Center.

eric_pesty

Your sketch isn't "closed". A closed area will show up shaded (like the slots and holes).

Aero_Modeler

  eric_pesty said:

Your sketch isn't "closed". A closed area will show up shaded (like the slots and holes).

Is there any way I can "close" the sketch? I essentially sketched one corner of the full plate and then mirrored across the front and right planes. I looked for a way to merge coincident points hoping that might close the sketch but didn't find anything.

matthew_stacy

@Aero_Modeler, I would strongly encourage you to sketch less.  A large complicated "masterpiece" sketch like you are working on can be challenging to troubleshoot and fix, like trying to find and close gaps as you are doing now.  Follow this example to see how you might break the model into small, bite-size pieces.  Step through the feature tree line by line to follow the progression.

I started with a single wedge comprising only an eighth of the final part.  The sketch is just a 45 degree triangle.  Then make another sketch defining just the slot.  Then mirror that part, resulting in a quarter wedge of the final part.  When ever possible pattern (or mirror) PARTS, or if necessary FEATURES.  Mirroring or patterning sketch entities is a last resort, and should be avoided whenever possible.

It can also be advantageous to create chamfers and fillets as parametric feature rather than sketching them in. 

In summary, sketch much less of the part and then mirror and/or pattern the part itself.  Make more, simple sketches that focus on a very small number of features.  Don't sketch geometry that can be more readily created with model features.  It's called parametric-feature-based CAD for a reason.  There are some great tutorials on these topics in the Onshape Learning Center.

martin_kopplow

To troubleshoot: "Show constraints" in the sketch dialog and see if there is a congruent condition wherever two curves meet. Alse, you have no closed face.

A "check curve gaps" tool, as is present with many other CAD systems, would sure help here. Is there maybe a custom script out there that can do that?

S1mon

@matthew_stacy
I largely agree with you, but there are a few exceptions to doing a lot of mirroring of features (as opposed to sketch elements) like this:

1. If there's any chance that some features which started out as being symmetric will need to be special cased later (say one of the drone arms needed a different mounting pattern because of a camera or some other feature), it can be more awkward to do that to the geometry instead of editing a sketch.
2. Capturing design intent could be harder. With the full sketch, I could easily dimension along the diagonals of this shape from one set of arm mounts to the other. I could add a bunch of mirror lines in the early sketches and put in the dimensions, but it might not be so clear what they were. Similarly, you've added the holes and the main corner chamfers later in the tree, but the clearance from the mounting holes to that chamfer might be an important distance which drives the overall size.

I think it's fair to say that some of the fillets on the complex sketch do not belong there and are much cleaner to add later. Lots of tangent relations tend to bog down the sketch solver and are more likely to cause issues.

matthew_stacy

A trick that I learned here in on of these forum threads is handy for tracking down gaps between sketch elements to close a profile.  Start with a profile with a grossly obvious gap to illustrate the method.

In a more typical scenario this gap would be too small to detect visually.  So let Onshape find it for you.  Sketch a line segment (arc, or other element/s) to split the profile into two isolated regions.

In this particular example the temporary sketch element that I added indicates that the portion of the profile below and to the right is closed.  The gap is in the upper left.  The intent is to isolate the discontinuity ... then fix it.