Problem trying to extrude a sketch under a wanted angle

[Anonymous]

I faced this problem several times and always found a different workflow. But this time I simply can't find a way to do it. I used to work in Alias before moving to Fusion 360 and it had an option to switch from global to local axis, which was an extremely powerful tool. I would like to know if there is anything like this in Fusion. I need to extrude a profile under a wanted angle, but it keeps following the global axis. The idea is to extrude it as it would continue the cylinder above.

If there is anybody who knows about this issue, i would be very grateful!!!

[Beyondforce]

Hi @Anonymous,

If I understand you correctly, then you can just sketch a line with the angle that you need in the middle of the profile and use the Swipe command.

Cheers / Ben
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[jeff_strater · Accepted solution]

Hi @Anonymous,

Extrude in Fusion is defined to always be perpendicular to the plane the sketch is on, which is why you are seeing the results you are seeing.  I think that you probably should use a Sweep feature to get the results I think you want.

Here is a simple screencast showing how to do this with a model similar to yours.  Sweep needs two sketches:  A profile sketch and a path sketch.  The easiest way to specify the path in this case is to put a work axis through the cylinder.  Then, create a path sketch, and project the axis into the path sketch.  Then, use Sweep to create the feature you need:

Hope this helps,

Jeff

[Anonymous]

Thank you, Jeff! That solved exactly my problem. 🙂

But about the question I asked. Do you have any idea if there is an option to switch from global to local axis?


Thank you once again!

[TrippyLighting]

There is no such option when modeing with solids.

In the T-Spline envronment that can be done.

[Anonymous]

So bad there is no such option! I would like to see it in the solid modeling as well. I can remember how helpful it was in Alias. I will suggest Autodesk to add this option, maybe they will take it into account.


Thank you one more time Peter!

[TrippyLighting]

If you put it into the Idea station I will vote for it!

It would help reducing the numer of sketches neeed to model things!

[Anonymous]

I have already done it. Thanks!

[gwildgoose]

I don't know if this is the same problem but I am trying to extrude at a 45 deg. angle to the sketch plane. You can see the profile in EXAMPLE1 and you can see the result in EXAMPLE2. what I need is to extrude along the existing body, or 45 deg to the plane, not perpendicular to the plane.

Do I just have to rethink how to do these things?

[davebYYPCU]

You can extrude to, an object, 

create a new plane perpendicular to the body, Project the profile into that sketch, and extrude back to object,.

one of many ways to do it, (Loft with two profiles in that case) if you don't like Jeff's sweep option.

Might help...

[gwildgoose]

I was able to extrude the profile in the manner I needed it, Thank You, however the length seemed to be odd. I needed a 0.25" thickness, but I had to put .025" in the length dialog to get the proper thickness.When I entered the .025" distance the sweep would end up like 6" long, very strange and frustrating.

[davebYYPCU]

Distance along a sweep path is not a measurement like a dimension, but is the percentage of the Path itself, 

example, if the Path curve is 6" long, the Sweep needs 0.5 to make the sweep stop at 3" long.

However you are given the pull arrow to move that sweep distance by eye.

Might help....

[gwildgoose]

Ahhhh.....makes much more sense now. Now I will watch how long I make my
paths. I am in the habit of just dragging them out beyond the bodies so
their easy to click (bad habit I suppose) but this makes a huge difference
thank you very much.