What is the easiest way to get the angle shown in the picture to be flush to the outside of the square tubing, and not centered?
I typically offset lines in the sketch, but figured that there must be an easier way.
I assume from looking at your screen shot that your square tubing is centered on your sketch lines. If your angle just happens to be the same size as your tubing (both are 1x1) you could use the "Locate Profile" function in the Structural Member Property Manager.
Another option is to consider design intent from the beginning of your design by sketching to the outside of your structure. Then use the "Locate Profile" to position your tubing inside of your sketch along with your angles.
You may get more answers if you post this in the weldments section.
The easiest way would probably be to use Move/Copy Body to shift the angle to the outside.
What I think will work the best is just to sketch on the side of the previous strucural member, and ensure that the point is selected in the "Locate Profile"
One other option that may work, depending on your situation, would be to place the angle, as you show, and then expand the Structural Member function, find the profile sketch, edit it, place a sketch point where you want the profile to intersect the path sketch, then close the sketch, open the Structural Member function, click on the Locate Profile button at the bottom, and select this new sketch point.
That method sounds pretty involved, but it isn't that bad, and I've used it occasionally with good results when I needed an unusual insertion point. And the edit only affects the sketch in your part, not the original sketch in the .sldlfp file.
Glenn, hadn't considered an "one the fly" local insertion point.... I'll have to add that to my bag of tricks.
Thank you for the post. I've learned so much here on the forum, and it's good to hear when I've helped someone else or showed them something new.
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