Unable to choose sweep path from complex sketch

[dannyspitz]

I have a complex sketch that gives me control of a number dimensions that drive the path that i want to seep along however when i try to sweep a profile i cannot pick the path, Fusion chooses the path for me. 

on deleting all the lines that dont make up the path, the sweep will then not complete the full length of the path.

I'm rally starting to get annoyed with some fundemental gaps in the abilities on Fusion 360 that were available in programs like SDRC ideas 15 years ago! 

Link to the file here http://a360.co/2s3xVil

Any idea how to keep the controls in place and select the path i want? 

Regards, 

Danny 

[SaeedHamza]

Hi,

The first thing to mention is that the sweep needs the path to intersect the profile, I guess you know that

Now the second thing is that you can select multiple paths for a sweep as long as they are connected

Your problem here when you said " Fusion picks the path for me " is that the chain selection is enabled

turn it off and then you will be able to select everything separately

Regards

Saeed

 

[jeff_strater]

What path do you want the sweep to use?  It seems as if there are a lot of lines and paths in this sketch.

There are a couple things you can do, in addition to what @SaeedHamza suggests.  You can use Trim to remove portions of the curve that you don't need.  You can also convert the curves you don't want in the path to construction and/or add lines that trace over existing sketch lines/arcs.

The one thing you cannot do is to use a path that you want to branch that comes from the middle of a line or arc.  I suspect that is some of what you are running into in this design.  You can use the Break command to break sketch lines where they intersect other lines.

Here is a quick simple screencast that illustrates.  It uses Pipe instead of Sweep (because I'm too lazy on a Saturday to make another sketch and a profile), but the idea is the same.  Both sets of curves start out the same (1 line, one tangent arc that joins the line in the middle).  I show how using Break on the second set of curves will split the line into two and let you sweep along the line until it meets the arc, then along the arc.

Jeff

[dannyspitz]

Hi Jeff,

thanks for the reply. yes there are a lot of lines in the sketch but thats how i prefer to control the sketch for future modifications and to keep the sketch constrained. I get that one needs to break the lines but i feel that this is a major limitation, one of many, with Fusion 360 as it forces you to break control points. i'll have to re think how i build the sketch to deal with the limitations. or move to a high end CAD package where these issues would exist. i do wonder if inventor suffers from the same...

regards, 

Danny 

[TrippyLighting]

There might be other higher end CAD systems that might be a tad easier to work with for this kind of application (I've used a few of them throughout my career), but this is easy to do even in Fusion 360. The limitation here is rather your unfamiliarity with the proper sketching technique and all the tools available in Fusion 360 to help with this.

The first thing I am doing in the screencast is to turn all the sketch elements that don't actually belong to the sweep path into construction lines.

This is a technique as old as stone and existed before modern CAD systems were around.

Then it becomes obvious that there are 2 lines left that need to be broken and then the "other" halves also are changed into construction lines. That leaves a clean sweep path and you don't even have to un-check "Chain selection" even though that would also perfectly work in case for some reason you did not want to turn lines into construction lines.