Trying to create a face from offset

[Anonymous]

I'm a Fusion noob.  I've done some work successfully with this tool before, but have been frustrated more with the fact that it's so powerful.  I figure I'd try and stumble through trying different projects to get the hang of things...with, as I said some success.

Here is my dilemma:  I've inserted an SVG and created an offset expecting that offset to create a new face.  My intent is to extrude both the original SVG (to 0.5"), and the offset (as a new face) to a different thickness (0.75").  So I now have the SVG correctly inserted (I believe), an offset path (which looks connected all the way around), but no new face between the original SVG paths and the offset path.

https://a360.co/2IJGHoX

[etfrench]

Use the Divide and Conquer method to find the break in the profile:

1. Draw a line dividing the profile in two avoiding endpoints as this can lead to false closures.
2. Usually one of the sides will turn yellow indicating the boundary is closed.
3. Continue dividing the remaining sections in two until you find the errors.
4. The usual fix is to extend both sides of the error, then trim them.

In your file, you'll find the error in the upper left quadrant.

[Anonymous]

Are you saying to use the Line Tool (L), draw a line from, say the center of a segment of the offset path, to the center of another segment on the other side of the sketch (also along the offset path)? All I get when I do that is that the two segments I intersect turn purple and the vertices also turn purple.

[etfrench · Accepted solution]

Instructions didn't include starting a new sketch

[Anonymous]

That was awesome!  Thx!

[Anonymous]

Another thing I didn't realize how modal Fusion is...that the offset path was created as a separate sketch.  Once I selected the offset sketch, then I was able to slice it up as you directed.  Thanks again for the help!!

[etfrench]

@jeff_strater: Can you take a look at this sketch? The initial line drawn should have created a closed boundary on the bottom half.  The boundary was only closed when the final line was drawn.

[jeff_strater]

@etfrench It looks like @Anonymous took your advice and fixed the model.  I don't see the same problems that you did in your video.  It is likely a bug in the profile recognition algorithm in Fusion, though.

One other word of advice.  I notice that this sketch has a LOT of constraints (parallel/perpendicular/tangent).  When dealing with sketches like this, I suspect that those constraints are not adding any real design intent to your model.  I noticed that when I got rid of all of them (set your selection filter to only select geometric constraints, do a window select, and hit delete), the performance got much better.  When creating sketches like this, if you hold down CTRL (CMD on Mac), it disables the constraint inferencing behavior.  I wish there was a better way to turn this off, but that is all we have for now.

[etfrench]

Here's the bad file.

[Anonymous]

It appears that all the constraints appear with the creation of the offset.  Is there any way to avoid that happening?  I don't believe I really need any constraints.  My plan is to make a plaque from it and that geometry wont change...or is there some way to remove them?

I'm not exactly sure what you're talking about when changing filtering.  Is the holding control when selecting the paths to begin with, or is it something done during the offset dialog box?

[jeff_strater]

@Sdconant, you are right.  I did not look closely enough at the sketch.  Those constraints were created, not by the offset itself, but by breaking the offset, either implicitly or explicitly.

See the screencast below for more info, and also for how to delete those constraints.

[Anonymous]

Thanks Jeff!  I wouldn't say necessarily confusion...but this whole exercise has been extremely educational.  I recreated the file from scratch, looking for all the things you were talking about.  It seems better to leave the offset association there rather than deleting it and getting the loads of constraints added.   

Any idea why, when the offset is created, that the path is not closed, thus not creating a face in that gap?

You guys are amazing!  Many thanks!

[jeff_strater]

thanks for the original (bad) design, @etfrench.  Yes, there appear to be some profile recognition problems in this sketch.  Filed as FUS-41422, we'll take a look at it.  I can correct them all, manually, by deleting geometry and adding new lines, but that should not be necessary.

Jeff